tormach P 770 Operator’s Guide

Download

PCNC 770 Manual

Part Number 32426 – 0412A

Questions or comments?

Using the Tormach

PCNC 770

Programmer’s and Operator’s Guide to the Personal CNC 770

Please email us at: info@tormach.com

iiContents

Using Tormach PCNC 770 ii 32426 Rev C1-1

Contents

1. Preface ............................................................................................. 1-1

1.1 Safety ............................................................................................................................... 1-1

1.1.1 Electrical Safety ................................................................................................................ 1-1

1.1.2 General Operating Safety .................................................................................................. 1-1

1.1.3 Safety Publications ........................................................................................................... 1-2

1.1.4 Safety Precautions............................................................................................................. 1-2

1.2 Personal CNC Concept ................................................................................................... 1-3

1.3 Performance Expectations .............................................................................................. 1-3

1.3.1 Cutting Ability .................................................................................................................. 1-3

1.3.2 Understanding Accuracy ................................................................................................... 1-4

1.3.3 Resolution, Accuracy and Repeatability of the PCNC ........................................................ 1-4

1.4 Scope and Intellectual Property...................................................................................... 1-4

1.5 Nomenclature .................................................................................................................. 1-5

2. Preparation ...................................................................................... 2-1

2.1 Planning for Your PCNC ................................................................................................ 2-1

2.1.1 Electrical Connection ........................................................................................................ 2-1

2.1.2 Location and Mounting ..................................................................................................... 2-1

2.1.3 Computer Mounting Arrangement ..................................................................................... 2-2

2.1.4 Learning and Training ....................................................................................................... 2-3

2.2 Receiving, Unpacking and Checking Shipment.............................................................. 2-4

2.2.1 Moving the Crate .............................................................................................................. 2-4

2.2.2 Uncrating and Inspection................................................................................................... 2-4

2.3 Mounting the PCNC ....................................................................................................... 2-4

2.3.1 Lifting onto Stand ............................................................................................................. 2-4

2.3.1.1 Lifting from Below ................................................................................................ 2-5

2.3.1.2 Lifting from Above ................................................................................................ 2-5

2.3.2 Fixing to Stand ................................................................................................................. 2-5

2.3.3 Installing central lubrication pump .................................................................................... 2-6

2.3.4 Accessories ....................................................................................................................... 2-6

2.4 Power to the PCNC ......................................................................................................... 2-6

2.5 Power for Machine Accessories ...................................................................................... 2-7

2.6 Tormach Machine Controller and Software Installation ............................................... 2-7

2.6.1 Control Computer ............................................................................................................. 2-7

2.6.2 Setting Up Your Controller ............................................................................................... 2-7

2.6.2.1 Positioning the Controller ....................................................................................... 2-7

2.6.2.2 Keyboard and Mouse ............................................................................................. 2-8

2.6.2.3 Display .................................................................................................................. 2-8

2.6.2.4 Speaker and Microphone Connections .................................................................... 2-8

2.6.2.5 Power Connections ................................................................................................ 2-8

2.6.3 Operating the Controller.................................................................................................... 2-8

2.6.3.1 About the Operating System ................................................................................... 2-8

2.6.3.2 Starting the controller ............................................................................................. 2-8

2.6.3.3 Stopping the controller ........................................................................................... 2-8

2.6.3.4 Mach3 License Installation ..................................................................................... 2-8

2.6.4 Machine Controller Maintenance and Configuration .......................................................... 2-9

2.6.4.1 Login and Software Installation .............................................................................. 2-9

iiContents

2.7 Connecting and Running the PCNC ............................................................................... 2-9

2.7.1 Main Switch and Control Panel ......................................................................................... 2-9

2.7.2 Changing the Spindle Speed Range ................................................................................. 2-11

2.7.3 Computer Control of the Spindle and Coolant .................................................................. 2-12

2.7.4 MDI for Entering G- and M-code Commands .................................................................. 2-13

2.7.5 Jogging the Axes............................................................................................................. 2-13

2.8 Summary ....................................................................................................................... 2-14

3. Making Your First Part .................................................................... 3-1

3.1 Coordinates ..................................................................................................................... 3-1

3.1.1 Referencing the Machine................................................................................................... 3-1

3.2 Loading a Demonstration Program ................................................................................ 3-2

3.3 Running the Demonstration Part-program .................................................................... 3-3

3.3.1 Part Material ..................................................................................................................... 3-3

3.3.2 Setting Work Offsets ......................................................................................................... 3-3

3.3.3 Cutting in Air.................................................................................................................... 3-4

3.3.4 Cutting the Actual Part ...................................................................................................... 3-4

3.3.5 Summary .......................................................................................................................... 3-5

4. Routes from an Idea to a Part ........................................................ 4-1

4.1 Controlling the PCNC ..................................................................................................... 4-1

4.2 Choosing the Appropriate Design Software ................................................................... 4-2

4.3 Software for CAD/CAM ................................................................................................. 4-2

4.3.1 3D CAD ........................................................................................................................... 4-3

4.3.2 2D CAD ........................................................................................................................... 4-3

4.3.3 CAM ................................................................................................................................ 4-4

4.3.4 Running the G-code .......................................................................................................... 4-6

4.3.5 CAD/CAM Systems.......................................................................................................... 4-6

4.4 Programming with Wizards ........................................................................................... 4-9

4.4.1 Machining Wizard Concept ............................................................................................... 4-9

4.4.1.1 Selecting and Running a Wizard ............................................................................. 4-9

4.4.1.2 Standard Wizard Features ....................................................................................... 4-9

4.4.1.3 G-code from a Wizard .......................................................................................... 4-10

4.4.1.4 Commercial Wizards ............................................................................................ 4-10

5. Machine Controls ............................................................................ 5-1

5.1 Machine Operation ......................................................................................................... 5-1

5.1.1 Operator’s Panel ............................................................................................................... 5-1

5.1.2 Tool Changing .................................................................................................................. 5-3

5.1.2.1 Tooling Strategy .................................................................................................... 5-3

5.1.2.2 Changing R8 Tools ................................................................................................ 5-3

5.1.2.3 Changing TTS Tools .............................................................................................. 5-4

5.1.3 Spindle Speed Ranges ....................................................................................................... 5-4

5.2 Screen Control Panels ..................................................................................................... 5-5

5.2.1 Using the Screens ............................................................................................................. 5-5

5.2.2 Families of Related Controls ............................................................................................. 5-5

5.2.2.1 Screen Switching Controls ..................................................................................... 5-5

5.2.2.2 Axis Control Family ............................................................................................... 5-6

5.2.2.3 Jogging Control Family .......................................................................................... 5-7

5.2.2.4 Spindle Speed Control Family ................................................................................ 5-8

5.2.2.5 Feed Control Family .............................................................................................. 5-9

5.2.2.6 Program Running Control Family ......................................................................... 5-10

5.2.2.7 Toolpath Control Family ...................................................................................... 5-11

Using Tormach PCNC 770 ii 32426 Rev C1-1

Contents

5.2.2.8 File Control Family .............................................................................................. 5-12

5.2.2.9 Work Offset and Tool Table Control Family ......................................................... 5-12

5.2.2.10 MDI and Teach Control Family ............................................................................ 5-12

5.2.2.11 Loop Control Family ............................................................................................ 5-13

5.2.2.12 Modes and Mode Alarm Control Family ............................................................... 5-13

5.2.2.13 Rotational Diameter Control Family ..................................................................... 5-13

5.2.2.14 Toolchange Position Control Family..................................................................... 5-14

5.2.2.15 Inhibits and Overrides Control Family .................................................................. 5-14

5.2.2.16 Feeds and Speeds Calculator ................................................................................ 5-14

5.2.2.17 Tapping Configuration Family.............................................................................. 5-15

5.2.2.18 Misc. Settings Control Family .............................................................................. 5-15

5.3 USB Jogging Pendants .................................................................................................. 5-16

5.3.1 Jog/Shuttle Controller ..................................................................................................... 5-16

5.3.2 Keypad Pendant .............................................................................................................. 5-16

6. Using Multiple Tools ....................................................................... 6-1

6.1 Offsets and Coordinate Systems ..................................................................................... 6-1

6.2 Tool Length Offsets and the Tool Table ......................................................................... 6-1

6.2.1 Example Operation of Multiple Tools ................................................................................ 6-1

6.2.1.1 To fill the table: ..................................................................................................... 6-2

6.2.1.2 Zeroing to work height ........................................................................................... 6-3

6.2.1.3 Using tool #2 ......................................................................................................... 6-4

6.2.1.4 Using other tools .................................................................................................... 6-4

6.2.1.5 Changing to a different work-piece ......................................................................... 6-4

6.2.2 How this multiple tooling setup works ............................................................................... 6-4

6.2.3 Programming, Buttons, or Direct Entry ............................................................................. 6-5

6.3 Alternative Methods Setting Up Tools ............................................................................ 6-6

6.3.1 Measuring techniques ....................................................................................................... 6-6

6.3.1.1 “Roll-Your-Own” Gauge Method ........................................................................... 6-7

6.3.1.2 Roller Gauge Method ............................................................................................. 6-7

6.3.1.3 Adjustable Parallel Method .................................................................................... 6-8

6.3.2 Comments on Accuracy .................................................................................................... 6-8

6.3.3 Working without the tool table .......................................................................................... 6-8

6.3.3.1 Direct Entry to Axis DRO ...................................................................................... 6-9

6.3.3.2 Using the Touch Buttons ........................................................................................ 6-9

6.3.4 Tool Table with General Tooling..................................................................................... 6-10

6.3.5 Tool table with the Tool Setter ........................................................................................ 6-10

6.4 Comments on Tool Offsets ............................................................................................ 6-10

6.5 Setting X and Y Offsets ................................................................................................. 6-11

6.5.1 By eye ............................................................................................................................ 6-11

6.5.2 With a Probe ................................................................................................................... 6-11

6.5.3 Measuring Off an Edge ................................................................................................... 6-11

6.5.4 Laser Centering Techniques ............................................................................................ 6-12

6.6 How Work Offsets work ............................................................................................... 6-12

6.7 Multiple Work Origins ................................................................................................. 6-14

6.7.1 G54 Work Offset ............................................................................................................ 6-14

6.7.2 Other Work Offsets ......................................................................................................... 6-14

6.8 Cutter Diameter Compensation .................................................................................... 6-15

6.8.1 CAD/CAM and Wizards ................................................................................................. 6-15

6.8.2 Concepts for Cutter Diameter/Radius Compensation........................................................ 6-15

6.8.3 Caveats in the Use of Cutter Compensation ..................................................................... 6-15

6.8.4 Examples of Operation .................................................................................................... 6-16

6.8.5 Look Ahead Issues .......................................................................................................... 6-19

6.8.6 Other Restrictions ........................................................................................................... 6-21

32426 Rev C1-1 iii Using Tormach PCNC 770

ivContents

6.8.7 Perspective on Cutter Compensation ............................................................................... 6-21

6.8.8 Resources for Debugging Cutter Compensation ............................................................... 6-21

7. Part-programming Language Reference ....................................... 7-1

7.1 Definitions ....................................................................................................................... 7-1

7.1.1 Control Software ............................................................................................................... 7-1

7.1.2 Linear Axes ...................................................................................................................... 7-1

7.1.3 Rotational Axes ................................................................................................................ 7-1

7.1.4 Scaling Input..................................................................................................................... 7-1

7.1.5 Controlled Point ................................................................................................................ 7-2

7.1.6 Coordinated Linear Motion ............................................................................................... 7-2

7.1.7 Feed Rate.......................................................................................................................... 7-2

7.1.8 Arc Motion ....................................................................................................................... 7-2

7.1.9 Coolant ............................................................................................................................. 7-3

7.1.10 Dwell................................................................................................................................ 7-3

7.1.11 Units ................................................................................................................................. 7-3

7.1.12 Current Position ................................................................................................................ 7-3

7.1.13 Selected Plane ................................................................................................................... 7-3

7.1.14 Tool Table ........................................................................................................................ 7-3

7.1.15 Path Control Modes .......................................................................................................... 7-3

7.2 Interpreter Interaction with Controls ............................................................................ 7-4

7.2.1 Feed and Speed Override controls ..................................................................................... 7-4

7.2.2 Block Delete Control ........................................................................................................ 7-4

7.2.3 Optional Program Stop Control ......................................................................................... 7-4

7.3 Tool File .......................................................................................................................... 7-4

7.4 Part-programs Language ................................................................................................ 7-4

7.4.1 Overview .......................................................................................................................... 7-4

7.4.2 Parameters ........................................................................................................................ 7-5

7.4.3 Coordinate Systems .......................................................................................................... 7-5

7.5 Formatting Code Lines (Block) ...................................................................................... 7-5

7.5.1 Line Number..................................................................................................................... 7-6

7.5.2 Subroutine Labels ............................................................................................................. 7-7

7.5.3 Word ................................................................................................................................ 7-7

7.5.3.1 Number.................................................................................................................. 7-7

7.5.3.2 Parameter Value ..................................................................................................... 7-7

7.5.3.3 Expressions and Binary Operations ........................................................................ 7-8

7.5.3.4 Unary Operation Value .......................................................................................... 7-8

7.5.4 Parameter Setting .............................................................................................................. 7-8

7.5.5 Comments and Messages .................................................................................................. 7-9

7.5.6 Item Repeats ..................................................................................................................... 7-9

7.5.7 Item Order ........................................................................................................................ 7-9

7.5.8 Commands and Machine Modes ...................................................................................... 7-10

7.6 Modal Groups ............................................................................................................... 7-10

7.7 G-codes .......................................................................................................................... 7-11

7.7.1 Rapid Linear Motion – G00............................................................................................. 7-11

7.7.2 Linear Motion at Feed Rate – G01 ................................................................................... 7-13

7.7.3 Arc at Feed Rate – G02 and G03 ..................................................................................... 7-14

7.7.3.1 Radius Format Arc ............................................................................................... 7-15

7.7.3.2 Center Format Arc ............................................................................................... 7-16

7.7.4 Dwell – G04 ................................................................................................................... 7-17

7.7.5 Coordinate System Data Tool and Work Offset Tables – G10 .......................................... 7-17

7.7.6 Clockwise/Counterclockwise Circular Pocket – G12 and G13 .......................................... 7-18

7.7.7 Exit and Enter Polar Mode – G15 and G16 ...................................................................... 7-18

7.7.8 Plane Selection – G17, G18 and G19 ............................................................................... 7-19

7.7.9 Length Units – G20 and G21 ........................................................................................... 7-19

7.7.10 Return to Home – G28 and G30 ...................................................................................... 7-20

Using Tormach PCNC 770 iv 32426 Rev C1-1

Contents

7.7.11 Reference Axes – G28.1.................................................................................................. 7-20

7.7.12 Straight Probe – G31 ....................................................................................................... 7-20

7.7.12.1 Straight Probe Command ..................................................................................... 7-20

7.7.12.2 Using the Straight Probe Command ...................................................................... 7-21

7.7.12.3 Example Code ...................................................................................................... 7-21

7.7.13 Cutter Radius Compensation – G40, G41 and G42 .......................................................... 7-22

7.7.14 Tool Length Offsets – G43, G44 and G49 ....................................................................... 7-23

7.7.15 Scale Factors – G50 and G51 .......................................................................................... 7-23

7.7.16 Temporary Coordinate System Offset – G52 ................................................................... 7-23

7.7.17 Move in Absolute Coordinates – G53 .............................................................................. 7-24

7.7.18 Select Work Offset Coordinate System – G54 to G59 & G59 P~...................................... 7-24

7.7.19 Set Path Control Mode – G61 and G64 ............................................................................ 7-25

7.7.20 Coordinate system rotation – G68 and G69 ...................................................................... 7-25

7.7.21 Canned Cycle – High Speed Peck Drill – G73 ................................................................. 7-25

7.7.22 Cancel Modal Motion – G80 ........................................................................................... 7-26

7.7.23 Canned Cycles – G81 to G89 .......................................................................................... 7-26

7.7.23.1 Preliminary and In-Between Motion ..................................................................... 7-27

7.7.23.2 G81 Cycle ............................................................................................................ 7-28

7.7.23.3 G82 Cycle ............................................................................................................ 7-29

7.7.23.4 G83 Cycle ............................................................................................................ 7-29

7.7.23.5 G85 Cycle ............................................................................................................ 7-30

7.7.23.6 G86 Cycle ............................................................................................................ 7-30

7.7.23.7 G88 Cycle ............................................................................................................ 7-30

7.7.23.8 G89 Cycle ............................................................................................................ 7-30

7.7.24 Distance Mode – G90 and G91 ........................................................................................ 7-30

7.7.25 G92 Offsets – G92, G92.1, G92.2 and G92.3 ................................................................... 7-31

7.7.26 Feed Rate Mode – G93, G94 and G95 ............................................................................. 7-31

7.7.27 Canned Cycle Return Level – G98 and G99 .................................................................... 7-32

7.8 Built-in M-codes ........................................................................................................... 7-32

7.8.1 Program Stopping and Ending – M0, M1, M2 and M30 ................................................... 7-32

7.8.2 Spindle Control – M3, M4 and M5 .................................................................................. 7-33

7.8.3 Tool change – M6 ........................................................................................................... 7-33

7.8.4 Coolant Control – M7, M8 and M9 ................................................................................. 7-34

7.8.5 Re-run from First Line – M47 ......................................................................................... 7-34

7.8.6 Override Control – M48 and M49 ................................................................................... 7-34

7.8.7 Call Subroutine – M98 .................................................................................................... 7-34

7.8.8 Return from Subroutine – M99 ........................................................................................ 7-34

7.9 Application Defined M-codes ........................................................................................ 7-34

7.9.1 Self-reversing Tapping Cycles......................................................................................... 7-34

7.9.2 Goto Toolchange Position – M998 .................................................................................. 7-35

7.9.3 User Defined M-codes .................................................................................................... 7-35

7.10 Other Input Codes ........................................................................................................ 7-35

7.10.1 Feed Rate – F .................................................................................................................. 7-35

7.10.2 Spindle Speed – S ........................................................................................................... 7-36

7.10.3 Select Tool – T ............................................................................................................... 7-36

7.11 Order of Execution ....................................................................................................... 7-36

7.12 Error Handling ............................................................................................................. 7-37

8. Machine Upgrades and Configuration........................................... 8-1

8.1 Fourth Axis – Rotary Table ............................................................................................ 8-1

8.1.1 Installing the Electronics ................................................................................................... 8-1

8.1.2 Utilizing the Fourth Axis ................................................................................................... 8-1

8.1.2.1 Referencing and Zeroing the Fourth Axis ............................................................... 8-1

8.1.2.2 Diameter Compensation Feature ............................................................................. 8-1

8.1.3 Fourth Axis Applications .................................................................................................. 8-1

8.1.3.1 Engraving on a Periphery of a Cylinder .................................................................. 8-2

32426 Rev C1-1 v Using Tormach PCNC 770

viContents

8.1.3.2 Gear Cutting .......................................................................................................... 8-3

8.2 Probes (Active and Passive) and Tool Setters ................................................................. 8-3

8.2.1 Introduction to Uses of Probes and Tool Setters ................................................................. 8-3

8.2.2 Probing for Work/Tool Setting .......................................................................................... 8-4

8.2.2.1 Simple X/Y Probing ............................................................................................... 8-5

8.2.2.2 Z Probing ............................................................................................................... 8-7

8.2.2.3 Comprehensive X/Y Probing .................................................................................. 8-9

8.2.2.4 Probe Calibration ................................................................................................. 8-12

8.2.3 Digitizing parts from a model or for reverse engineering .................................................. 8-13

8.2.4 The Probe Electrical Interface ......................................................................................... 8-13

8.2.5 Other .............................................................................................................................. 8-14

8.3 Auto-reverse tapping .................................................................................................... 8-14

9. Specifications, Customization and Troubleshooting ................... 9-1

9.1 Intended Use Statement .................................................................................................. 9-1

9.2 Support............................................................................................................................ 9-1

• This manual – ALWAYS the first place to check!! ................................................. 9-1

• Related documents found at: http://www.tormach.com/documents.html .................. 9-1

• Our website at: www.tormach.com ......................................................................... 9-1

• Email to: info@tormach.com .................................................................................. 9-1

• Telephone Tormach at: 608-849-8381 .................................................................... 9-1

• Fax Tormach at: 209-885-4534............................................................................... 9-1

9.3 Outside of the Scope of Intended Use ............................................................................. 9-1

9.4 Specifications................................................................................................................... 9-2

9.4.1 Mechanical ....................................................................................................................... 9-2

9.4.2 Electrical .......................................................................................................................... 9-2

9.4.3 System .............................................................................................................................. 9-3

9.4.4 Options ............................................................................................................................. 9-3

9.5 Maintenance .................................................................................................................... 9-3

9.5.1 Foreword – Understanding Machine Design ...................................................................... 9-3

9.5.1.1 Machine Stiffness................................................................................................... 9-3

9.5.1.2 Backlash, Friction, and Lost Motion ....................................................................... 9-4

9.5.1.3 Factors Combine .................................................................................................... 9-4

9.5.1.4 Adjusting Geometry ............................................................................................... 9-4

9.5.1.5 Achieving Accuracy in Machining.......................................................................... 9-5

9.5.2 Protecting from Rust ......................................................................................................... 9-5

9.5.3 Gibs, Dovetail Slideways and Lubrication ......................................................................... 9-5

9.5.4 Way Covers ...................................................................................................................... 9-6

9.5.5 Axis Gib Adjustment ........................................................................................................ 9-6

9.5.6 Adjusting Ballscrew Preload ............................................................................................. 9-8

9.5.6.1 Understanding Preloaded Angular Contact Bearings ............................................... 9-9

9.5.6.2 Making the Adjustment .......................................................................................... 9-9

9.5.7 Adjusting Mating Surfaces .............................................................................................. 9-11

9.5.8 Speed Calibration............................................................................................................ 9-11

9.5.9 Using a Non-standard Printer Port ................................................................................... 9-13

9.5.10 Defining Your Own Sizes for Step-mode Jogging ............................................................ 9-14

9.5.11 Defining Probe Type ....................................................................................................... 9-15

9.5.12 Enabling 4th axis homing ................................................................................................ 9-15

9.5.13 Configuring to start in Metric units .................................................................................. 9-15

9.6 Troubleshooting ............................................................................................................ 9-16

9.6.1 Overview ........................................................................................................................ 9-16

9.6.2 Philosophy of Troubleshooting ........................................................................................ 9-16

9.6.3 Tips and Tools for Troubleshooting (Equipment and Procedures)..................................... 9-19

9.6.3.1 Safety .................................................................................................................. 9-19

9.6.3.2 Tip on Computer Diagnostics ............................................................................... 9-19

Using Tormach PCNC 770 vi 32426 Rev C1-1

Contents

9.6.3.3 Tools ................................................................................................................... 9-20

9.6.3.4 Using the digital multi meter for electrical tests .................................................... 9-20

9.6.3.5 Contacting Technical Support............................................................................... 9-21

9.6.4 Frequently Found Problems (Repeat Offenders) .............................................................. 9-21

9.6.4.1 Loose Wires ......................................................................................................... 9-21

9.6.4.2 Wire Hairs ........................................................................................................... 9-22

9.6.4.3 Poor Cable Connections ....................................................................................... 9-22

9.6.4.4 Software Restart ................................................................................................... 9-22

9.6.4.5 Sensors (on the PCNC770 the End of Travel Sensors aka Limit Switches) ............ 9-22

9.6.4.6 Flaky Computer ................................................................................................... 9-22

9.6.4.7 Control Software license not installed ................................................................... 9-22

9.6.4.8 Unexplained stop or limit switch error while running ............................................ 9-23

9.6.5 Which sub-system should I troubleshoot .......................................................................... 9-23

9.6.5.1 Computer and Coolant Power Distribution Sub-system ......................................... 9-24

9.6.5.2 Control Power Sub-system Overview ................................................................... 9-26

9.6.5.3 9.6.5.3 Computer Control Communication Sub-Section ........................................ 9-29

9.6.5.4 Axes Drive Sub-system ........................................................................................ 9-31

9.6.5.5 Spindle Drive Sub-system .................................................................................... 9-46

9.7 Mechanical maintenance.............................................................................................. 9-56

9.8 Electrical maintenance .................................................................................................. 9-56

9.9 Preparation for Transport ............................................................................................ 9-57

9.10 Disassembly for Transport ........................................................................................... 9-57

10. Appendices .................................................................................... 10-1

10.1 Appendix 1 – Not Used.................................................................................................. 10-1

10.2 Appendix 2 – Exploded Parts Views ............................................................................. 10-1

10.3 Appendix 3 - Use of a Standard PC to control PCNC ................................................ 10-14

10.3.1 Choice of computer ....................................................................................................... 10-14

10.3.2 Optimizing the Windows Installation............................................................................. 10-15

10.3.3 Installing the Control Software ...................................................................................... 10-15

10.3.3.1 Installing .............................................................................................................10-15

10.3.3.2 Vital Re-boot ......................................................................................................10-16

10.3.3.3 Testing the Installation ........................................................................................10-16

10.3.3.4 DriverTest After a Software Crash .......................................................................10-17

10.3.3.5 Manual Driver Installation and Un-installation.....................................................10-17

10.3.4 Optimization of Windows XP ....................................................................................... 10-18

10.3.4.1 Remove Unnecessary Services and Startup Programs...........................................10-19

10.3.4.2 Disable Power Management ................................................................................10-19

10.3.4.3 Disable sound card ..............................................................................................10-19

10.3.4.4 Disable Automatic Updates .................................................................................10-20

10.3.4.5 Set Computer to Standard PC not ACPI PC .........................................................10-20

10.4 Revision history ........................................................................................................... 10-21

11. Index .................................................................................................. 23

32426 Rev C1-1 vii Using Tormach PCNC 770

1. Preface

1.1 Safety

Any machine tool is potentially dangerous. Computer controlled machines are potentially more dangerous than manual ones because, for example, a computer is quite prepared to plunge a 3" diameter facing cutter at 50 inches per minute into a block of high-carbon steel or to mill the clamps off your table.

1.1.1 Electrical Safety

The PCNC 770 can deliver sufficient force to break brittle tools, to crush bones and to tear flesh.

This manual tries to give you guidance on safety precautions and techniques but because we do not know the details of your workshop or other local conditions we can accept no responsibility for the performance of the machine or any damage or injury caused by its use. It is your responsibility to ensure that you understand the implications of what you are doing and to comply with any legislation and codes of practice applicable to your country or state.

Power Input: The PCNC 770 supply is 115 VAC. A circuit rated at 20 amps is required. This power supply can provide lethal electrical shocks. The power input should be unplugged before working in the electrical cabinet.

Preface

Grounding: The power input must be grounded. During installation it is not enough to assume that the ground line of a wall outlet is properly grounded. Check continuity between the machine frame and true earth ground (water pipe or similar) to ensure a good ground connection.

A Ground Fault Interrupt or GFI (i.e., Residual Current Circuit Breaker or RCCB in Europe) outlet is not recommended as the filters in the spindle drive can give leakage currents sufficient to trip a normal 30 mA breaker.

Electrical Panel: NEVER operate the machine tool with the cabinet door open. NEVER allow a coolant pump to operate with the cabinet door open. DO NOT allow the coolant system to flow coolant directly at the cabinet door seal or on the operator console controls. Neither the cabinet door seal nor the electrical controls are sealed against liquids.

Retained Electrical Power: Electronic devices within the electrical cabinet may retain dangerous electrical voltages after the power has been removed.

Electrical Service: Certain service and troubleshooting operations require access to the electrical cabinet while the electrical power is on. Only qualified electrical technicians should perform such operations.

1.1.2 General Operating Safety

Safe operation of the machine depends on its proper use and the precautions taken by each operator.

Read and understand this manual. Be certain every operator understands the operation and safety requirements of this machine before operating the machine.

Always wear safety glasses and safety shoes. Always stop the spindle and check to ensure the CNC control is in the stop mode before

changing or adjusting the belt/pulley position, tool or work piece.

32426 Rev C1-1 1-1 Using Tormach PCNC 770

Preface

Never wear rings, watches, gloves, long sleeves, neckties, jewelry or other loose items when operating or working around the machine. Long hair should be bound or kept under a hat.

Use adequate safeguarding around the operating envelope. It is the responsibility of the employer to provide and ensure point of operation safeguarding per OSHA 1910.212 – Milling Machine.

1.1.3

1.1.4

Safety Publications

Tormach recommends the following publications for assistance in enhancing the safe use of this machine.

• Safety Requirements for The Construction, Care and Use of Drilling, Milling and Boring

Machines (ANSI B11.8-1983). Available from The American National Standards Institute, 1430 Broadway, New York, New York 10018.

• Concepts and Techniques of Machine Safeguarding (OSHA Publication Number 3067).

Available from The Publication Office – O.S.H.A., U.S. Department of Labor, 200 Constitution Avenue, NW, Washington, DC 20210.

Safety Precautions

1. Do not run this machine without knowing the function of every control key, button, knob or

handle. Refer to the manual or contact Tormach if any function is not understood.

2. Protect your eyes. Wear approved safety glasses (with side shields) at all times. You should

never use compressed air to remove chips or to clean the machine. An air blast will often launch a metal chip into a place it should not be.

3. Ear protection should be used on any operations that exceed sound levels of 85dBa.

4. Avoid moving parts. Before operating this machine remove all jewellery including watches

and rings, neckties and any loose-fitting clothing.

5. Keep your hair away from moving parts.

6. Take off gloves before you operate the machine. Gloves are easily caught in moving parts

or cutting tools.

7. Never operate with unbalanced tooling or spindle fixtures.

8. Remove all tools (wrenches, chuck keys, etc.) from the spindle and machine surface before

you begin. Loose items can become dangerous flying projectiles.

9. Use adequate work clamping. Do not allow your work piece to become a projectile.

10. Never operate a milling machine after consuming alcoholic beverages or taking strong

medication.

11. Protect your hands. Stop the machine spindle and ensure that the computer control is

stopped before you:

• Change tools;

• Change parts or adjust the work piece;

• Change the belt/pulley position;

• Clear away chips, oil or coolant – always use a chip scraper or brush;

• Make an adjustment to the part, fixture, coolant nozzle or take measurements;

• Remove protective shields or safeguards – do not reach for the part, tool or fixture around

a guard.

12. Keep work area well lit. Ask for additional light if needed.

13. Keep the computer area clear of clutter. Recognize that machine motion can occur when

certain keys are pressed. Objects falling on the keyboard can result in unexpected motion.

14. Avoid getting pinched in places where the table, saddle or spindle head create “pinch

points” while in motion.

Using Tormach PCNC 770 1-2 32426 Rev C1-1

15. Securely clamp the work piece in a vise, on the table or in the fixture. Use proper holding

clamping attachments and position them clear of the toolpath. Be aware of larger pieces that will be cut free during operations – loose parts can become projectiles.

16. Always use proper feeds and speeds, as well as depth and width of cut, to prevent tool

breakage.

17. Use proper cutting tools for the job.

18. Do not use dull or damaged cutting tools. They break easily and become dangerous

projectiles. Never use longer or larger tools than necessary.

19. Chips and dust from certain materials (e.g., magnesium) can be flammable. Fine dust from

normally non-flammable materials can be flammable or even explosive.

20. Chips and dust from certain materials can be toxic. Vapours from certain overheated

materials can be toxic. Always check a Materials Safety Data Sheet (MSDS) of suspect materials. Refuse machining work requests of unknown materials.

21. If you are in any doubt you must seek guidance from a professionally qualified expert

rather than risk injury to yourself or to others.

1.2 Personal CNC Concept

The PCNC 770 is a machine tool intended to make CNC machining more personal. As with the evolution of personal computers, the evolution of personal CNC alters the paradigm of what a machine tool is about. We aim for a machine tool so affordable that anyone can have one.

We feel that the work of engineers, inventors, technicians, hobbyists, educators and others will be enhanced when they have access to CNC machinery. In education, each student can run his own machine instead of waiting in line when the machine tool costs less than 20% of a small machining center. In R & D, turn-around on prototype design takes minutes instead of days when a machine is “at the ready” and on site. In general engineering, designs sent to the production machine shop are improved when the design engineer has been more involved in the prototype creation.

Preface

The PCNC offers the precision of a production machine but with cost/performance optimized for short run operation.

1.3 Performance Expectations

1.3.1 Cutting Ability

The machine is capable of cutting most materials at or near their recommended feeds and speeds. For example, for fast metal removal on 6061 aluminium we will run a 1/2" diameter 2 flute cutter at around 18 IPM (inches per minute) and 3000 RPM, using a full 1/2" depth of cut.; that is a pretty good volumetric rate of metal removal so it is essential to clear chips with a flood coolant. We will run smaller cutters when we are not trying to remove large amounts in a hurry. For most aluminium work we use 3/8". The example above, using a 1/2" cutter, results in a surface speed of 390 SFM (surface feed per minute), a 1/4" cutter needs 6000 RPM to get the same surface speed, well within the performance envelope of the machine.

Cutting steel and iron needs a lower volumetric rate, thus slower feed and speed. The PCNC will run best using smaller cutters when working with tougher materials. For example, the general machining recommendation for some oil hardening steels is 30 SFM. Doing this with a ¾" end mill, the surface speed calculation indicates 150 RPM, but that is below the minimum spindle speed of the PCNC 770 and certainly at minimum speed limited power is available. By switching to a 1/4" end mill the recommended spindle speed becomes 460 RPM, well within the capability of the PCNC. By keeping close to general machining recommendations your tools will last longer and you will have a better cut.

32426 Rev C1-1 1-3 Using Tormach PCNC 770

Preface

1.3.2 Understanding Accuracy

While a machine tool may seem absolutely rigid, the truth of the matter is that everything has some elasticity. Related to elasticity is the compressibility of components such as ball nuts and bearings. Preloading of bearings and ballscrews can remove the physical open space between moving parts, but the technique cannot eliminate compressibility. The key to achieving maximum accuracy is understanding and controlling the magnitude and direction of forces. Maximum accuracy is achieved when the forces are minimized, as occurs in a finishing cut. Maximum repeatability is achieved when the forces are repeatable, both in magnitude and direction.

1.3.3 Resolution, Accuracy and Repeatability of the PCNC

The minimum discrete position move is 0.0001", this is the resolution of motion. Machine accuracy is closely related to ballscrew accuracy. Our ballscrews are accurate to 0.0006" per foot, but considering all the other factors that come into play, we prefer to keep accuracy expectations to 0.0013" per foot. Repeatability will be better than 0.001" per foot.

Machining is a mix of science, skill and art. The caveat in stating accuracy and repeatability is that these factors depend on the techniques used by the machinist. A skilled machinist can often deliver accuracy that exceeds the accuracy specified by the machine builder, while an inexperienced machinist may have difficulty delivering the expected accuracy. With this understanding, we cannot tell you what accuracy you will be able to achieve in your own work. Nevertheless, the accuracy specified by a machine builder remains an important reference point.

1.4 Scope and Intellectual Property

This document is intended to provide sufficient information and detail to allow you to install, setup and use your Tormach mill. It assumes that you have appropriate experience and/or access to training for any Computer Aided Design/Manufacture software that you intend to use with the machine. This document also assumes familiarity with typical Microsoft Windows applications programs as the control software for the PCNC runs under the Windows operating system.

Tormach LLC is dedicated to continual improvement of its products, so suggestions for enhancements, corrections and clarifications will be gratefully received.

Tormach LLC, Art Fenerty and John Prentice assert their right to be identified as the authors of this work. This work is copyrighted by Tormach LLC. The right to make copies of this manual is granted solely for the purpose of training courses related to, evaluation of and/or use of the PCNC. It is not permitted, under this right, for third parties to charge for copies of this manual beyond the cost of printing.

Every effort has been made to make this manual as complete and as accurate as possible but no warranty or fitness is claimed or implied. All information provided is on an “as is” basis. The authors, publisher, and Tormach LLC shall not have any liability for, or responsibility to, any person or entity for any reason for any loss or damage arising from the information contained in this manual.

Tormach, PCNC1100 Personal CNC, PCNC770 Personal CNC, and Tormach Tooling System are registered trademarks of Tormach. Windows XP and Windows 7 are registered trademarks of Microsoft Corporation. If other trademarks are used in this manual, but not acknowledged, please notify Tormach LLC so this can be remedied in subsequent editions.

Tormach milling machines and accessories are covered by one or more of the following U.S. Patents: 7,386,362, D606,568, D612,406, D621,859 and Patent(s) Pending.

Using Tormach PCNC 770 1-4 32426 Rev C1-1

1.5 Nomenclature

This manual uses the following typographical nomenclature:

Software control

Refers to a Control Software “soft” control. (i.e., a Windows control on the PC screen).

Hardware Control

Refers to a physical button or switch on the Operator’s Panel of the machine.

G-code (e.g., G01X34.8)

Used to show G-code programs.

Key name (e.g., Enter)

Tells you to press the indicated key.

Preface

32426 Rev C1-1 1-5 Using Tormach PCNC 770

2. Preparation

This chapter describes the work required to unpack and to commission the

hardware and software of the PCNC.

It contains a lot of detail but can be completed in one or two hours by a person

familiar with CNC machines. Enough detail is given here so that a beginner

should be successful but some users may prefer to arrange for a machine tool

expert to do this work.

If your machine has already been set-up then you can skip this chapter

2.1 Planning for Your PCNC

2.1.1 Electrical Connection

The PCNC 770 is shipped with a 3-wire cord and no electrical plug. There are several different NEMA (National Electric Manufacturers Association) and non-NEMA plug patterns that can be used. Straight blade patterns are common in household use; twist-lock patterns are more common in industrial locations. Power required is 115 to 130 VAC, 50 or 60 Hz. Continuous current is below 15 amps, but a 20 amp breaker or slow blow fuse is recommended.

Preparation

The power input must be grounded. During installation it is not enough to assume that the ground line of a wall outlet is properly grounded. Check continuity between the machine frame and true earth ground (water pipe or similar) to ensure a good ground connection.

2.1.2 Location and Mounting

People experienced with CNC machining will undoubtedly have ideas as to how they want to setup their PCNC (figure 2.1). While the machine can be configured in many different ways, there are a few limitations. Many fully enclosed vertical machining centers incorporate high volume coolant systems that make the inside of the machine look like the inside of a dishwasher. The PCNC electrical cabinet and operator console should not be exposed to such conditions. Additionally, there should never be an enclosure or accessory that limits access to the emergency stop. Please keep these limitations in mind when you plan your configuration.

If your prior experience is limited to manual mills then keep in mind that, as CNC dramatically extends your machining capabilities, it will also change the way you cut metal. When your metal cutting is done by turning handles on a manual mill your operations will generally be limited to cleaning up a surface, drilling a hole pattern or cutting to a dimensional outline. With manual milling many people are accustom to dry cutting, clearing chips with a small brush as they go.

Figure 2.1 – An example mounting on stand

32426 Rev C1-1 2-1 Using Tormach PCNC 770

Preparation

With CNC you have a whole new world open to you. In many cases you may turn the majority of the stock into chips, cutting a shape out of a solid block of metal the way Michelangelo would cut a sculpture from a block of marble. Unless you are limiting yourself to cutting cast iron, wood, printed circuit boards or certain other materials, you will probably want a coolant system on your machine. Mist coolant can be effective for keeping your cutting tools cool, but it does little for clearing chips. Flood coolant will cool the cutting tools while clearing chips, but is more challenging to contain. We strongly recommend that you plan your setup with a full motion tray and splash guards, such that coolant will be captured as it overflows the machine table within the full operating envelope of the machine.

Another reason to use a full motion tray is to reserve the space that will be required when the machine moves. If you use a narrow drip tray or none at all, you should plan for full machine motion plus some human space when you place the machine in your workshop. You do not want to locate it where you can create crush points between the machine table and a wall. When in operation, the X, Y and Z motions will not stop when they hit something. The machine will move with hundreds of pounds of force, enough to punch through a wall, tip over the machine or crush someone in the way.

Machine safety is the responsibility of the operator. This includes all aspects of safety: setup, location, operation, security and all other factors that involve safety.

The PCNC 770 requires a minimum plan area of 60" wide by 40" deep. This gives clearance for the full motion of the table and for minimal access for cabling etc. The overall height required is 73" assuming that it is installed with the table at a working height of 36".

Tormach offers a suitable heavy duty stand with built in storage for tooling and the control computer. It is also available with a coolant sub-system.

You should choose a well lit location and provide any additional task-lighting to make it easy to setup work on the table.

Over time you will find that you accumulate a range of tools and tool holders so you should allocate space for storage of these near the machine. A rack with numbered slots is convenient to avoid errors when doing tool changes during a job.

USB jogging

pendant

LCD

Screen

Keyboard

Personal computer

Figure 2.2 Computor and Display

2.1.3 Computer Mounting Arrangement

Keep the computer in a clean location, preferably inside the stand of the milling machine. Resist the temptation to expose the computer in any way. Providing access to floppy disks, CDs

Using Tormach PCNC 770 2-2 32426 Rev C1-1

Preparation

or direct computer controls will also open the computer to contamination and risk. Tormach offers accessories that will allow you to operate the system without exposing your computer.

While there are many possible configurations for your machine control computer, we suggest the following (figure 2.2):

1. USB bulkhead (panel mount) cable. This allows you to mount a USB socket directly on the

side of the cabinet. You can use a standard USB flash drive to transfer G-code programs and other files to the machine controller. This is Tormach PN 30278 (USB bulkhead mount cable – 3' Version 2.0 USB A to A extension M-F).

2. USB extension cable, extending the short cable normally found on keyboards and other

USB devices. Tormach PN 30279 (10FT USB 2.0 A to A Male/Female Extension Cable).

3. USB mini-keyboard. This is about the size of most laptop keyboards. The keyboard

includes a key which will power down the computer, allowing a convenient way to shutdown the system. This is Tormach PN 31371 (Mini Keyboard). The keyboard can be protected against coolant or chips by addition of Keyboard Cover PN 31384.

4. A Tormach USB jogging pendent is a very useful accessory for jogging, manual operations

and machine setup. Two options are available: a key based pendant (Tormach PN 30214 Pendent, 10 key USB keypad) and a jog/shuttle controller pendant that gives very fine control of jogging speeds and distances. (Tormach PN 30616 Jog/Shuttle Controller).

5. LCD monitor signal cables are normally too short. Most inexpensive VGA signal extension

cables create serious signal degradation. This is particularly true with Super VGA screen resolutions. Tormach PN 30280 (10FT SVGA Super VGA M/F Monitor Cable w/ ferrites) is designed to extend Super VGA signals without degradation.

6. This is simply the AC power cord of the computer. The Computer switch on the operator

console controls a convenience outlet on the bottom of the machine control cabinet. If you set the BIOS/CMOS configuration in your computer to start the computer when it sees AC power then the console switch will allow you to start the computer from the console. You should not shut off the computer from this switch due to issues with the Microsoft Windows operating system, but you can turn the computer on from the keyboard/screen

controls. There are several important points to bear in mind when using devices interfaced with USB (Universal Serial Bus).

Do not attempt to run a G-code program that is stored on a USB drive (often called pen drives, memory stocks, flash drives). Copy your G-code files into a folder on the hard drive (usually C: of the control computer. Remove the USB drive after making the copy.

Do not use external USB hubs or devices like monitors or keyboards containing hubs. USB devices can be affected by electrical noise on the computer mains power line. Devices

with large motors like compressors and ‘shop vacuum cleaners should not be plugged in to a multiple outlet used by the control computer.

These rules minimize the chance of Windows deciding to manage USB devices when you are running cuts on the mill.

The milling machine itself requires a 115 volt single phase wall power outlet rated at 20 amps.

2.1.4 Learning and Training

The final element of planning your installation is to consider the training that you and any other users of the machine will need.

This manual will give you the basic information required to start manufacturing components with you PCNC. You must, however, expect to have to invest time in learning how to achieve the best results. The areas which you will find easy and those which will require more effort will of course depend on your background; you might be most comfortable with machining or with component design or even with information technology.

32426 Rev C1-1 2-3 Using Tormach PCNC 770

Preparation

Figure 2.4

– Un-crated machine on pallet

We believe that you will find it highly cost-effective to acquire additional training materials for areas of CAD/CAM/CNC which are new to you. Tormach sales can help point you in appropriate directions.

2.2 Receiving, Unpacking and Checking Shipment

2.2.1 Moving the Crate

The PCNC is supplied on a standard pallet and can be offloaded from a truck with a tailgate lift and moved on smooth surfaces using a hydraulic pallet jack. This makes delivery very economical (figure 2.3).

Remove the crate top and sides with care as the axis drive stepper motors are in vulnerable places (figure 2.4).

The crated system weighs less than 800 lbs (400 kg) nevertheless, it requires mechanical handling to move it over rough ground. The machine is designed to be modular so it can be dismantled to move through small doorways or along narrow corridors and has an optional moving kit (Part number 31333) to facilitate this. Some mechanical handling equipment will be needed to lift it onto the stand. Tormach advises you to employ the services of a specialist rigger if the machine has to be moved in situations where the pallet lifter cannot be used or where there is no crane to lift the machine onto its stand. It is possible to improvise using a small trailer, a portable engine crane and similar tools if there is no alternative but this risks injury to you and damage to the machine.

Figure 2.3 – Crated machine as delivered

2.2.2 Uncrating and Inspection

After uncrating you should check the contents against the parts listed on the packing slip and inspect the machine for any damage incurred during transit so any claims can be made within the carrier’s deadline.

2.3 Mounting the PCNC

2.3.1 Lifting onto Stand

The machine can be lifted onto an operating stand by either of two methods: from below using the base connection points or from above using a slinging technique. In either case caution and common sense are needed for the protection of the machine and the people involved. Lifting up to 600 lbs can be simple with proper preparation and good equipment, but it is never trivial and the dangers involved should be taken seriously.

The work of lifting and placing heavy equipment is called rigging. If you are not trained or prepared then you should seek the advice of those who are. Professional riggers can be found in most areas.

Using Tormach PCNC 770 2-4 32426 Rev C1-1

2.3.1.1 Lifting from Below

The base of the machine has four 7/8" diameter holes. By sliding two steel bars into these holes, at least 32" in length, you end up with some outrigger wings that can be used in combination with a fork lift truck to lift the machine. These should be solid steel bars, not pipes and be ¾" or

" in diameter.

2.3.1.2 Lifting from Above

The alternative way to mount your PCNC to a stand involves lifting from above. The eye in the top of the column is suitable for lifting the machine, but it is not in line with the center of gravity. The machine will tilt when lifted solely from the eye. The alternative is to sling the machine using a combination of the eye and an eye in a T-nut on the table using a Tormach special tool (part number 30576 -

Machine Hoist Bar) (figure 2.5).

Preparation

Figure 2.5 – Hoist bar for slinging the mill

Figure 2.6 shows the geometry of the slinging. The table should be as far away from the column and as far to the right as possible to optimize the balance.

It is most important that the machine is not lifted by the control cabinet or by any of the protruding stepper motors or the head or the table. Incorrect rigging of the sling will likely result in serious damage to the PCNC.

The optimal balance for lifting should be checked with the machine an inch or two off the floor.

The X-, Y- and Z-axes can easily be moved by hand if the covers on their coupling boxes are removed. The smooth (i.e., outside face) of an old auto engine timing belt or poly-vee auxiliary drive belt, which has been cut to make a strip, can be used to turn the coupling between the stepper motor and ball screw (figure 2.7).

When you are ready to lift the machine you should remove the nuts from the four screws holding it down to the pallet.

2.3.2 Fixing to Stand

Figure 2.6 – Slinging geometry

Unlike very large mills, the level of your

32426 Rev C1-1 2-5 Using Tormach PCNC 770

Preparation

mill does not significantly alter machine accuracy. Leveling should be sufficient to provide proper coolant drainage, but precision leveling is not necessary.

The supports under the corners of the base of the mill are important to machine accuracy. Despite the apparent stiffness of the base casting, it will respond to the weight of the machine. The result will be errors in the left/right tram of the mill. For best accuracy, add shims under the left front or right front corners of the machine as needed, such that the left/right tram is within your desired tolerance. Something like

0.002” is usually all that is needed; however it is certainly possible to do even better.

A welded steel stand is unlikely to be flat. Furthermore, if it is flat sitting on its own, it will sag down as the 800 lb machine is placed on it. Be aware that welded steel stands are neither stress relieved nor as stiff as the machine base itself. If, for example, you place a

0.050” shim between the base of the mill and the stand, you’re not actually lifting the corner of the base up by

0.050”. It is more likely that you are moving the mill up by 0.005” and the corresponding point on the stand down by 0.045”.

2.3.3 Installing central lubrication pump

The standard pump is manually operated. An optional automatic pump is available. It comes with its own installation instructions.

The manual pump is fixed by the two socket screws provided to tapped holes on the left hand side of the stand. You may find that your pump mount bracket is oriented backwards.

Simply remove the 4 screws connecting the bracket to the pump and rotate the bracket 180 deg.

Connect the lube pipe to the elbow on the pump and fill it with suitable clean way lubrication oil.

2.3.4 Accessories

You should now try out the positioning of the screen, computer and coolant subsystem, if any.

2.4 Power to the PCNC

Figure 2.8 – Fitting manual oiler

The PCNC 770 is powered by 115 volt single phase AC (50 or 60 Hz). The computer, monitor and coolant pump should all be specified for 115 volt operation..

The main machine power lead is shipped with a US style

Using Tormach PCNC 770 2-6 32426 Rev C1-1

Figure 2.9 – Power outlets

Preparation

plug. Should you need to change this please note that the wire color code is Black = Hot (Live), White = Neutral and Green = protective ground.

2.5 Power for Machine Accessories

The 115 VAC outlet under the control cabinet that is nearest to the column feeds the coolant pump and is controlled by the CNC software and panel switch. The pair of similar outlets further from the column is switched by the Computer switch on the front panel.

2.6 Tormach Machine Controller and Software Installation

2.6.1 Control Computer

We recommend that you purchase a Tormach Machine Controller as part of the mill package. Tormach Machine Controllers include MachOS, an implementation of Microsoft Windows Embedded which was developed by Tormach to avoid the problems frequently seen with configurations based on Windows XP, Vista, or 7 . The Machine Controller is available as either a Basic and Performance model. Because of the high spindle and axis speeds possible, we recommend using the Performance model.

If, in exceptional circumstances, you wish to provide your own computer, it needs to run the 32 bit (x86) version of Microsoft Windows XP (Home or Professional edition) or Microsoft Windows 7. Our experience is that the more modern and high performance the motherboard in your computer is, the less reliable the performance running a real-time task will be. This is due to many power saving and temperature control tricks used by the chip manufacturers. The Tormach Machine Controller is specifically designed for real-time applications.

Details of the computer requirements and software installation for a standard PC can be found in Appendix 3.

2.6.2 Setting Up Your Controller

2.6.2.1 Positioning the Controller

The controller should be positioned where it will remain clean and dry. It can be placed vertically or horizontally. When vertical it should be resting on the rubber pads. When horizontal it should be resting such that the CDROM drive is above, with the power button on the lower right corner.

Do not allow anything to block the vented cabinet holes. The steel cabinets design for PCNC series mills have storage sections intended for the controller. The cabinet storage areas are large enough to provide adequate cooling without the need for additional fans. The controller remains well protected in the machine stand, but access to the controller is less inconvenient. This isn't a concern if you power the controller through the computer outlet on the PCNC mill (see the section below Operating the Controller: Starting the Controller) and if you extend the USB ports using USB Bulkhead Cable (PN 302781) which positions a USB port to the outside of the machine stand.

Figure 2.10 – Front of TMC

Refer to http://www.tormach.com/document_library/DS30278_USBBulkheadCable.pdf

32426 Rev C1-1 2-7 Using Tormach PCNC 770

Figure 2.11 – Rear of TMC

Preparation

2.6.2.2 Keyboard and Mouse

The controller supports with USB (figure 2.11 - sockets at 5) or PS/2 style mouse and keyboard connections (sockets 1 & 2). Wireless keyboards and mice are not recommended. Both powered and passive USB hubs have a history of problems when used in combination with Mach3 software. We recommend that all USB devices plug directly into the USB ports on the controller (sockets 5).

2.6.2.3 Display

Connect the display to socket 4 - figure 2.11.

2.6.2.4 Speaker and Microphone Connections

Speaker and microphone connections are possible but not recommended.

2.6.2.5 Power Connections

Check the voltage setting before connecting power (figure 2.11 – location 13). The controller can be set to run on either 115 VAC or 230 VAC and will operate equally well on 50 or 60 Hz power.

2.6.3 Operating the Controller

2.6.3.1 About the Operating System

The MachOS operating system is built with Microsoft Embedded Standard, but it looks and acts much like Windows XP Pro. If you are familiar with Windows XP, then you know how to use MachOS. The Tormach Machine Controller has s been designed and configured to work with Mach CNC control software. Under most circumstances, no modification to the configuration is needed. Modification to the configuration of the operating system can disable the controller.

2.6.3.2 Starting the controller

The Controller is configured to boot immediately upon the application of power. This allows you to turn on the computer using a remote power switch, such as the power switch marked COMPUTER on the front of the PCNC mill control panel. You can also start the controller using the power button on the front panel. For the present just power the Controller and your monitor from a wall outlet.

PCNC control software (Mach3) will start immediately after the Controller boots. If you need to exit the control program you can restart it using the desktop icon.

2.6.3.3 Stopping the controller

The controller should be stopped by clicking on the Start > Shutdown function on the lower left corner of the computer screen. It is not a good idea to simply turn off the controller, it should be allowed to shutdown properly.

After you have shutdown the computer, turn off the computer power using the switch on the front panel of the mill. This will allow you to use the power switch to turn the computer back on. If you forget to turn off the power then you will not be able to turn it on using a quick offon cycle of the computer power switch. The computer needs to be off for 30 seconds before the function of "Boot upon Power" will work.

2.6.3.4 Mach3 License Installation

Important Note: The controller is shipped without the Mach3 license on its hard drive. The Mach3 control program installed, but without the license it will only work in demo mode (limit 500 lines of code) without the Mach3 license. Tormach ships the Mach3 software license on a separate CD. To install you license file, simply insert the license CD after the controller has

Using Tormach PCNC 770 2-8 32426 Rev C1-1

Preparation

booted up. The license file will automatically be transferred to the hard drive. You can then remove the license CD and store it in a safe location.

2.6.4 Machine Controller Maintenance and Configuration

2.6.4.1 Login and Software Installation

The controller boots up to an automatic login with Username: Operator and a blank password. The Operator has rights to use the software but cannot install software or modify the MachOS configuration. If you need to install software or modify configuration you must logout Operator and login again with:

Username: Administrator Password: administrator

Note that the upper/lower case is important. The Administrator login will be necessary if you need to reinstall the PCNC software or install new software.

The controller is licensed as a dedicated machine controller. Do not attempt to use it as a desktop computer and do not try to install general purpose software such as Microsoft Office or Microsoft Word. You can install CNC related software such as CAD, CAM, or machining utility programs such as Machinist's ToolBox although Tormach does not recommend this..

2.7 Connecting and Running the PCNC

You have now completed the installation and merely need to connect the PCNC to the computer.

Now close down MachOS and switch off the Controller. Connect the parallel port of the computer (figure 2.11 socket 11) to the D25 connector on the underside of the PCNC control cabinet. The cable provided to connect the computer to the mill meets IEEE 1284 specifications. This provides a high level of immunity to electrical noise, which is important to reliable operation. Do not use inferior cables.

Now power the Controller from the outlet near the D25 connector and if relevant, power the monitor from the connector adjacent to it below the PCNC control cabinet. Viewed from behind, the inlet is on the right next to two outlets for computer and monitor. The coolant pump outlet is to the left of these (figure 2.9).

2.7.1 Main Switch and Control Panel

The rotary main switch on the right hand side of the control cabinet disconnects the mains power from the PCNC itself and isolates computer/coolant outlets that are on the bottom of the cabinet.

Warning: You should not open the control cabinet until the mains power to the machine and to the computer/coolant pump are both removed from the wall outlet. Live parts may be exposed even when the main switch is in the off position.

Computer On/Off

Warning: The following power-up and power-down sequences should be followed exactly to

avoid the risk of unintended machine motion which could cause injury to you or damage to the machine.

32426 Rev C1-1 2-9 Using Tormach PCNC 770

Preparation

Switch the main switch ON and switch the computer power on at the PCNC control panel

Figure 2.12 – Control panel layout

(figure 2.12). The computer will power up and run the Control Program (figure 2.13). This will allow you to

perform all the important functions on the standard machine. If you have the 4th axis or want to use G-code features like Optional Stop then you may wish to use the Comprehensive Run screen (figure 2.14). In this case click the Comp Run button to change the display.

The screen “Light Emitting Diodes” (LEDs in this manual) by the Reset button will be flashing as will the

Machine OK LED.

Now, returning to the operator’s panel:

Start and EStop

The Start button will energize the circuits for the axis drives and for the spindle motor. The

Stop button stops all motion and is the

Emergency Stop (EStop) control. The Stop button locks in the off position once it has been pressed as safety feature. It can be released by a turning the button-head a quarter-turn clockwise. Note: Once the stop button has been pressed the start button is inoperative until the stop button is released.

The Machine LED indicates that the Start button has been pressed. When it is lit then the

Machine OK LED on the computer screen should be solid green. If this does not happen then

Figure 2.13 – Simple main screen

Figure 2.14 – Comprehensive Run screen

Using Tormach PCNC 770 2-10 32426 Rev C1-1

Spindle

Preparation

you should check that the cable between the PCNC and computer is fully plugged-in at both ends. You will be able to test some controls on the PCNC, even if the LED does not give the correct indication but you will have to find the fault before you can move the PCNC axes under computer control.

An important safety interlock is that the rotation of the spindle can be disabled (while maintaining axis drive power) by the Spindle Lockout key-switch. The switch on the spindle drive door performs the same function. These are used to ensure that the spindle cannot start when an R8 tool holder is being changed (door open) or when a tool is being changed in a collet chuck. Turning the Spindle Lockout key or opening the spindle cover while the spindle is running will also stop the spindle. Stopping the spindle in that way will not damage any components, but it is generally a poor practice.

The controls to the right of the key-switch are all concerned with manual control of the spindle. If the Manual/Auto switch is in the Auto position then none of the other spindle controls have any effect. In the Manual position the computer control of the spindle is disabled.

Switch to Manual and turn the speed control knob fully counterclockwise. Press the Spindle

Start rocker. The spindle should start turning slowly in the clockwise (forward) or

counterclockwise (Reverse) direction (viewed from above) depending on the setting of the

Forward/Reverse switch. You can safely switch directions while the spindle is turning.

Try changing the speed using the rotary control knob. The actual speed will depend upon which of the two pulley ratios you have selected.

Pressing the Spindle Stop rocker will halt the spindle.

Coolant

The Coolant switch controls the power to the coolant pump outlet on the underside of the control cabinet. In the Off position the outlet is not powered and the pump will not run. In the

On position power is applied to the outlet and the pump will run until the switch is switched to

either off or auto positions. In the Auto position outlet power is under program control the pump will run if the Control Program requests coolant.

Accessory Socket

The Accessory socket is for connection of accessories such as a touch probe. See Chapter 8 for details of the interface.

2.7.2 Changing the Spindle Speed Range

The PCNC 770 has two speed ranges. The low range, 175 to 3,250 RPM, is suitable for most machining operations with ferrous and other tough materials. The high range, 525 to 10,020 RPM is suitable for small diameter cutters, plastics and non-ferrous materials. The range change is performed by moving the multi-vee belt from the upper pair of pulleys (high speed range) to the lower pair (low speed range).

Figure 2.15 – Changing spindle pulley setting

Open the spindle drive door. The interlock will prevent the motor from running. Note:

32426 Rev C1-1 2-11 Using Tormach PCNC 770

Preparation

Opening the spindle drive door will also stop a running spindle; however, this is a safety hazard and should not be used as a substitute for stopping the spindle with the spindle controls in the Control Software. Use the included wrench to loosen the motor mounting plate and the front handle to pull the motor forward. The belt will slacken and can be moved from one set of pulleys to the other (figure 2.15).

For the following tests, select the low speed range by placing the belt on the lower pair of pulleys). Retighten the belt so there is between 1/8" and ¼" movement between the pulleys, lock the motor mounting and stow the handles in the vertical position.

2.7.3 Computer Control of the Spindle and Coolant

Switch the Spindle and Coolant to Auto on the control panel. Make sure the computer is displaying the Simple Run screen as shown in figure 2.13. The portion shown in figure 2.16 shows the controls for the spindle.

Use the mouse to click the Hi/Lo button. You will see that the screen LEDs depicting the pulleys will change and the appropriate maximum speed will be displayed below them. Choose the Low setting to correspond to the PCNC pulleys.

Note: Just after starting the system the screen LEDs may not correspond to the indicated maximum speed. The speed value is always correct and a click on the Hi/Lo button will bring the LEDs into step.

Next to the label S, is a digital read-out (DRO) of the requested spindle speed. You can change this by clicking the mouse on it. It will become highlighted. Type a number, say 525 (for 525 rpm) and press Enter. Figure

2.17 shows the screen just before pressing Enter. If you make a mistake you can press Esc to return to the original value.

This technique is used for setting any DRO. Remember to

Figure 2.16 – Spindle controls

use Enter after any DRO change. If you forget and just click on another DRO, then any value you have just entered will be discarded. This is designed to avoid accidental changes.

Now check that the machine is safe and that the motor door is closed and click on the Spindle CW F5 button. The spindle will start running. Clicking the button again will stop it.

The F5 in the caption tells you that function key F5 is a “shortcut” to this button; it can also be used to start and stop the spindle.

Figure 2.17 – Setting S word

Notice that there are two sets of screen LEDs. The outer set indicates that the machine is dwelling to ensure the spindle has started and fully stopped. The center LED indicates that it is running.

If you have connected a coolant pump to the outlet under the control box (see vacant outlet in figure 2.9) then you will be able to control it by the Coolant Ctrl-C button or its shortcut which is the Ctrl-C key. Beware of the position of the coolant nozzle before you try this!

Using Tormach PCNC 770 2-12 32426 Rev C1-1

Preparation

2.7.4 MDI for Entering G- and M-code Commands

When you are making parts the commands to the machine (G- and M-codes) will generally be read from a file. It is however often convenient to command the PCNC directly. This can be done by typing command into the Manual Data Input (or MDI for short) line.

The command to start the spindle in the clockwise direction is M3 and the command to stop it is M5.

Click the mouse in the bar marked MDI. It will highlight. You type the command in the highlighted line. Unlike in DROs, the Backspace, Del, Left and Right arrow keys are available to help you correct any typing errors.

When you press Enter the command will be executed. Pressing Esc abandons it and closes the MDI line. You can try starting and stopping the spindle with M3 and M5 G-codes.

Figure 2.18 – MDI Line in use

Notice that the recent commands are displayed in a fly-out box. You can choose one of these to copy into the MDI line using the Up and Down arrow keys.

Figure 2.18 shows the MDI line after the spindle has been started (M3) and the M5 has been typed but not yet executed by Enter.

There are some handy features of the MDI box. It can be opened by pressing Enter (rather than needing a mouse click). It stays open after a command has been executed. It can be closed by Enter when it is blank.

Note: All keystrokes go to the MDI when it is open so it is not possible to execute shortcuts or jog the axes. If the keyboard does not do what you expect then you probably still have the MDI line open.

2.7.5 Jogging the Axes

The final thing to try before actually making your first part is to move (jog) the PCNC axes using the keyboard.

There are several options for jogging which will be explained in detail below. The jogging controls are at the top right hand side of the screen (figure 2.19).

Click the Jog ON/OFF button (or use its shortcut Ctrl-Alt-J) to turn on the screen LEDs beside it if they are not already on. Click Jog Mode (or use its shortcut) to turn on the larger of the LEDs above the word Cont (for Continuous jogging). Type the value 10 into the Slow Jog Rate DRO; do not forget the Enter to accept the value)

Figure 2.19 – Simple jog controls

In the next steps you may find the directions of movement are unexpected. Therefore, when you use the arrow keys you should be prepared to quickly release the key if the axes moves in an unexpected direction or is near its limit of travel. Now, press the Left, Right, Up and Down arrows on the keyboard. The table will move while you hold the key down. If you crash into the limit switches then the LED beside the red Reset button will flash and the machine will stop. Click on Reset and very carefully jog the other way. Take care not to mechanically hit the limit doing this in the wrong direction. You will lose the referenced status if you trip a limit switch.

32426 Rev C1-1 2-13 Using Tormach PCNC 770

Preparation

You might find the directions of movement are unexpected. Figure 2.20 shows the tool above a work piece. The positive X, Y and Z directions are marked by arrows. If you press the Right arrow key then the tool will move in the positive X direction (i.e., to the right of the work). Similarly the Up arrow moves the tool in the positive Y direction (i.e., towards the PCNC column). Of course, this actually happens on the PCNC by the table moving under the tool but you must

Figure 2.20 – Jogging is to move the tool relative to work

imagine what it would look like if you were sitting on the table and watching the tool.

You should jog around until you are quite confident which way the machine moves when you press any key. Notice that the values in the Axis DROs change as you jog the tool around.

Jogging the Z-axis is done by using the Page up and Page down keys. Here of course it is the tool that moves, so “Up” is indeed up.

2.8 Summary

This chapter has covered a lot of basic ground. Much of it only has to be done once. You may however wish to revisit the latter parts if you are not fully confident with using buttons, DROs, the MDI and jogging. We will give less detail on using these (e.g., assume you know about shortcuts and when to use Enter) in subsequent chapters.

Using Tormach PCNC 770 2-14 32426 Rev C1-1

Making your first part

3. Making Your First Part

This chapter shows you how to make your first part with the PCNC. It assumes

that you have no prior experience with running a part-program on a Computer

Numerically Controlled machine tool.

Even if you have previous experience you will find that following this tutorial

gives you an introduction to the controls of the machine.

3.1 Coordinates

Coordinates are simply how you describe where the tool is positioned. We assume that you have the computer and PCNC setup and switched on and are looking at the Simple screen.

3.1.1 Referencing the Machine

You have seen that jogging the machine moves the tool and this changes the numbers in the X-, Y- and Z-axis DROs. You may have wondered where these numbers come from and indeed doubted that they are very sensible. The answer is that they are probably meaningless. The computer has no way of knowing yet where the tool or table is positioned.

Referencing is the process which puts the machine in a known mechanical position and sets the corresponding axis DROs. The known position is where the limit switches operate with Z at the top of the column and the spindle over the top lefthand corner of the table. This position is called Home and so these limit switches are called the Home switches. Their operation is very obvious on the Z-axis. A software trick makes the X and Y arrangement slightly harder to understand but this is of no importance at present.

Figure 3.1 shows how the DROs might look when you start up the system. They have arbitrary values in them and the three screen LEDs are red.

Check that the LEDs by the red Reset button are not flashing and that nothing is in the way of movement of the table and head of the PCNC. Click the Ref All button.

The Z-axis will first move up to the top of the column, stop at the switch and then move down a fraction. The Z DRO will be set to zero and its LED turn to green. This will be followed by the same action with X and Y. Be wary the first time you do this and if an axis does not stop at its switch you must hit the EStop button on the PCNC control panel and look at the Maintenance/Troubleshooting section of this manual (figure 3.2).

Figure 3.1 – The axis DROS un-referenced

Figure 3.2 – Referenced and ready to use

Note: It is helpful to reference the PCNC before using it. This allows the working envelop in X and Y to be shown on the tool path display and helps avoid running into the limit switches or, worse, the tool attempting to cut into the vise or table. The Control Program tries to protect you

32426 Rev C1-1 3-1 Using Tormach PCNC 770

Making your first part

from this sort of trouble but intentionally leaves the responsibility of referencing to you. You can repeat the referencing operation at any time if you have reason to suspect that the PCNC is in the wrong position (e.g., an error in a depth of cut has stalled the machine).

Despite the advantages of having the machine referenced, you can still use it without reference, for example if one of the home switches fails or becomes unreliable. We advise you to treat this as a crippled mode for use until you can get the switch fixed. The Goto toolchange position macro M999 and G28 will not work if the machine is not homed but you can ignore the error message and jog the axes by hand to get clearance to change the tool. The home reference procedure is how the machine learns where it is within its own framework and that knowledge is essential to execute M998 and G28.

The accuracy of the limit switches is subject to contamination by dried up coolant, the presence of chips, and other factors. Consider the work offsets to be approximate only and do not depend on the automated reference procedure for your most accurate work. For maximum accuracy, you should touch off in X, Y, and Z after referencing and before proceeding to cut.

The Control Software now knows exactly where the PCNC axes are and has called this home position X = 0.0, Y = 0.0 and Z = 0.0. You probably think that this position is not very convenient and you are correct. The Control Software will let you define any other place to be 0, 0, 0 when you are running a part-program but will always keep a record of the machine position using home as machine zero. Normally the axis DROs will show your coordinates for the position but you can see the Control Software machine coordinates by clicking the Machine

Coords button. A big flashing LED warns

you that you are not looking at your version of the coordinates.

3.2 Loading a Demonstration Program

The system comes with a demonstration program in the file

C:\PCNC3\GCode\FirstPart.nc

Run the Control Software and make sure the screen LEDs by Reset button are not flashing and that the axes are referenced.

Click the OpenG button. You will be given a Windows open file dialog. Navigate to the G-code folder and open the file (figure 3.3).

You will see the code of the program in the window at the left of the screen and the path that the tool will take in the toolpath display. Use the mouse to drag with the left-hand button in the toolpath display to rotate the display. It behaves as if it is drawn inside a clear ball and the mouse turns the ball.

Figure 3.3 – File opening

Figure 3.4 – The drawing for FirstPart

So that you understand what is going to happen we should look at the way this file was produced using a Computer Aided Design/ Computer Aided Manufacturing (CAD/CAM) program. The PCNC will produce parts designed

Using Tormach PCNC 770 3-2 32426 Rev C1-1

Making your first part

in any available industry standard tools. Tormach offers a number of powerful, yet reasonably priced software tools, some of which are used as examples in this manual.

The original drawing is shown in figure 3.4. It consists of the characters “PCNC” and an irregular quadrilateral.

Having drawn the outline of the part, we defined the material from which it will be cut, the size of tool to cut the letters ( ¼") , the depth of the letters, the size of tool to cut the recess (½") and the depth of the recess. The program automatically creates the part-program (G- and M-codes) to make the part and can display a visualization of the finished work (figure 3.5). We will discuss the options which you have for designing your own parts in the next chapter.

You should now be able to relate the toolpath display to the part

Figure 3.5 – CAD/CAM Visualization of finished part

illustrated

3.3 Running the Demonstration Part-program

3.3.1 Part Material

We suggest that you use a free-cutting material to make this first part. MDF, birch ply or, as we used, resin impregnated ply are all suitable. You need a piece at least ½" thick and 7" by 4". Clamp this securely to the PCNC table. For many jobs it is worth putting a layer of scrap material under the work. This will protect the table when through holes are to be cut and may save damage in the event of a mistake in the part program or in operating the machine.

Put a ¼" diameter tool into a tool holder in the spindle. Ensure the lower spindle pulleys are selected on the machine and are set on the screen using the Hi/Lo button.

Use masking tape to indicate a 5" length near the middle. This length must be clear of the clamps.

Figure 3.6 – Tool setup at zero points

3.3.2 Setting Work Offsets

Jog the axes so that the tool is just above the material at the top left-hand corner of the 5"

Figure 3.7 – Toolpath during a cut

section (figure 3.6). We suggest that you do a dummy run cutting in the air so jog the Z-axis up about two inches.

32426 Rev C1-1 3-3 Using Tormach PCNC 770

Now click in the X-, Y- and Z-axis DROs, in turn and type the value 0 into each of them. Do not forget to press Enter to accept the values. The reason for doing this is that you want the position of the tool (i.e., at the top left of your material and an inch above it) to be X = 0, Y = 0 and Z = 0. The Control Software still refers to the home switches as zero internally but lets you have your own separate coordinate system for the work. If you click the Machine Coords button then you will be shown how your zero relates to the home position. The difference between the machine coordinates and your coordinates is called the Work Offset.

Note: We are going to cut this part by giving you a "recipe". You will learn why and how it works later. Please don't add anything extra to the recipe. Adding yeast to a soda bread recipe makes a fine mess. For example, here, you should have the length of each tool in the tool table still set to zero.

You are now ready to run the program.

3.3.3 Cutting in Air

Click the Cycle Start button. The PCNC will start running but almost immediately ask for tool number 1. This is already loaded so just click Cycle Start again. The machine will trace the letters PCNC in the air. It does this four times because they are to be cut 0.2" deep and the program is designed only to cut 0.05" each time. This is conservative but runs no risk of breaking the ¼" diameter tool.

Making your first part

The toolpath shows the tool as it moves by a different colored line (figure 3.7).

After “cutting” the letters the machine will stop and ask for tool number 2. Jog the Z-axis up a few inches so you can put the ½" cutter into the tool holder. Then jog down to about 2" above the material, and type the value 0 into the Z DRO. Do not forget to press Enter to accept the value.

Now click Cycle Start again. The machine will use a spiral path to cut out the recess (called a pocket).

3.3.4 Cutting the Actual Part

You should now be ready to actually cut the part.

Jog the Z-axis and swap back to the ¼" tool. You must now set this so it is just touching the surface of your material and define this as Z = 0. There are many good ways of doing this and we will look at them in a later chapter. For now you just need a thin sheet of paper or perhaps a plastic wrapper from a candy packet.

Figure 3.8 – Touching a tool

Figure 3.9 – Cutting the text

Jog the Z-axis down to ¼" or so above the material. If you are using keyboard jogging, change the Slow Jog % DRO from 10% to 2%. The Tormach Jog/Shuttle Controller allows you to control the speed depending on how far you turn the ring.

Using Tormach PCNC 770 3-4 32426 Rev C1-1

Making your first part

Then with the paper below the tool, carefully jog down until the paper just gets trapped by the tool. You must avoid ramming the tool into the material; you want to just touch the paper (figure 3.8).

When in position type 0 and Enter into the Z-axis DRO. You now have the Work Offsets set to suit your material thickness and length of tool.

Make certain you have properly shut the door protecting the motor and spindle belts or the spindle will not start and a non-rotating tool will try to cut the work.

Click Cycle Start. The program will stop for a tool change to tool 1. Just click Cycle Start as you have tool 1 already in the spindle.

The PCNC will cut the letters in four passes. Figure 3.9 shows this process in pass two.

When the text is done the machine will stop and request a change to tool

2. Jog up so you can change the tool to the ½" cutter. If you hold the Shift key down when jogging the jog will take place at full speed rather than the 2% used for very careful positioning. Change the tool and jog down with the paper

Figure 3.10 – Cutting the pocket

under the tool. Type 0 and Enter into the Zaxis DRO to define the new Work Offsets. Again check that the door is shut.

Click Cycle Start to run the program to cut the pocket. Figure 3.10 shows this partially done.

When the pocket is completed the machine will stop and rewind the program so it can be used to cut another copy of the part.

The completed piece is

Figure 3.11 – The completed part

shown in Figure 3.11. You can compare this with the CAD/CAM visualization in figure 3.7.

3.3.5 Summary

This chapter has allowed you to make your first part with the PCNC. Although it is fairly simple it would be very difficult to make without a CNC machine. When you are experienced you should be able to design and make something like it from scratch in about 45 minutes.

32426 Rev C1-1 3-5 Using Tormach PCNC 770

Making your first part

You might have wondered about some of the things that you were told to do. Why did you cut the text then remove half its depth with the pocket? Could the system be told how long each tool is so you do not need to touch tools each time you make a part? Could the part be made in steel with the same program?

These are all good questions. What you were told to do was to make this first part in the easiest way not necessarily the quickest or most accurate. Subsequent chapters will tell you the answers to these questions and give you the understanding to make the right design and manufacturing decisions for yourself. This experience and understanding will be invaluable whether you make production parts yourself or your designs are manufactured by others.

Using Tormach PCNC 770 3-6 32426 Rev C1-1

From an idea to a part

4. Routes from an Idea to a Part

This chapter describes the different ways in which you can define parts to be

made with the PCNC.

It explains, in detail, how to use those features which are supplied built-in to or

bundled with the PCNC Control Software.

4.1 Controlling the PCNC

If you have run the sample program used in the previous chapter then you will have seen the control language of the PCNC scrolling through the G-code window as it is executed. Although this may look complex it is actually very simple. It was originally designed for machines whose computer was comparable in power to the one in a microwave oven or multifunction TV remote control!

Computer hard disc

Keyboard

G0 X2.1 Y3.4

PCNC 1100 Software

G0 X2.1 Y3.4 G90G80G49 G0 Z20.0000 S1000 G0 Z20.0000 G0 X2.8521 Y3.0343 M3 f239.000 G1 Z0.0000 f239.000 G2 X2.5087 Y3.6823 I3.2919 G1 X2.5087 Y6.6988 G2 X2.8521 Y7.3468 I3.2919 J6.6988 G1 X3.8022 Y7.3468 G2 X4.1456 Y6.6988 I3.3623 J6.6988 G1 X4.1456 Y5.7764 G3 X4.4890 Y5.1284 I4.9288 J5.7764 G1 X5.5160 Y5.1284 G3 X5.8594 Y5.7764

M & G Code Program File

Manual Keyboard Controls

Direct Code Entry on MDI

Run Code Program File

Standard Text Editor (Microsoft Notepad)

PCNC 1100 Wizards (Conversational Programming)

DXF, HPGL, JPG File Conversions

CAD / CAM Program

Methods to Create Program Files

Figure 4.1 – Schematic on how to generate part-programs

The PCNC is always controlled by commands in a part-program. Most of these are G-codes although many other letters are used to define the details like the spindle speed, feed rate, etc. which are required. Thus a part-program is sometimes referred to as a G-code program.

Movement of the machine axes is controlled by three different G-codes.

32426 Rev C1-1 4-1 Using Tormach PCNC 770

From an Idea to a part

• G00 moves at the maximum speed of the machine so is used when no cutting is required

• G01 moves in a straight line between two points at the set feed rate

• G02 (and G03) move in a circular arc between two points in a plane and possibly in a

straight line in other direction (e.g., to make a spiral).

All the moves take place from the current position of the tool. G00 and G01 need the coordinates of the ending position (e.g., G01 X3.2 Y2.1 Z -0.3 would move the three linear axes together so the tool will follow a straight line ending at X = 3.2, Y = 2.1 and Z = -

0.3). G02 and G03, clockwise and counterclockwise arcs respectively, need additional information to define the center point to be used.

Most G-codes are what is termed Modal. This means they stay in effect until another one is used. So if G01 has been used on one line of code then the following lines only need to give the position of the end of the move. As an example the following code will move the tool to a start position (X = 1, Y = 2) and then move it in a square of side 3.1.

G00 X1.0 Y2.0 G01 X4.1 Y5.1 X1 Y2

In practice, however, the simplicity of G-codes is deceptive. Calculating the position of the “center” of the tool by hand is tedious and error prone. If you wanted to cut around the outside of a block of material to make the 3.1" square then you need to allow for the diameter of the tool and need to move the Z-axis to take acceptable sized cuts in each of several passes.

You will easily be able to learn what a part-program is intended to do but it is unusual to write one by hand as there is a wide range of software tools that can help you (figure 4.1).

4.2 Choosing the Appropriate Design Software

A mill is capable of producing three different classes of work which are usually referred to as 3D, 2½D and 2D.

A 3D product has complex and often smooth curves in all three dimensions. A typical example is a mold for die-casting, vacuum forming or injection molding.

A 2½D product has detail at several depths from the surface of the material but each piece of detail has a flat bottom surface. The FirstPart cut in Chapter 3 is an example of a simple 2½D component.

A 2D product has no changes in depth. This might be a mechanism link cut out of a sheet of steel or lettering cut out of vinyl sheet. 2D products can be milled but are usually produced on specialist machines (e.g., a laser table or plasma cutter).

Design and particularly production of a 3D shape is much more time consuming than something which is 2½D. If the pocket in FirstPart had a dished shape with a fillet in the corners then it would have been cut with a ball nosed tool and would have required many passes a few thou apart rather than the passes about 0.3" apart that could be used with the flat end mill. In addition the design process is complicated because the pocket cannot be defined by a single number (i.e., its depth) if it is 3D.

With current CAD software you will probably find it is easiest to design 2½D parts with a 2½D CAD package or with a full 3D one running in 2½D mode.

4.3 Software for CAD/CAM

This section gives some guidance on things to consider when choosing software. It is a very big topic whose surface we try to skim.

Using Tormach PCNC 770 4-2 32426 Rev C1-1

The two most important points are that (a) the PCNC, because of its open and standard

but line moved

architecture, will run the part-programs produced by virtually all Computer Aided Design/Computer Aided Manufacture (CAD/CAM) software and (b) that the more comprehensive the software that you use, the greater will be your and the PCNC’s, productivity and the better the quality of the parts made. A common mistake is to purchase inadequate design software and then have to discard it and the investment made in learning to use it.

The Control Software itself includes features for defining and cutting simple parts like keyways, rectangular and circular pockets or a plane face by conversational Wizards. You will be able to do useful work with these features but you will get better control and documentation of your parts be using a dedicated CAD/CAM system. Some software integrates the “drawing” (CAD) and G-code production (CAM) functions but it is equally common to use different programs from different suppliers for the two functions.

It is perfectly possible and often efficient to design using a 3D CAD package and machine with a 2½D CAM package.

4.3.1 3D CAD

3D CAD software has the biggest range of purchase cost and the steepest learning curve. If you want to produce true 3D parts like molds then you have no option but to buy the best package you can afford. Alibre produces a good example of a mid-range 3D CAD package and Alibre Design XPress is bundled with the PCNC 1100.

From an idea to a part

Alibre allows you to design parts by extruding 2D shapes. The extrusions can be from different planes or surfaces of the part as it is built up and can be solid material or holes.

Several parts can be put together into an assembly and conventional orthographic engineering drawings more or less automatically produced from the model.

High-end programs like Solidworks and Pro/ENGINEER also work in the same way and can be used to design for manufacture with the PCNC.

A 3D CAD program will typically allow the export of solid models (IGES or STL format) for input to a 3D CAM program or DXF format files for use in 2½D CAM.

4.3.2 2D CAD

In a 2D CAD program you represent parts by drawing the individual views of the engineering drawings. A vast range of software is available (much of it “free”).

We advise that you use software that allows you to express the “intent” of your design in the drawings rather than just drawing a set of lines.

As an example let us assume you want to make a key-hole shaped slot in a block of material. This can easily be drawn as two arcs and two lines with the hole that accepts the key’s shank being highlighted (figure 4.2).

Figure 4.3 – Line moved

Figure 4.2 – Keyhole

Figure 4.4 – Joined

points

How useful this drawing is depends of how intelligently the CAD program can interpret the lines. As drawn they are probably separate and can be moved independently (figure 4.3). Most software will allow joining the lines so they move together (figure 4.4). This however does not really reflect what the part is like.

32426 Rev C1-1 4-3 Using Tormach PCNC 770

From an Idea to a part

The important things about the intent of this design are that the straight lines should be parallel and the same length and that they form a tangent to the arc at the bottom of the slot. If these constraints can be given to the CAD software then it will be possible to change its sizes (e.g., the width of the slot by dragging the radius of the bottom arc) while retaining the shape (figure 4.5).

If the shape is defined like this then the software can display the minimum set of dimensions required to define it (figure 4.6). Finally if a dimension is changed then the part can be redrawn to correspond to the new size (figure 4.7).

4.3.3 CAM

We have seen the sort of features you can get from a CAD program. There are also big differences between different CAM programs. Some CAM programs accept 2D models (drawings) of your part (e.g., DXF) files and expect you to define the Z depth of features like pickets, engraved text and holes. Alternatively a 3D CAM program will find all the dimensional information in the model

Figure 4.6 – Automatic dimensions displayed

(e.g., IGES) file. The main issues to consider are how many times you need to tell the CAM program how to

machine the part and how good a visualization of the part you will be shown.

Figure 4.5 –

Constrained and

size changed

Figure 4.7 – Changed dimension

changes drawing

Suppose we decide that the inside of the keyhole slot is to be cut with a 0.125" end mill using

Figure 4.8 – Path of tool and G-code

Using Tormach PCNC 770 4-4 32426 Rev C1-1

From an idea to a part

conventional milling to a depth of 0.5" with each pass being 0.1" deep. The CAM software will generate a G-code program for this.

In some freestanding CAM software, if the size of the slot is changed so the drawing changes, then you would have to create the pocket G-code for the slot from scratch with each revision of the drawing. Integrated CAD/CAM software will work dynamically with the CAD and automatically recreate the new G-code with each change in dimension.

A reasonably sophisticated CAM program will give you a choice of views of the finished part and the path of the tool as it is manufactured.

Figure 4.8 is a screen shot of a typical CAD/CAM program and shows the toolpath for one version of the slot. It is shown in a plan view together with a pane which displays the G-code generated to perform the operation.

Figure 4.9 is the result of retyping the radius of the end of the slot as 0.15" and displaying a rendered isometric view of the part. The G-code (moved into a smaller pane for clarity on the rendered view) was automatically updated to reflect the new slot width.

Figure 4.9 – Rendered Isometric view of narrower keyhole slot

32426 Rev C1-1 4-5 Using Tormach PCNC 770

4.3.4 Running the G-code

From an Idea to a part

Figure 4.10 – Keyhole loaded and ready to run

The CAM program will write the G-code part-program to disk. Assuming you are using a different computer to design your part from that controlling the machine you need to transfer the file to the hard drive of the control computer. Then you can load and run it in the same way you did for the FirstPart program. Figure 4.10 shows the keyhole loaded into the Control Software.

Note: Do not attempt to run part-programs off a USB key drive or floppy disc.

4.3.5 CAD/CAM Systems

Vectric Cut 2D is a 2½D system which will accept DXF drawings from virtually any source, has powerful features and is very easy to learn. If you already have a favorite CAD program then this will be a good choice for you to do CAM work.

Figure 4.12 – Model for mount

Figure 4.11 – Motor Mount DXF

Figure 4.11 shows a DXF drawing of a mounting plate for a motor. This was produced from the solid model in figure 4.12 but could have been drawn with virtually any program.

Using Tormach PCNC 770 4-6 32426 Rev C1-1

From an idea to a part

Figure 4.13 – Cut2D job for Motor Mount

Figure 4.13 shows the drawing loaded as a Cut 2D job If your work needs more

powerful parametric solid modeling and 3D milling from these models then the matched combination of Alibre Design and SprutCAM is available from Tormach. Figures 4.14 through

4.16 illustrate a part being designed in Alibre, the manufacture being defined in SprutCAM and a finished test piece.

Figure 4.14 – Modelling a 3D part

32426 Rev C1-1 4-7 Using Tormach PCNC 770

From an Idea to a part

Figure 4.15 – Defining the machining technology

Figure 4.16 – The machined test piece

Virtually any other commercially available CAD/CAM systems can be used with the PCNC control software because of its compliance with industry standards. CAD/CAM software is configured to generate appropriate code for a particular machine tool by a post-processor. You should consult Tormach for advice on the best post-processor option to purchase with your preferred software.

Using Tormach PCNC 770 4-8 32426 Rev C1-1

From an idea to a part

4.4 Programming with Wizards

There will be situations when a simple piece of one-off machining has to be performed and you do not have suitable CAD/CAM software or, perhaps, the machine user is unfamiliar with the software that is available. The Wizard facility built into the Control Software is an ideal solution.

4.4.1 Machining Wizard Concept

A Wizard is a special screen that is displayed on demand by the Control Software. It has a series of DROs with which you define the cuts that need to be made. Figure

4.17 shows the general appearance of a surfacing Wizard.

4.4.1.1 Selecting and Running a Wizard

The Wizards>Pick Wizard menu displays a list of Wizards which are installed on your control computer. Wizards can be obtained from a variety of online sources and you can modify a standard one or write your own from scratch. Figure 4.18 shows an example of what the list could contain.

Figure 4.17 – General view of a typical Wizard screen

Click on the Wizard that you want to use and click Run. Notice that a list that is too large to fit in the dialog has a scrollbar but, rather unusually, it is on the left hand side of the list. The Wizard screen will replace the screen currently visible.

4.4.1.2 Standard Wizard Features

Figure 4.19 shows a Wizard for milling a circular pocket.

As many different authors write Wizards, there are detailed differences between the screens but each one should have the following:

• Save Settings button.

This causes the Control Software to remember the values in each DRO so they will be available next time you choose the particular Wizard.

• Post Code button. This causes the Wizard to generate a G-code program to cut the shape

with the sizes you have specified. Most Wizards have a toolpath window and you will see the cuts to be made in it. You can manipulate the toolpath display in the usual way with the mouse (Rotate, Zoom if Shift depressed and Pan if Right-button drag)

Figure 4.18 – Wizard selection list

• Exit button. This returns you to the screen that was displayed before you ran the Wizard

in preparation for running its code.

• An error line and button to Clear the text from it. This will display any problems found

trying to post code using the values that you defined.

32426 Rev C1-1 4-9 Using Tormach PCNC 770

From an Idea to a part

Note: A common problem when filling in the DROs of a Wizard is to forget to press Enter to accept each value. It is easy to type a value and click in the next DRO. This discards the typed value.

4.4.1.3 G-code from a Wizard

You should carefully check the code generated by a Wizard – particularly if it is one which you have not used before.

Things to look out for are:

• Whether the Wizard sets a speed for the spindle (S-word) and starts it and how it controls

the coolant;

• If any motion will conflict with clamps for your work;

• Which position on the work piece the Wizard considers to be X = 0, Y = 0. A good check

is to define Z = 0 to be a plane a few inches above your work piece and do a test run of the Wizard’s code.

4.4.1.4 Commercial Wizards

While many Wizards are bundled free of charge with the PCNC, a set from New Fangled Solutions is a trial version of a product which requires a separate license. You can use all its features to evaluate what the Wizards can cut but, without the license, you cannot actually produce the G-code part-program.

Figure 4.19 – Circular Pocket Wizard

Using Tormach PCNC 770 4-10 32426 Rev C1-1

5. Machine Controls

This chapter gives a description of all the PCNC controls on the operator’s panel

and the Control Program screens.

If you have been through the section “Running the PCNC” in Chapter 2 you

already have a good grounding and may wish to skim through this chapter on

first reading of the manual and come back to it when you want to understand

exactly how some feature works.

5.1 Machine Operation

5.1.1 Operator’s Panel

The operator’s panel is illustrated in figure 5.1. It generally controls the PCNC directly and is independent of the software in the control computer. When the Spindle and Coolant switches are in the Auto position then control of these functions is given to the computer.

Machine controls

Figure 5.1 – Operator's panel

Main Switch

The main switch is mounted on the right hand side of the control cabinet. A padlock can be inserted to lock it in the off position. It controls the power to the main machine and the separate power from the IEC inlet under the control cabinet to the computer and coolant system.

Note: Disconnect the machine from the wall outlets before opening the control cabinet door as it is possible that live terminals can be touched even when the isolator is in the OFF position.

Computer On/Off

This rocker switch controls the power from the IEC inlet to the two outlets that are intended for the computer and monitor. This is provided for convenience. In some applications the computer/monitor might be powered directly from a wall outlet and this “computer” circuit left unused or used for other functions such as to powering a work-light.

32426 Rev C1-1 5-1 Using Tormach PCNC 770

Start and EStop

The Start button will energize the circuits for the axis drives and for the spindle motor. The

Stop button, which locks in once pressed, stops all motion and is the Emergency Stop (EStop)

control. The Stop button is released by a turning the button-head a quarter-turn clockwise. Machine start is protected by a no-volt relay from failure of the mains supply. The PCNC

requires Start to be pressed on re-application of power.

Status LEDs

The Machine LED indicates that the Start button has been pressed. When it is lit then the

Machine OK LED on the computer screen should be solid green.

The Computer LED indicates that the Control Software is running.

Spindle

An important safety interlock is that the rotation of the spindle can be disabled (while maintaining axis drive power) by the Spindle Lockout key-switch. The switch on the beltguard door performs the same function. These are used to ensure that the spindle cannot start when an R8 tool holder is being changed (door open) or when a tool is being changed in a collet chuck.

Machine Controls

Coolant

The controls to the right of the key-switch are all concerned with manual control of the spindle. If the Manual/Auto switch is in Auto position then none of the other panel spindle controls have any effect. In the Manual position the computer cannot control the spindle.

The rotary control potentiometer (RPM x 100) controls the speed on the spindle when it is in Manual mode. Its legend indicates approximate spindle speed in the two pulley ranges.

The Spindle Start spring loaded rocker starts the spindle and the Spindle Stop rocker stops it. The direction is determined by the setting of the Forward/Reverse switch. Forward corresponds to clockwise rotation of the spindle. You can safely switch direction while the spindle is turning.

The Coolant switch controls the power from the coolant pump outlet on the underside of the control cabinet. In the Off position the pump does not run. In the On position it runs irrespective of the computer control. In the Auto position it will run if the Control Program requests coolant.

Accessory Socket

The Accessory socket is for connection of accessories such as a touch probe.

Using Tormach PCNC 770 5-2 32426 Rev C1-1

Figure 5.2 – Holders in the TTS range with collet

5.1.2 Tool Changing

5.1.2.1 Tooling Strategy

The PCNC uses a R8 spindle and so you have access to a vast range of standard tooling. The main options open to you are:

• Tormach Tooling System (TTS) – this

allows you to have all the tools that you commonly use mounted in low cost tool holders and to change them very quickly. The working length of each tool is accurately maintained each time it is loaded into the spindle so it can be used for cutting with no further setup. Tool lengths can be setup and checked in a stores or inspection area without using the PCNC (figures 5.2 &

5.3).

• R8 tool holders – offer similar features to TTS holders but need to be setup once in the

machine and are slower to exchange (figure 5.4).

• Screwed shank cutter collet chuck

(Clarkson/Posilok type) – allows you to exchange a cutter while maintaining a known length as the center hole at the back end of the cutter registers in the chuck (figure

5.5).

• ER or similar collet – accepts a

wide range of cutter diameters but the length of the tool is not accurately repeatable so the offset needs to be reset after each tool change (figure 5.6).

Machine controls

Figure 5.3 – TTS presetting

Figure 5.4 – R8 tool-holder

• R8 collet – gives the shortest overhang from the

spindle nose but requires an individual collet for each tool diameter and, as with ER collets, length is not repeatable.

The tool changing procedure is slightly different depending on the tool-holders you have.

5.1.2.2 Changing R8 Tools

Open the spindle drive cover. Swing the spindle locking fork so

it engages with the flats on the upper part of the spindle. You will have to turn the spindle a little to get it to line-up.

The locked spindle is shown in figure 5.7

To remove any installed tools:

Figure 5.5 – Autolock chuck

Figure 5.6 – ER32 collet tool holder

32426 Rev C1-1 5-3 Using Tormach PCNC 770

Machine Controls

• Wipe any debris from the spindle nose and the tool being removed to avoid any risk of it

getting into the spindle bore;

• Using the supplied 13 mm wrench on the

squared end, loosen the drawbar by about one turn. Tap the end of it with a copperfaced hammer to disengage the R8 taper;

• While holding the tooling in one hand, fully

unscrew the drawbar and remove the tooling.

To insert a new tool:

• Check that the R8 taper on the tool-

holder/collet is quite clean;

• Insert the tool-holder/collet into the spindle

turning it to ensure that the drive keyway engages with the key in the spindle. Start the drawbar thread to retain the tool-holder/collet;

• If you are using a tool-holder then the drawbar can be tightened. Otherwise, using the

drawbar to prevent the collet jaws from closing in the spindle taper, insert the TTS holder or tool into the collet. Then tighten the drawbar.

• Finally disengage the locking forks and close the door.

5.1.2.3 Changing TTS Tools

For more information on the Tormach Tooling system, please review the TTS manual from the Tormach web site titled "31866_TTS_Manual.pdf". For detailed reading on the subject, feel free to read up on "Preventing Collet Slip" in the Engineering Documents section of the web site.

The system uses a precision ¾" R8 collet in the spindle. Insert this as described above for R8 tooling.

Tool holders can be changed by loosening the drawbar by just one turn and using the copperfaced hammer on the squared end to disengage the collet taper. You do not need to remove the collet.

Note: You can change the tools in TTS drill chucks or the ER collet adaptor while these are fitted to the PCNC spindle although doing this will not exploit the pre-settable nature of the tools. You should use both spanners on the ER chuck rather than relying on the holder not turning in the ¾" collet.

Figure 5.7 – Spindle lock fork engaged

If you change a cutter or drill without opening the door to lock the spindle you should use the Spindle Lockout key to avoid any risk of the spindle starting. If the door is open the spindle is automatically inhibited.

Note: the draw bar is a wear part. After many repeated tool changes, the draw bar will become worn both at its threads, and on the shoulder near the top. This wear can adversely affect your ability to tighten tools properly. Inspect your draw bar regularly and replace as required.

5.1.3 Spindle Speed Ranges

The PCNC has two speed ranges. The low range, 175 to 3250 RPM, is suitable for most machining operations with ferrous and other tough materials. The high range, 525 to 10,200 RPM is suitable for small diameter cutters and plastics and non-ferrous materials.

The range change is performed by moving the belt from the motor from the top pair of pulleys (high speed range) to the lower pair (low speed range).

To change the belt position:

Using Tormach PCNC 770 5-4 32426 Rev C1-1

Machine controls

• Open the protective door. Use the

included wrench to loosen the motor mounting plate and the front handle to pull the motor forward. The belt will slacken and can be moved from one pulley to another (figure 5.8). It is slightly fiddly to get the belt through the slot between the bottom pulley and the head casting.

• Retighten the belt so there is

between

" and ¼" belt movement

midway between the pulleys. Lock the motor mounting and stow the handles in the vertical position.

5.2 Screen Control Panels

5.2.1 Using the Screens

Although at first sight you may feel daunted by the range of options and data displayed by Control Software, this is actually organized into a few logical groups. We refer to these as Families of Controls. By way of explanation of the term “control,” this covers both buttons and their associated keyboard shortcuts used to operate the software and the information displayed by DROs (digital read-outs), labels or LEDs (light emitting diodes).

The elements of each control family are defined for reference in this chapter. The families are explained in order of importance for most users.

You should, however, note that all the screens of your system do not include all the controls of a family. This may be to increase readability of a particular screen or to avoid accidental changes to the part being machined in a production environment

5.2.2 Families of Related Controls

Figure 5.8 – Changing spindle speed range

5.2.2.1 Screen Switching Controls

These controls appear on each screen. They allow switching between screens and also display information about the current state of the system (figure 5.9).

Figure 5.9 – Screen switching control family

Reset

This is a toggle. When the system is Reset the LED glows steadily.

Error and Profile Information

The Machine OK LED indicates that the PCNC is started.

32426 Rev C1-1 5-5 Using Tormach PCNC 770

The “intelligent labels” display the last “error” message, the current modes, the file name of the currently loaded part-program (if any) and the Profile that is in use.

The Clear button clears the text from the error line. The entries written to the error line are logged in the file C:\PCNC3\LastErrors.txt. This can be opened and inspected with a text editor like Notepad if you want to analyze a history of events.

Screen Selection Buttons

These buttons switch the display from screen to screen. You are viewing the screen whose label is blue. The keyboard shortcuts are given after the names. For clarity they are letters are shown in upper-case. You should not, however, use the shift key when pressing the shortcut.

5.2.2.2 Axis Control Family

This family is concerned with the current position of the tool, or more precisely, the controlled point (figure 5.10).

The axes have the following controls:

Coordinate Value DROs

These are displayed in the current units (inch/metric = G20/G21). The value is the coordinate of the controlled point in the displayed coordinate system. This will generally be the coordinate system of the current Work Offset (initially 1 – i.e., G54) together with any Tool length offset and G52/G92 offsets applied.

Machine Controls

Figure 5.10 – Axis control family

If the X and Y coordinates display in red then they have been rotated by a G68 command. You can type a new value into an Axis DRO. This will modify the current Work Offset to make

the controlled point in the current coordinate system be the value you have set. You are advised to set-up Work Offsets using the Offsets screen until you are fully familiar with working with multiple coordinate systems.

Referenced

The LED is green if the axis has been referenced (i.e., is in a known actual position). Many users prefer to always run the PCNC in the referenced state.

Using Tormach PCNC 770 5-6 32426 Rev C1-1

Each axis can be referenced using its Ref button or the linear axes can be referenced together

family

using the Ref XYZ button. The De-Ref All button does not move the axes but stops them being in the referenced state.

Scale

Scale factors for any axes can be set by G51 and can be cleared by G50. If a scale factor (other than 1.0) is set then it is applied to coordinates when they appear in G-code (e.g., as X words, Y words etc.) . The Scale LED will flash as a reminder that a scale is set for an axis. The value defined by G51 will appear and can be set, in the Scale DRO. Negative values mirror the coordinates about the relevant axis.

The G50 button executes a G50 command to set all scales to 1.0

Correction Radius

Rotary axes can have the approximate size of the work piece defined using the Rotational Diameter control family. This size is used when making blended feed rate calculations for coordinated motion including the 4th Axis. The LED indicates that a non-zero value is defined.

Jog/Shuttle Axis

The axis that is selected for jogging by the Tormach Jog/Shuttle Controller is indicated by a LED by the top left corner of the corresponding DRO.

Machine controls

5.2.2.3 Jogging Control Family

Jogging can be performed in two ways: (a) using the keyboard (or optional Keypad pendant) or (b) Using the optional Tormach Jog/Shuttle Controller

Keyboard Jogging

Whenever the Jog ON/OFF button is displayed on the current screen then the axes of the machine can be jogged using the jog hotkeys on main keyboard or a pendant keyboard

If the Jog ON/OFF button is not displayed or it is toggled to OFF then keyboard jogging is not allowed for safety reasons.

There are two modes, Continuous and Step which are selected by the Jog Mode button and indicated by the LEDs.

Continuous mode moves the axis or axes at the defined slow jog rate while the hotkeys are pressed.

The continuous jog speed is defined as shown below but this can be overridden by pressing Shift with the hotkey(s). A LED beside the Cont. LED indicates this full speed jogging is selected.

The jogging speed used with hotkeys in Continuous mode is set as a percentage of the rapid traverse rate for the axis and for the Windows compatible joystick as a percentage of the feed for the given stick deflection by the Slow Jog Percentage DRO. This can be set (in the range

0.1% to 100%) by typing into the DRO. It can be nudged in 5% increments by the buttons or their hotkeys.

Figure 5.11 – Jogging control

Step mode moves the axis by one increment (as defined by the Step DRO) for each key press. The current feed rate (as defined by the F word) is used for these moves. The size of increment can be set by typing it into the Step DRO or values can be set in this DRO by cycling through a set of predefined values using the Jog Step button.

32426 Rev C1-1 5-7 Using Tormach PCNC 770

Incremental mode is selected by the toggle button or, if in Continuous Mode temporarily selected by holding down Ctrl before performing the jog.

Tormach Jog/Shuttle Controller

This jogging device is available as an optional accessory (part number 30616, figure 5.12).

Many users will find that it increases their productivity, especially on shortrun jobs requiring a lot of setting up of workpiece and tooling.

The four buttons starting at the left are allocated to select jogging of axes X, Y, Z and A respectively. A LED beside an axis DRO indicates that this axis is the one that will be jogged.

The fifth button cycle through the available jog step sizes. Alternatively you can type a step size into the Step

DRO.

Continuous jogging is performed by turning the spring loaded ring counterclockwise for the minus direction and clockwise for the plus direction. There are seven speeds, in geometric ratio, from very slow to full speed so you can position any axis with great speed and precision.

Machine Controls

Figure 5.12 – Tormach Jog/Shuttle Controller

The inner wheel (with finger dimple) will jog by one Step as defined in the Step DRO for each click. The move will be made at the current feed rate.

5.2.2.4 Spindle Speed Control Family

The machine spindle can be controlled in two ways: (a) by hand or (b) by switching to Auto on Operator’s panel, thus making the speed and direction set by the Control Software.

This control family is only important for case (b). The S DRO has its value set when an S word is used in

a part-program. It is the desired spindle speed. It can also be set by typing into the DRO (figure 5.13).

It is an error to try to set it (in either way) to a speed greater than that displayed in Max Speed for the chosen pulley and the nearest legal value will be chosen.

The Hi/Lo button toggles between the two belt/pulley settings with the LEDs indicating the configuration (spindle on left, motor on right)

The maximum available speed is indicated. The S- and S+ buttons increase and decrease the value

in the S DRO geometrically using a ratio of 1.15 for each click on the button. This reflects the usual arrangement of gearbox in a manual machine tool.

Figure 5.13 – Spindle speed

control family

The spindle can be started in a clockwise direction by the Spindle CW button. An M-code (M4) in the MDI box is required if you want to select counterclockwise running.

Using Tormach PCNC 770 5-8 32426 Rev C1-1

The main LED above the Spindle CW button indicates that the spindle is “running” – although

Figure 5.14

– Feed control family

actual movement may be inhibited by the key and/or door interlocks. The two LEDs that flank it indicate a Dwell while the spindle gets up to speed or fully stops.

The Coolant button and its associated LED control the coolant power outlet under the control cabinet.

5.2.2.5 Feed Control Family

Feed Units per Minute

The F DRO gives the feed rate in current units (inches/millimeters per minute). It is set by the F word in a part-program or by typing into the F DRO. The control software will aim to use this speed as the actual rate of the coordinated movement of the tool through the material. If this rate is not possible because of the maximum permitted speed of any axis then the actual feed rate will be the highest achievable (figure 5.14).

Feed Units per Revolution

As modern cutters are often specified by the permitted cut per “tip” it may be convenient to specify the feed per revolution (i.e., feed per tip x number of tips on tool). In this case the F DRO gives the feed rate in current units (inches/millimeters) per rev of the spindle. It is set by the F word in a part-program or by typing into the DRO.

Machine controls

Notice that the numeric values in the control will be very different unless spindle speed is near to 1 rpm! So using a feed per minute figure with feed per rev mode will probably produce a disastrous crash!

Feed Display

The actual feed in operation allowing for the coordinated motion of all axes is displayed in

Units/min and Units/rev. If the spindle speed is not set and the actual spindle speed is not

measured then the Feed per rev value will be meaningless.

Feed Override

Unless M49 (disable feed rate override) is in use, the feed rate can manually be overridden in the range of 20% to 100% by entering a percentage in the (feed rate override) DRO with a % sign. While it is possible to enter numbers higher than 100%, the practice is not recommended. The LED warns if an override is in operation.

The control software will apply any changes in feed rate override as quickly as possible. This could be very important if you decide you have too high a feed rate for safety. To optimize performance, the software keeps a queue of moves ready to be implemented. It is possible if you increase the federate that you will make one of these queued moves be faster than the PCNC can move or accelerate and so it will loose steps. The best strategy is to write the part program to run at the highest anticipated feed rate and then use the override at less than 100% to reduce it to produce the best operating condition.

32426 Rev C1-1 5-9 Using Tormach PCNC 770

The FRO DRO displays the calculated result of applying the percentage override to the set feed rate.

5.2.2.6 Program Running

Control Family

These controls handle the execution of a loaded part-program (figure 5.15).

Cycle Start

Safety warning: Note

that the Cycle Start button will, in general, start the spindle and axis movement.

Stop

Stop halts axis motion as quickly as possible. Unless used when Paused, it may result in lost

steps and restarting may not be valid.

Machine Controls

Figure 5.15 – Program running family

Rewind

Rewinds the currently loaded part-program.

Single BLK

Single BLK is a toggle (with indicator LED). In Single Block mode a Cycle Start will execute

the next single line of the part-program.

Pause

Pause brings the current move to a controlled stop applying deceleration etc. Although jogging

while paused is possible we do not recommend doing it. The best sequence is to Pause and then press Stop. Resume by editing the program or using the Run From Here feature.

Line Number

Line DRO is the ordinal number of the current line in the G-code display window (starting from

0). Note that this is not related to the “N word” line number. You can type into this DRO to set the current line.

Run from Here

Run from here performs a dummy run of the part-program to establish what the modal state

(G20/G21, G90/G91, etc.) should be and then prompts for a move to put the controlled point in the correct position to for the start of the line in Line Number. You should not attempt to Run

from here in the middle of a subroutine.

Set next line

Like Run from here but without the preparatory mode setting up processing.

Block Delete

The Ignore "/" Blocks button toggles the Block Delete “switch.” If enabled then lines of G-code which start with a slash (i.e., / - will not be executed).

Using Tormach PCNC 770 5-10 32426 Rev C1-1

Optional Stop

The M01 Break button toggles the Optional Stop “switch.” If enabled then the M01 command will be treated as M00.

Goto Toolchange

This button provides manual movement of the controlled point when the part-program is stopped.

Tool Details

Controls display the current tool, its name, the offsets for its length and diameter and whether the offsets are active (ON).

Unless tool change requests are being ignored, on encountering an M6 the Control Software will stop and flash the Change Req LED. You continue (after changing the tool) by clicking

Cycle Start.

Work Offset Details

The name of the current work offset coordinate system is displayed.

Machine controls

5.2.2.7 Toolpath Control Family

The currently loaded part-program is displayed in the G-code window. The current line is highlighted and can be moved using the scroll bar on the window (figure 5.16).

The Toolpath display shows the path that the controlled point will follow in the X, Y and Z planes. When a part-program is executing, the path is over painted in green. This over painting is dynamic and is not preserved when you change screens or indeed alter views of the toolpath.

On occasions you will find that the display does not exactly follow the planned path. This occurs because the Control Software prioritizes the tasks it is doing. Sending accurate step pulses to the machine tool is the first priority. Drawing the toolpath is a lower priority. It will draw points on the toolpath display whenever it has spare time and it joins these points by straight lines. So, if time is short, only a few points will be drawn and circles will tend to appear as polygons where the straight sides are very noticeable. This is nothing to worry about.

The Simulate Program Run button will execute the G-code, but without any tool movement and allow the time to make the part to be estimated.

The Absolute Motion Extremes data allow you to check if the maximum excursion of the controlled point is reasonable (e.g., not milling the top of the table).

The toolpath display can be rotated by left clicking and dragging the mouse in it. It can be

32426 Rev C1-1 5-11 Using Tormach PCNC 770

Figure 5.16 – Toolpath and G-code display

family

zoomed by shift-left clicking and dragging and can be panned by dragging a right click. The Regenerate button will regenerate the toolpath display from the G-code with the currently

enabled fixture and G92 offsets. The Display Mode button will chose whether the default toolpath display is sized for the

machine envelope (as defined by the “soft limits”) or the object defined by the extremis of the part-program.

The Jog Follow button allows the toolpath display to be automatically scrolled as the controlled point is jogged.

5.2.2.8 File Control Family

These controls are involved with the file of your part-program. Most should be self-evident in operation.

Change G-code allows you to use the Notepad editor to edit the part-program you have loaded.

When clicked it displays the current file (figure 5.18).

Machine Controls

Figure 5.17 – File control family

5.2.2.9 Work Offset and Tool Table Control

Family

This family is explained in detail in Chapter 6 (figure 5.19).

5.2.2.10 MDI and Teach Control Family

G-code lines (blocks) can be entered, for immediate execution, into the MDI (Manual Data Input) line. This is selected by clicking in it or the MDI hotkey (Enter). When the MDI line is active its color changes and a fly-out box showing the recently entered commands is displayed (figure 5.20). The cursor up and down arrow keys can be used to select from the fly-out so that you can reuse a line that you have already entered. The Enter key causes the current MDI line to be executed and the MDI remains active for input of another set of commands. The Esc key clears the line and de-selects it. You need to remember that when it is selected all keyboard is written in the MDI line rather than controlling the machine. In particular, jogging keys will not be recognized – you must Esc after entering MDI.

Figure 5.18 – Notepad++ to edit G-code

The Control Software can remember all the MDI lines as it executes them and store them in a file by using the Teach facility. Click Start Teach, enter the

Figure 5.20 – MDI and Teach control family

required commands and then click Stop Teach. The LED blinks to remind you that you are in Teach Mode. The commands

Using Tormach PCNC 770 5-12 32426 Rev C1-1

are written in the file with the conventional name C:/PCNC3/GCode/MDITeach.tap. Clicking Load/Edit will load this file so it can be run or edited in the usual way – you need to go to the Simple Run or Comp Run screen to see it. If you wish to keep a given set of taught commands then you should Edit the file and use Save As in the editor to give it your own name and put it in a convenient folder.

5.2.2.11 Loop Control Family

The Control Software can execute a partprogram many times, automatically updating a limit to the depth to which the Z-axis can move (figure 5.21).

Machine controls

The part-program must end with an M30 (rewind) code.

The number of passes you require is entered into the Cycles DRO. The initial lowest Z position is put into Z inhibit (note this will often be negative) and the distance Z is to move down each cycle is put into Z Step (usually positive). The On/Off button enables the feature.

The Multipass button will prompt for the values by a series of dialogs rather than requiring the DROs to be filled in.

5.2.2.12 Modes and Mode Alarm Control Family

These families display the current modes of the Control Software and an “alarm” LED for unusual modes. The alarm is on the Diagnostics screen. Click on the flashing LED to see a list of unusual modes (figure 5.22).

Figure 5.22 – Current modes display

These modes might arise from running a part-program produced by a CAD/CAM system not customized for all the features of the PCNC.

Figure 5.21 – Loop control

An unusual mode does not imply a fault in your system, simply a hint of what to look for if unusual things are happening (figure 5.23).

If for any reason the standard modes do not suit your normal working then by

Figure 5.23 – Unusual modes display

on Diagnostics

double-click on the unusual modes LED you can define the current state as “usual.”

5.2.2.13 Rotational Diameter Control Family

As described in the Feed Rate control family, it is possible to define the approximate size of a rotated work piece so the rotational axis speed can be correctly included in the blended

Figure 5.24- Rotational diameters

feed rate. The relevant diameters are entered in the DRO on this family (figure 5.24).

The Axis control Family has a warning LED to indicate the setting of a non-zero value here. Note: A value is not required if rotary movement is not to be coordinated with linear axes. In

this case a suitable F word for degrees per minute or degrees per rev should be programmed.

32426 Rev C1-1 5-13 Using Tormach PCNC 770

Machine Controls

5.2.2.14 Toolchange Position Control Family

This family defines the place the machine should go to when a request to change a tool occurs or when the Goto Toolchange button is clicked. A part-program can go to it by using the M998 code (figure 5.25).

The position is defined in machine coordinates (i.e., relative to the home switches) and in the default machine units.

Enter the special value 9999 if you do not want a given axis to move when a tool change is requested.

The units in which you define your toolchange position can be configured by the Toggle T/C Units button.

Note: The move will take place correctly whatever units the machine is in at the time and, because machine coordinates are used, to a fixed place irrespective of the offsets in use.

Figure 5.25 – Tool change position

The tool change position is also used when you want to use the central lubrication system. This family also allows you to set the machine coordinates used if your part-program executes a

G28. We advise you to use the M998 toolchange location whenever possible as this checks that the machine is referenced (i.e., the machine coordinates are valid). G28 will use whatever values are in use irrespective of them being valid because the machine is referenced.

5.2.2.15 Inhibits and Overrides Control Family

In testing a part-program it is sometimes useful to be able to inhibit the movement of an axis (e.g., typically Z). This is done with the Axis Inhibit buttons (figure 5.26).

When an axis hits a limit switch it will trigger a software EStop condition so all movement will cease. If Auto LimitOverRide is enabled then you can reset the system and carefully jog off the limit. If you want more security in this situation you can disable AutoLimitOverRide and click the OverRide Limits button before clicking Reset on each occasion.

5.2.2.16 Feeds and Speeds Calculator

Different materials and tooling require different cutting speeds and feed so you will need to use published tables and your experience to define the optimum spindle speed and the feed rate for any given job. A simple calculator on the Settings screen will, however, do the math for you when you know a cutting speed (in feet per minute) and a chip per tooth loading (figure 5.27).

Figure 5.26 – Inhibits and overrides family

Enter your cutting data into the DROs, not forgetting to press Enter for each value and click the Calc

RPM/Feed button. The screen labels

show the calculation that is being

Using Tormach PCNC 770 5-14 32426 Rev C1-1

Figure 5.27 – Speed/Feed calculator

done for you.

5.2.2.17 Tapping Configuration Family

The control software allows use of the Tormach Tapping Heads (PN 30612 and 30613) without a detailed understanding of the sequence of moves that are needed to control the head. The holes are tapped by using one of the M-code macros M871, M872, M873 or M874. The macros work as a kind on canned cycle. Each macro is set up for a particular pitch of thread and choice of tapping head. This information is provided by the Tapping Configuration family of controls (figure 5.28).

The TPI or Pitch DRO is interpreted in a different way depending on whether the part program calling its macro is running in Inch (G20) or metric (G21) mode. In G20 mode the value is a number of threads per inch and in G21 mode it is the pitch of the thread in millimeters. It is perfectly possible to change modes within a program and so have a job with mixed thread standards. Fortunately Inch numbers are unlikely to be pitches and vice-versa. The control software checks that the chosen pitch can be cut at the current spindle speed when the macro is called so there is little chance of damage to a tap.

Machine controls

Figure 5.28 – Tapping Configuration

If you select Dwell mode then the macro will use an alternative movement algorithm which dwells (pauses) at the bottom of the thread. This gives a more accurate depth but slower tapping and more wear on the mechanism of the tapping head.

Both tapping heads have a high-speed reverse feature to minimize tapping time. As the gear ratios are different for each head you must define which is going to be used by toggling to the appropriate large or small LED.

5.2.2.18 Misc. Settings Control Family

Current Units

This displays the units currently selected (figure 5.29).

Ignore Tool Change

Normally when the part-program calls for a different tool execution will stop, the Tool Change LED will flash and you need to press Cycle Start to continue. Tool change requests can be ignored by clicking the

Ignore M6 Tool Change button. This can be useful when air-cutting to prove/time a part

program.

Figure 5.29 – Misc. settings

G73 Pullback

This DRO defines the distance that a high speed peck drill cycle (G73) will pullback when breaking the chip. You may need to alter this value for metric use.

32426 Rev C1-1 5-15 Using Tormach PCNC 770

IJ Mode

The IJ mode defines how the I, J and K words in a G02 or G03 are interpreted. There is no standard for this so different CAM post processors will use different conventions. The PCNC usually runs with I, J and K being incremental distances from the current point. You can make the Control Software treat them as absolute positions by clicking the Set Abs I/J button. The symptoms of an incorrect setting are that small arcs can display a massive circle on the toolpath or you get an error message about the radius of an arc being different at the start and end of a cut.

5.3 USB Jogging Pendants

Optional accessories purchased by many users are the USB jogging pendants. These provide access to the main axis jogging controls on a unit that can be positioned for use while touching-off the tool position. They are not resistant to coolant and, for safety reasons, do not have controls for starting and stopping machining.

The pendants should be plugged into USB ports on the computer motherboard. We have found connections through hubs can lower responsiveness.

Machine Controls

Figure 5.30 – Jog Wheel pendant

5.3.1 Jog/Shuttle Controller

The Jog /Shuttle Controller is a low cost but very precise and fast way of jogging the four axes. There are five buttons and two rotary controls (figure 5.30).

The buttons allow you to select which axis you wish to jog. The chosen axis is indicated by a LED next to the corresponding DRO. For example, figure 5.31 shows that the X-axis is the one to be jogged. If a Jog/Shuttle Controller is not installed then all the LEDs will be dark.

The Step button will cycle through a set of jog step sizes in the Step DRO in the Jogging family. The available preset step sizes can be customized with XMLTweak (see chapter 9)

The outer rotary shuttle control is spring-loaded. Turning it will jog the selected axis at a speed proportional to the amount it is turned. There are seven different speeds arranged geometrically so you have instant control from the full rapid speed (65 rpm) down to the slowest crawl.

The inner rotary control, operated by fingertip, has detents. Each click will jog at the current feed rate by the distance defined in the Step DRO. If you turn it faster than the axis can move the impossible steps will be ignored so the axis will never buffer up a backlog.

Figure 5.31 – X-axis will be jogged

5.3.2 Keypad Pendant

The keypad pendant has two modes of operation. The CNC/Num key toggles between these modes (figure 5.32).

When the Numeric LED is lit it is a conventional numeric pad. It can be used for entering values into DROs. Note that as Backspace in not available on the main keyboard during DRO entry it cannot be used on the pendant either.

Figure 5.32 – Keypad pendant

When the LED is not lit the majority of the keys are

Using Tormach PCNC 770 5-16 32426 Rev C1-1

Machine controls

concerned with jogging the four labeled axes (X, Y, Z and A – keys 2, 3, 4, 6, +, 8, 9, - ) The 7-key will perform a Home All operation (homing Z to limit switches and then X and Y). The 1-key will toggle the state on the Optional Stop LED. When the LED is lit, M01 is treated

exactly like M00 (i.e., end program), otherwise M01 is ignored. The /-key toggles between Continuous and Incremental (or Step) jogging modes. In step, one

key press produces a single step axis movement. The step size is displayed in a DRO. The *-key (labeled Size) cycles through the available Increment (Step) sizes.

32426 Rev C1-1 5-17 Using Tormach PCNC 770

Offsets

6. Using Multiple Tools

This chapter explains how you can configure the PCNC to use several tools

without having to waste time at each tool change defining the length of the new

tool. It also covers techniques for simplifying machining of work in a vise or

other fixture.

Offsets used are often considered as advanced features but the design of the

PCNC Control Software should make them easy to use. You will find it

worthwhile to master this chapter even if it needs more than one reading to do

so.

6.1 Offsets and Coordinate Systems

If you made the FirstPart then you will already have met and used the ideas explained in this section.

When you Reference the PCNC, when it is started, the X-, Y- and Z-axes are moved so that they are just off the home switches and the machine coordinates are set to 0.0. We saw that this is not useful when you want to run a part-program as the program will have its own view of where zero should be; in the case of FirstPart this is the top left corner of the material for X = 0, Y = 0 and the top surface for Z = 0. By moving the tool to this position and zeroing the axis DROs you defined relationship between the Machine Coordinates and the coordinates which the part-program would use – the Program Coordinates. The general term for the relationship is Offsets.

6.2 Tool Length Offsets and the Tool Table

For a given machining operation the X and Y position of the workpiece will be fixed. However you will often need to use several tools and as these will be different lengths then you need to change the Z offset. The control software allows you to switch tools quickly and without the need to set up the machine every time a tool is mounted. Each tool and holder only needs to be “measured” once, either offline or in the machine.

If you do not have enough holders for all the tools for a job then you will need to set the Z work-offset each time you load a new tool. Using the tool table is only useful if you can put each tool into the spindle in a fixed position. Skip this section if you do not want to use the tool table.

The following example demonstrates a typical sequence using the Tormach Tooling System and setting up a “touch off” tool and 3 cutting tools in the tool table.

6.2.1 Example Operation of Multiple Tools

The following example has three simple steps

1. Fill the tool table with the tools

you plan to use

2. Zero to the work height

3. Apply the tool offset

32426 Rev C1-1 6-1 Using Tormach PCNC 770

Figure 6.1 – The set of tools

6.2.1.1 To fill the table:

Figure 6.2 – Open tool table

• Select the three tools to use, we'll use the touch off tool as #1 and the cutting tools of drill,

end mill, and face mill as #2, #3 and #4

• Use the Config menu to open the tool table (figure 6.2) . It will look something like figure

6.3

• Using the TTS height gauge, the standard spacer and the granite block, measure the tools,

adding each one’s name and length to the table. The touch tool (#1) length is measured

Offsets

Figure 6.3 – Tool table

Figure 6.4a

Figure 6.4b

Figure 6.4c

Figure 6.4d

when the dial indicator pointer reads 0.

• Here are the measurements we took:

Tool Number Description Height Tool #1 Touch Tool 7.084"

Tool #2 Drill 3/16" 7.151" Tool #3 End Mill 3/8" rougher 4.396" Tool #4 Face Mill 1.5" face 4.115"

The completed table will look like figure 6.5. Note: The Diameter Wear and Height Wear values in the table should have data in them as they

are ignored by the current version of the control software.

Using Tormach PCNC 770 6-2 32426 Rev C1-1

Offsets

Figure 6.5 – Data in tool table

Note: The values in this table are always in inches. If you want to input tool lengths in millimetres then you can do this when you are in metric (G21) mode by using the tool length part of the Offsets screen.

If you change a tool, for example by sharpening it, if it comes loose in its holder or fitting a new cutter, then you must make sure you re-measure it on the granite block and update the tool table.

6.2.1.2 Zeroing to work height

Here you are going to set the work offset of Z so tool #1 is touching the top of the work when Z = 0.0. As the tool table gives the lengths of all tools that means Z will be zero when each tool in on the spindle and selected from the tool table by its number.

• Mount the touch tool (#1) in the spindle

• Set the current tool by typing 1 (followed by Enter) into the DRO labelled T

• Jog the Z axis down so the dial indicator touches the top of the work and reads 0.0 (i.e. the

Figure 6.6 – Selecting tool #1

Figure 6.8 – Setting work offset so Z = 0.0

Figure 6.7 – Dial zero touching work

32426 Rev C1-1 6-3 Using Tormach PCNC 770

Offsets

position of the pointer when you measured the tool length – remember the tool is upside down now relative to when you measured it) (figure 6.7)

• Click the Zero button on the Z Axis DRO (to set the work offset) (figure 6.8)

6.2.1.3 Using tool #2

• Set the value 2 in the T DRO.

• Mount tool #2 in the spindle.

The Z axis DRO now reads the distance between the tool tip and the work.

6.2.1.4 Using other tools

Repeat the above for any tool number that you have defined in the tool table

6.2.1.5 Changing to a different work-piece

All you have to do is repeat the Zeroing to work height process with the touch off tool when you have clamped another work-piece in the vise or on the table.

6.2.2 How this multiple tooling setup works

As explained above the machine works with two types of coordinates: Machine coordinates are really an internal function of the machine. It's the machine's way of

Figure 6.9 – A possible way of measuring coordinates

Using Tormach PCNC 770 6-4 32426 Rev C1-1

Offsets

keeping track the positions of its parts, like the height of the spindle head. Program coordinates are what we worry about. Program coordinates are what shows up in the

normal axis DROs and they are the positions that most G code commands reference. The conversion between program coordinates and machine coordinates is done by the offsets.

They apply to all linear axes, X, Y, Z and the rotary axis A. The way offsets work in Z is shown in figure 6.9.

In the image above, it should be clear that the following equation applies:

Program Coordinates + Work Offset + Tool Length = Machine Coordinates

The tool length comes from the tool table. The work offset comes from the work offsets table, also sometimes called the fixture table. There 255 different work offsets available. The first few are called by G54 through G59. You can do virtually all straightforward machining using just the one default work offset system (G54). You only need multiple systems if you decide to use more than one vise or other complex fixturing clamps. We will talk more about the work offsets later.

When we used the Z axis Zero button with the tool touching the top of the work, what happened is that current value of the Program Coordinate was added to the current work offset. For example, if we had the following before pressing the Zero button.

Program Coordinate + Work Offset + Tool offset = Machine Coordinate

3 +

2 + 4 = 9

Then after the Zero button was pressed we would have the following result:

Program Coordinate + Work Offset + Tool offset = Machine Coordinate

0 +

5 + 4 = 9 so making the program coordinates of the top of the work be zero as is conventional for most programs.

Figure 6.9 shows the top of the table as being machine zero. This is arbitrary. We could have chosen the top face of the stand and the diagram would have looked very similar – just that the work offset and machine coordinates for the given head position would have been bigger.

In practice the zero position of the referenced machine is chosen to be where the head stops after clicking Ref

Z i.e. just below the Z limit/home switch (figure 6.10).

This means that in normal use all Z machine coordinate values will be negative numbers and the work offset

Figure 6.10 – Actual machine zero

values will be negative too. The arithmetic of the equation

Program Coordinates + Work Offset + Tool Length = Machine Coordinates

works fine with the negative values but it is not possible to draw a simple sketch like figure 6.9. The fact that machine zero can be anywhere and the work offset relates it to the work location

explains why it is possible to use the machine un-referenced. In this case machine zero can be anywhere; below the floor, up in the roof space, etc. The work offset value when you have touched the tool on the top of the work will make this position be program coordinate Z = 0.0.

6.2.3 Programming, Buttons, or Direct Entry

The example above shows the tool being selected directly through typing a number into the tool DRO.

32426 Rev C1-1 6-5 Using Tormach PCNC 770

Offsets

You can also command the tool change by entering directly into the MDI line. Specifically when switching to tool number n, enter Tn M6 G43 Hn on the MDI line. M6 is the command to do a tool change and T indicates the tool number to use. G43 says that a tool length offset must be be applied with H giving the offset length to use – this is usually the same as the number of the tool you have chosen. As an example, if you want to change to tool #21, the command would be:

M6 T21 G43 H21

If you're creating a G&M code program by hand, in a text editor, this sort of line will be needed when your code intends to command a switch from one tool to the next. If you develop your code using a CAM program, your CAM program will automatically insert this line.

6.3 Alternative Methods Setting Up Tools

The previous section showed you how to measure tools and set up the tool table if you have the Tormach Tooling System (TTS) and its touch tool. Working this way is easy to explain and understand as well as allowing you to set up tools for the next job while using the machine to run a job. Offline measurement is common in professional toolrooms but TTS is one of the few systems making it available to small ‘shops.

This section describes ways of using the mill itself to measure tools and is applicable to standard R8 tooling which is difficult to measure offline.

It can, of course, also be used with TTS if you do not wish to measure offline. You must however be consistent with the method you use. You cannot measure some tools offline and some online. The reason for this is that any measurement is based on a reference or datum position. In TTS the datum is the cylindrical ground spacing piece in which the tools stand. When measuring online you have to consider one of your tools to be the reference or “master” tool.

6.3.1 Measuring techniques

Now it is time to go from the theory of coordinate systems to the very practical choice of the best ways of finding where a tool is in relation to stock which you want to machine. We will look at ways of measuring tool position and then how you use these measurements to set up the PCNC.

We will concentrate for the present on the position of the Z-axis. There are several reasons for this:

• The Z dimension is often the one

with the highest accuracy constraints because the stock is often oversize in both dimensions in X and Y and is, at any event, not easy to locate precisely on the table.

Figure 6.11 – "Roll-your-own" gauge in use

• The Z direction is not only important for setting the initial position of the stock it needs

to be accounted for when using several tools which are, almost inevitably, of different lengths.

Note: We assume that the top surface of your work-piece is the plane Z = 0.0.

Using Tormach PCNC 770 6-6 32426 Rev C1-1

6.3.1.1 “Roll-Your-Own” Gauge Method

This is a time honored machinists’ method which traditionally used Rizla or similar cigarette paper as a gauge. The plastic foil from candy wrapping is a good substitute. Both materials are fairly strong and around

0.002" in thickness. Jog the tool very carefully down to the

stock with a piece of paper/foil on it (figure

6.11). You will be able to feel when the paper/foil gets trapped.

You then know that the tool is 0.002” (two “thou”) above the stock.

The advantage of this method is that you will always be able to “find” a gauge and it can be used on a very small flat surface on the stock (e.g., the boss of a casting). The disadvantage, particularly with hard stock and brittle tools (e.g., carbide) is that it is easy to jog down too far and damage the tool cutting edge.

Offsets

Figure 6.12 – Tool much too low for gauge

6.3.1.2 Roller Gauge Method

For this method you need a short length of rod of a known diameter (¼" is quite suitable for most jobs). The shank of a twist-drill can be used in an emergency but take care to use one without scoring on it and measure the diameter rather than assuming it is the nominal size of the drill.

Jog the tool so it is clear of the stock but no more than the gauge diameter above it. You will be unable to roll the gauge under the tool (figure 6.12). While attempting to roll the gauge into the gap, very slowly jog upwards. You will easily feel the point where the gauge rolls under (figure

6.13). If you jog too far then it is easy to remove the gauge, jog down a little and try again.

You know that the tool is the diameter of the gauge above the stock.

Figure 6.13 – Gauge just rolls under tool

Figure 6.14 – Parallel adjusted to gap

The advantages of this method are that you do not risk crashing the tool into anything. If you are repeatedly gauging, (say multiple tools) then you do not have to keep typing a measurement into the Control Program. One disadvantage is that any backlash in the Z axis will cause an error as you are jogging on the other side of the backlash from that when a cut has been applied. You also need to be able to jog slowly to get an accurate result. The Jog/Shuttle device is very convenient on account of its variable jogging speeds..

32426 Rev C1-1 6-7 Using Tormach PCNC 770

6.3.1.3 Adjustable Parallel Method

You need an adjustable sliding parallel gauge.

Jog by eye so that the tool is about the nominal size of the parallel. Insert it in the gap between tool and stock, slide it to fill the gap and lock it off (figure

6.14). Carefully remove the parallel and

measure it with a micrometer or caliper (figure 6.15).

The advantage of this method is that you do not need any careful jogging. The disadvantages are the need to measure the parallel and then to accurately type the result, which will generally be an awkward number, into the DRO.

You can of course use a combination of these methods depending on what you have to hand on a job and which is most convenient.

Offsets

Figure 6.15 – Measuring the parallel gauge

6.3.2 Comments on Accuracy

With practice you will be able to use these methods to measure to better than 0.001". It is, however, interesting to look at other issues which affect the accuracy of your work.

The PCNC is a rigid machine and is fitted with precision anti-backlash ballscrews and laser aligned in the factory so is inherently very accurate. You do however need to consider the following points:

• You are measuring at one point on the stock. If its surface in not flat or it is not

clamped exactly parallel to the table then the height at other places will be different.

• A change of 40oF in the temperature of a ballscrew (say between early morning in the

winter and when the shop and machine has heated up in the afternoon) will amount to a difference of around 0.004" when the tool is near the table at the bottom of the Z-axis.

General Accuracy Issues

6.3.3 Working without the tool table

You do not need to use the tool table. If you hold your tools by a method which does not give a consistent length (e.g. exchanging

tools in a collet) then you will not be able to use a tool table.

Using Tormach PCNC 770 6-8 32426 Rev C1-1

If you have work which is generally one-off and you use a very wide range of tools (e.g. many

Figure 6.16

– Gauge size entered to DRO

different drill diameters) then it is probably not worth the trouble of setting up the tool table. To work without a tool table you merely reset the Z axis work offset value each time you

change the tool.

6.3.3.1 Direct Entry to Axis DRO

All the measurement methods give the current position of the tool relative to the stock, assuming the face you have measured to is to be zero in the program coordinates, all you need to do is to type the value into the relevant axis DRO. You can do this on any screen.

For example after using the adjustable parallels (figure 6.15) and without moving the axis, you would enter 0.547 into the Z-axis DRO (figure

6.16). The program coordinates say Z = 0.547 and the tool is 0.547" above the stock so, for example,

G00 Z0.0 will move the tool so it exactly touches the stock. You may have noticed that in making FirstPart we cheated a little by assuming the paper

gauge was zero thickness. This is often sufficiently accurate and allows use of the Zero buttons rather than typing a value.

Offsets

6.3.3.2 Using the Touch Buttons

The “roll-you-own” and roller gauge methods will always give you the same measurement to be typed in. On the Offsets screen you can do this once and use it each time you want to set-up an offset.

The gauge thickness is typed into the Touch

Correction DRO on the Offsets screen. Figure

6.17 shows this being set for the ¼" roller gauge. Note the correction is also enabled as shown by the LED by the On/Off button.

When the gauge is in place, clicking the

Touch button for the axis will set the offset. Figure 6.18 shows the program coordinates after

Touch on Z-axis.

Figure 6.17 – Entering roller gauge size

32426 Rev C1-1 6-9 Using Tormach PCNC 770

Figure 6.18 – Touch done on Z with roller gauge

6.3.4 Tool Table with General Tooling

With conventional tool holders you will not be able to measure them with a height gauge (unless, of course, you make your own dummy R8 spindle nose). The following procedure uses the PCNC as a measuring rig.

Note: If you follow these instructions very carefully you can mix tool entered into the tool table by measuring on the TTS granite block with those measured in the machine. We suggest, however that you do not mix the two methods. If you want to use TTS and R8 tools on a job the just measure all of them on the machine as described below.

Mount a piece of flat stock on the table or in a vise on the PCNC. Work throughout on the Offsets screen.

If you have some TTS tools preset in the tool table then one of these must be the master tool. If you have R8 tooling choose one that you do not expect to wear much in use to be tool #1. This is termed the master tool

Load the master tool, select tool #1 (or tool #0 if you have a non-cutting master) in the T DRO. If it is a TTS tool and so already in the table then its length should be shown as in the Length DRO. If it is not in the table them type 0.0 in the Length press Enter to accept it.

Offsets

Figure 6.19 – Setting up a

conventional

tool holder as tool #4

Now set the work offset with it touching the work to Z = 0.0 by any of the gauging methods described above.

Now jog the Z-axis so you can load each tool holder in turn. Enter its number into the T DRO. Jog and gauge (by any of the touching methods already used) but instead of entering the gauged position into the Z-axis DRO you must always enter it into the Touch Correction DRO and click the tool Touch button marked Length – not any of those in the Work Offsets column. For completeness, enter the diameter of the tool in the Tool Diameter DRO. Do not forget that you have to press Enter to accept values typed into DROs.

What you are doing is setting the lengths of all the tools relative to the Master Tool. Figure 6.19 shows this having been done for tool #4.

6.3.5 Tool table with the Tool Setter

If you have the Tormach Tool Setter then this can easily be used to set entries in the tool table. Details are given in Chapter 8 (figure 6.20).

Figure 6.20 - Toolsetter

6.4 Comments on Tool Offsets

If you do not save the Tool Table then, when you close down the Control Program, you will be asked if you want to save it. Unless you have made a serious error in setting up tool offsets you should save them or you will have to enter them again next time you run the Control Program.

Using the T DRO on a screen is a very easy way of changing a tool. The process is more complex in a part-program. This is because the RS-274 standard part-programs can run on large

Using Tormach PCNC 770 6-10 32426 Rev C1-1

CNC systems with complex automatic tool changers. The RS-274 process consists of choosing the next tool to use with a T word, Loading the tool with M06 and applying its offsets with G43. The required commands will be generated by CAD/CAM systems and the Wizards. We strongly advise you to put all three stages (T~, M06 and G43 H~) on one line in you program and to check that the post processor of your CAM system does this. If you do not follow this "Triplet Rule" then you will encounter problems if you mix using tool lengths in the tool table and just setting the work offset when you change a tool.

6.5 Setting X and Y Offsets

The X and Y offsets allow the actual position of you work on the table to be converted to the machine coordinates whenever a movement is required. It is usual to the top left coner of the work-piece to be used in the G-code as X = 0.0, Y = 0.0. If your code uses another convention then set 0, 0 to the place used in your code.

6.5.1 By eye

It is sometimes quite acceptable to define the program coordinate zeros by eye as was done for FirstPart.

Move the tool to be above the point you want to be X = 0.0 and click the Zero button by the X axis DRO (on any screen). Now move the table so the tool centre is above the position to be Y = 0.0 and click

Zero by the Y axis DRO. You can if you prefer just

type 0 (followed by Enter) into the DRO and Y = 0.0 and

Offsets

There are useful techniques when more accuracy is required.

6.5.2 With a Probe

By far the most accurate and often the quickest way of setting X and Y offsets to a piece of stock material or to a part-machined component is with a probe such as

Figure 6.21 – The Tormach probe

that illustrated in figure 6.21 Full details of the support for this accessory are given in chapter 8.

6.5.3 Measuring Off an Edge

Any of the above gauge methods can be used with a “tool” touching the edges of the stock or equally usefully the jaws of a vise used to hold the stock.

It is not really practicable to use a cutter because the spiral flutes do not give a clear place to gauge to. A cylindrical bar (e.g., ½" diameter) is ideal. It should be mounted in a tool holder so that it runs true. It is slightly easier to feel the contact point if a spherical finder is used. This is shown in the illustrations below.

Figure 6.22 show the measurement of the coordinates on the corner of the fixed jaw of a machine vise.

32426 Rev C1-1 6-11 Using Tormach PCNC 770

Figure 6.22 – Measuring vise jaw Y position

Offsets

The value to be use in the Touch Correction DRO (or entered in the axis

DRO) is half the diameter of the probe tool plus the measurement of the gauge. In the illustrated setup the ball has a diameter on 0.369" so with 0.002" foil the correction is numerically -0.1865".

The same technique can obviously be used on the edges of a piece of stock clamped to the table.

Note: You need to be careful about whether the correction is plus or minus. In the case of the vise jaw it is negative (the center of the tool is actually nearer to 0.0 that the touching point). For the outside of a workpiece it should be positive. Thus in the example illustrated, the value typed into the Touch Correction DRO will be -

0.1865 (figure 6.23).

6.5.4 Laser Centering Techniques

If you need to setup the X and Y program coordinates to features marked on, or already machined in, the workpiece then a laser finder or centering microscope is very useful.

Figure 6.24 shows a laser finder located near a center-punch mark on the stock. The point of light can be more clearly seen in the close-up view (figure 6.25)

Viewing the feature through a centering microscope has the same effect although the height of the Z-axis is then much more important as it affects the focusing of the microscope.

Figure 6.23 – “Inside” corrections are negative

Figure 6.24 – Laser finder on scribed mark

Obviously no correction is needed for the position as the beam is where the center of the tool will be.

6.6 How Work Offsets work

We have shown you several uses of offsets. This section gives a summary of how they work internally.

As explained above the PCNC keeps track of the absolute position of all axes. If it has been referenced then these will be measurements relative to the home switches on the X, Y and Z axes. It it has not been referenced then the machine coordinates will be arbitrary.

Machine coordinates are useless for

Figure 6.25 – Close-up of spot of light

programming the machine as you will not

Using Tormach PCNC 770 6-12 32426 Rev C1-1

Offsets

know when designing a part what they will be at a datum position (e.g. one corner of the part. This is why you define a relation between the Program Coordinates and Machine Cordinates..

Figure 6.26 – Illustrating Program and Machine coordinates

This relationship is just a series of Offsets. The offsets are numbers which are added by the Control Software to your program X, Y, Z coordinates to get the machine coordinates.

Figure 6.26 is a view of part of the Offsets screen. You will probably find it useful to look at this screen on your machine as you read this material. The machine is set-up in Inch (imperial units). If your machine is set-up for metric units then you can either experiment with the same numbers as we use or, of course, roughly convert them to inches

To obtain figure 6.26 the PCNC was referenced (notice the green “referenced” LEDs at right of screen) and a tool jogged to the surface of a piece of stock just touching the surface at the

Figure 6.27 – Axis DROs corresponding to

figure 6.26

top left corner. So you can imagine it, let us say that the jogging moved the Z-axis down about 9.5", the tool 3" to the right and 2.5" towards the front of the machine.

The Zero button for X-, Y- and Z-axes was clicked (we could have typed 0 into the axis DROs with exactly the same effect). The Manual Data Input (MDI) was then used to go to the program coordinate position X = 1, Y = -1.4 and Z = 0.5 by:

G00 X1.0 Y1.4 Z0.5

Figure 6.27 shows the axis DROs that you would see, while the whole story is shown in figure

6.26. Let us use X as an example. The program coordinate for the tool is currently X= 1.0 (we did a G00 X1.0). The offset to be added to this to get the machine coordinate is 3". Adding these two values together gives the machine coordinate value of 4. These numbers are nice round values in practice if you jogged exactly to the top left corner of the stock they will have a decimal fraction part (e.g. 9.076).

Now look at Z. The jog was about 9.5" down but we put the tool exactly on the surface of the stock. The program coordinate is Z = 0.5 (from the G00 Z0.5). The Z offset value is actually

-9.5. Adding the program coordinate to the offset gives the machine coordinate of -9.0. This is of course the distance that the head currently is below the home switch position. It may seem strange at first when you have negative numbers. All you have to remember is that a sum:

4.3 + (-2.1) is identical to 4.3 – 2.1 The offsets we have been setting are called Work Offsets as they are different for each piece of

work loaded onto the machine. The Z offset includes the length of the tool. If you change the tool then you would have to jog so the new one is just touching the work and click Zero again.

32426 Rev C1-1 6-13 Using Tormach PCNC 770

In the next section we will see how another sort of offsets, Tool Offsets, can allow for the different projection of different tools from the spindle nose.

You are probably wondering how you can jog so that the spindle axis (i.e. the centre of the tool) is exactly over the corner of a work-piece (to set X = 0.0 and Y = 0.0) and how to safely lower the tool to the top of the work to get Z = 0.0. There are many possible techniques some of which are explained later in this chapter.

Although we Referenced the machine so machine coordinates are zero at the home switch position this is not essential. Clicking the Zero button on axis DROs will set a work offset value whatever the value of the machine coordinates.

So to summarize, any move made in a part-program or by typing in the MDI line which gives a new set of program coordinate values will cause the Control Software to add on the appropriate offsets and then move the machine position to the newly calculated value of the machine coordinates value. The sum it does is shown on the Offsets screen.

You may find it helpful to move the tool around on your machine above some scrap stock and use a tape-measure to reconcile the DRO readings with the machine position relative to the switches and the stock. When you have a clear picture in your mind of what is happening you have mastered the idea of offsets and should have no problems with this chapter.

6.7 Multiple Work Origins

Offsets

6.7.1 G54 Work Offset

The previous explanations of offsets have only referred to a single set (X, Y, Z, A) of work offsets. These are always in effect when the Control Software is loaded.

It is sometimes useful to have another set of offsets and for them to be persistent when the system is closed down and reloaded. Suppose you have a machine vice permanently fixed to the table. It would be useful to remember the top left corner of its fixed jaw as this is a simple datum to locate stock.

6.7.2 Other Work Offsets

The control software allows you to setup a total of more than 250 different sets of work offsets; most people will only use the first six as these are easily selected using the codes G54 to G59. The Offsets screen has a pair of buttons to select the work offsets that are in use and displayed (figure 6.28).

When you Touch or enter values in the axis DROs then you will update the current set of work offsets.

You can save the work offset values using the Edit/Save table Now button above the Work Offset DROs. This button displays the complete table. It can be edited manually and is saved by clicking the Save button. The dialog is closed by clicking OK.

If you do not save the work offset table then, when you close down the Control Program, you will be asked if you want to save it. Unless you have made a serious error in setting up work offsets, you should save them or you will have to enter them again next time you run the Control Program. We advise you not to alter the G54 offsets although it is remembered from run to run of the Control Software.

Using Tormach PCNC 770 6-14 32426 Rev C1-1

Figure 6.28 – Choosing

Work Offsets

Offsets

ear Compensation Example

6.8 Cutter Diameter Compensation

6.8.1 CAD/CAM and Wizards

We have shown how it is necessary to allow for the diameter of the tool when cutting around an object or cutting out a pocket. You are strongly advised to do this by your CAD/CAM software or the Wizard which generates the part-program. The advantage of it being done this way is that the software has knowledge of the future path of the tool so can avoid overshooting on sharp inside corners. In general this cannot be done by the control software.

Some systems allow code written by hand of by CAM to be fine tuned when it is run by adjusting the diameter of the cutter. We advise against trying to do this with the current version of the Control Software. Generate code by using CAM or writing by hand to move the centre of the cutter along the path that will give you the cut you require with the planned diameter of cutter. In other words, avoid the use of G41 or G42 commands.

You are unlikely to need to read the remainder of this chapter which describes the actual operation of the Control Software.

6.8.2 Concepts for Cutter Diameter/Radius Compensation

The standard mode is for cutter compensation to be off (G40). Without cutter compensation the machine will follow a tool path that is defined by the G- code program. With cutter compensation turned on (G41, G42) the actual path the machine follows will be offset, left or right of the stated path, by an amount specified in the tool offset table.

There are two ways to use cutter radius compensation. The most obvious way is to have the offset stated in the tool table to be the diameter of the tool. In theory this would allow the Gcode program to simply define the geometry of the actual part to be machined with the machine controller left to calculate the tool paths necessary to compensate for cutter diameter. In practice the problem is far more complex and can lead to a great deal of trouble in debugging the G-code program.

Another way to use cutter compensation is as a small correction factor, where the tool path planning is done outside of the machine and the offset is used to only to make minor adjustments. This approach can be used to make fine adjustments for tool wear, part tolerance, or final finish cuts for rough cutting to finish cutting.

Suppose a shop prefers to resharpen cutting tools, not disposing of a tool until it is more than 0.005” reduced in diameter. In this situation a programmer could do his CAM work and create a G & M code with

6.8.3 Caveats in the Use of Cutter Compensation

While the concept has useful applications, there are many pitfalls in actual practice. This is not a programming technique for beginners. A few of the issues are listed below:

a tool path that assumes a 0.495” diameter for a 1/2” diameter tool. When the tool is new and has a true

0.500” diameter, the operator will put 0.005” in the offset table for the tool (0.495 + 0.005 = 0.500). As the

1. Proper application is complex and involves a

large number of coding specific rules. The most complete reference we know of is A

Comprehensive Guide to Practical CNC Programming2 in which the author describes

how to apply radius offsets in 24 pages of the book.

tool is sharpened and becomes smaller, the offset is appropriately reduced. When the offset needed is zero, the tool is replaced. Using this approach the operator can us both new and resharpened tools with the same G&M code program.

2. Path planning is highly sensitive to lead in and

lead out planning. The machine controller cannot compensate under all conditions.

A Comprehensive Guide to Practical CNC Programming (ISBN 978-0-8311-3347-4) by Peter Smid is one of

several advanced machining and programming books available from the Tormach web site (www.tormach.com).

32426 Rev C1-1 6-15 Using Tormach PCNC 770

(begin at X1.50, Y-1.25)

Actual Tool Path with

3. There is no truly standard implementation of cutter compensation. If you have

experience in using cutter compensation with Fanuc, Siemens, GSK, Haas, Centroid, or other control systems, do not expect the Mach3 implementation to react in the same manner.

4. Utility and application may be limited by the look-ahead limit. Cutter compensation in

Mach3 cannot prevent clipping corners when going into internal cavities. See the example in section 6.6.4.

5. Mach3 has limitations in scope of application of cutter radius compensation. We

advise against using cutter compensation in combination with subroutine programming, canned cycles, macro programming, polar mode, with run from here function, and with multiple work offsets.

The complexity of application for cutter compensation can lead to hours of programming debugging. Given the nature of the problem, Tormach cannot provide program debugging support nor resolve application specific questions regarding the use of cutter compensation.

6.8.4 Examples of Operation

The program below plans cutting a rectangle which is 2” x 2”. The graphic below shows two paths. On the left, in a solid line, we see the path described by the G code program. On the right, in the dashed line, we see the actual path that is followed by the Mach3 controller when tool #1 is programmed with a 0.5” diameter.

Offsets

G Code Path

(begin at X1.50, Y-1.25)

(end at X1, Y-1.5)

Figure 6.29 – Toolpath in Example 1

Cutter Compensation

Example 1:

G17 G20 G40 G49 G50 G64 G90 G94 M6 T1 G43 H1 (Select Tool 1 and offset 1) G0 Z1 M3 S1000 (Start Spindle) X1.5 Y-1.25 (Move to lead in position) G1 z-.5 f50 (Z down to cutting level) G41 (Turn on cutter compensation) G1 X1 Y-1 (Cut around block which is 2x2 in dimension) X-1 Y-1 X-1 Y1 X1 Y1 X1 Y-1.5 G40

(end at X1.25, Y-1.5)

Using Tormach PCNC 770 6-16 32426 Rev C1-1

Offsets

)

ActualT

oolPathwit

)

G0 X 1.5 Y-1.5 Z1 M5(Z up, spindle off)

The result of the offset is that the planned 2”x 2” block is cut out. A composite drawing, figure 6.30, shows this along with the tool diameter.

Now let’s look at a slightly different example to see what can go wrong. The example below is nearly identical, but a slightly different starting point is used which is 0.25” lower in Y. At first glance it seems fine.

(begin at X1.50, Y-1.25)

Example 2:

G17 G20 G40 G49 G50 G64 G90 G94 M6 T1 G43 H1 (Select tool1) G0 Z1 M3 S1000 (Start Spindle) X1.5 Y-1.5 (position above lead in point) G1 z-.5 f50 (Z down to cutting level) G41 (turn on cutter compensation) G1 X1 Y-1 X-1 Y-1 X-1 Y1 X1 Y1 X1 Y-1.5 G40 G0 X 1.5 Y-1.5 Z1 M5

M30

CutterCompensation

GCodePath

(end at X1.25, Y-1.50)

Figure 6.30 – Example 1 overlaid

(beginatX1.50,Y-1.50)

Figure 6.31 – Toolpath in example 2

(beginatX1.50,Y-1.50

(endatX1.25,Y-1.50)

The coded path and resulting compensated tool look similar, but the lead in here is coming in at a 45 degree angle.

Looking at the combined result (figure 6.32) we what might seem correct.

(beginatX1.50,Y-1.50

(endatX1.25,Y-1.50)

Figure 6.32 – Example 2 overlaid

32426 Rev C1-1 6-17 Using Tormach PCNC 770

But when we take a closer look at the first corner we can see that the lead in came a bit short, leading to a burr on the corner. An adjustment of the initial lead in position is necessary to fix this. Detailed issues like this are difficult to find in advance, which is one of the reasons that use of cutter compensation can be time consuming to debug. Programming of entry moves is critical when using cutter compensation and some debugging of a program is frequently necessary.

Offsets

Figure 6.33 – Detail of example 2

Programming Entry Considerations

In general, an alignment move and two entry moves are best to begin compensation correctly. However, where the G41/G42 compensation is only going to be used as a small correction factor, it’s usually possible to incorporate only one entry move (plus, possibly, a pre-entry move) is needed. The general method, which will work in most situations, is described first. We

Figure 6.34 – General Entry Move solution

Using Tormach PCNC 770 6-18 32426 Rev C1-1

Offsets

assume here that the programmer knows what the contour is already and has the job of adding entry moves.

General Method

The general method includes programming an alignment move and two entry moves. The entry moves given above will be used as an example. Here is the relevant code:

G1 X1 Y4.5 (make alignment move to point C)

G41 G1 Y3.5 (turn compensation on and make first entry move to point B)

G3 X2 Y2.5 I1 (make second entry move to point A)

Figure 6.34 shows the two entry moves but not the alignment move. First, pick a point A on the contour where it is convenient to attach an entry arc. Specify an arc outside the contour which begins at a point B and ends at A tangent to the contour (and going in the same direction as it is planned to go around the contour). The radius of the arc should be larger than half the diameter given in the tool table. Then extend a line tangent to the arc from B to some point C, located so that the line BC is more than one radius long. After the construction is finished, the code is written in the reverse order from the construction. Cutter radius compensation is turned on after the alignment move and before the first entry move. In the code above, line N0010 is the alignment move, line N0020 turns compensation on and makes the first entry move and line N0030 makes the second entry move.

In this example, the arc AB and the line BC are fairly large, but they need not be. For a toolpath contour, the radius of arc AB need only be slightly larger than the maximum possible deviation of the radius of the tool from the exact size. Also for a toolpath contour, the side chosen for compensation should be the one to use if the tool is oversized. As mentioned earlier, if the tool is undersized, the interpreter will switch sides.

6.8.5 Look Ahead Issues

There can be problems with cutter compensation related to the lack of foresight on the part of the controller. The program below plans cutting an edge using cutter compensation shown in the graphic as CDEFGHIJ. The segments AB and BC are entry segments as described above.

G17 G20 G40 G49 G50 G64 G90 G94 M6 T1 G43 H1 G0 X-1 Y2 Z1 M3 S1000 (position above starting point) G1 z-0.5 f50 (Z down to cutting height) G41 X-1 Y1 (Making the first entry move to point B) G3 X0 Y0 R1 (Doing the entry arc to point C) G1 X1 (cutting to point D) Y-1.5 (cutting to point E) X2 (cutting to point F) Y-0.5 X1.5 Y0 X3.5 G40 G0 Z1 M5 M30

In figure 6.35 we can see how a 1/4” tool will cut this. The process is successful, but only because of the small diameter of the cutter.

32426 Rev C1-1 6-19 Using Tormach PCNC 770

Offsets

Figure 6.35 – Compensating a small tool

If we change to a 0.787” cutter (common 20 mm end mill) we see the results in figure 6.36.

Figure 6.36 – Compensation fails with large tool

Using Tormach PCNC 770 6-20 32426 Rev C1-1

What has happened here is that the cutter is too big for the channel in the pocket. As it is cutting path DE, it’s removing the sidewall of IH. Likewise on the way out, it will destroy a segment of wall DE while it climbs out along path IH. We would prefer that the controller would either,

1) stop and generate an error message, or 2) cut a path from D to I, avoiding the cavity created by EFGH. That’s not what happens. This type of error is less common when doing cutter offsets and exact path planning in your CAM software as opposed to using the controller to calculate offsets.

6.8.6 Other Restrictions

• All moves should be longer than the amount to be offset. This restriction makes it clear

the increased limitations of using cutter compensation to offset for the full tool radius instead of using it to only compensate for wear, tolerance, or final finish depth of cut.

• Leadin moves should be longer than the amount you want to offset.

• The radius of an inside arc should be greater than that of the cutting tool.

• The Mach3 tool table includes both Diameter and Diameter Wear columns. Always use

the Diameter column, even when only using G41/G42 for wear compensation. The Diameter Wear data column in the Mach3 tool table is for future development and does not function as of this writing.

• There must not be more than 50 consecutive lines of code without a movement command,

e.g. XY positions only.

Offsets

• Cutter compensation must not be applied or canceled on a G02 or G03 command. A legal

line would be:

G01 G42 P2.5 X20 (legal)

G02 G42 P2.5 X20 Y0 R10 (illegal)

6.8.7 Perspective on Cutter Compensation

In the past, effective and affordable CAM software was simply not available and, despite all the pitfalls and complications, application of G41/G42 cutter compensation in a CNC machine tool was more common. There was simply no other solution. Now that high quality CAM software is widely available most people do tool offsets in CAM and don’t bother with using G41/G42 for offsets in the machine controller.

Nevertheless, there remain instances where controller based offsets are useful. If you decide to use the G41/G42 codes, be prepared for considerable debugging. Some apparent roadblocks may be avoided through experimentation and minor modifications to your G-code program. Others may be inherent to Mach3 or the desired geometry you are trying to achieve.

As a matter of practical experience, we recommend path planning in CAM and avoiding the use of G41/G42 where possible. When it becomes necessary to us the G41/G42 functions we suggest you apply the codes to simple geometry parts, applying small compensations (i.e. wear compensation, not cutter radius compensation), using 2 segment lead in, and be prepared for some experimentation/debugging.

6.8.8 Resources for Debugging Cutter Compensation

As noted earlier, Tormach cannot provide program debugging support nor resolve application specific questions regarding the use of cutter compensation. Basic solutions for debugging code files can usually be resolved through a systematic approach of “divide and conquer”, where you section codes and single step through a code, sometimes in combination with M1 optional stop statements. Additional guidance can be had from:

Programming of CNC Machines, by Ken Evans. Refer to section 4 pages 250 to 261

32426 Rev C1-1 6-21 Using Tormach PCNC 770

Offsets

CNC Programming Techniques, by Peter Smid. Refer to chapter 4, pages 46 to 66

Both of these reference books are available through the Tormach web site (www.tormach.com) Final Note: We should re-iterate that it is much better for a CAM program to generate the path

of the tool allowing for its diameter because it can "see" the implications of cutting complex corners in a way which the control software cannot.

Using Tormach PCNC 770 6-22 32426 Rev C1-1

Programming language reference

7. Part-programming Language Reference

This section defines the language (G-codes, etc.) that are understood and

interpreted by the Control Software.

This chapter is intended for reference purposes. Sample programs using these

commands are included in the folder C:/PCNC3/GCode.

If you want to learn about the principles of the control language so you can write

programs by hand from first principles then you should consult an introductory

textbook on G-code programming.

7.1 Definitions

7.1.1 Control Software

This is the term used for the program running under Microsoft Windows in the PC connected to your PCNC. In this chapter the Control Software is shortened to the CS.

7.1.2 Linear Axes

The X-, Y- and Z-axes form a standard right-handed coordinate system of orthogonal linear axes. Positions of the three linear motion mechanisms are expressed using coordinates on these axes.

7.1.3 Rotational Axes

The rotational axes are measured in degrees as wrapped linear axes in which the direction of positive rotation is counterclockwise when viewed from the positive end of the corresponding X-, Y- or Z-axis. By “wrapped linear axis,” we mean one on which the angular position increases without limit (goes towards plus infinity) as the axis turns counterclockwise and decreases without limit (goes towards minus infinity) as the axis turns clockwise. Wrapped linear axes are used regardless of whether or not there is a mechanical limit on rotation.

Clockwise or counterclockwise is from the point of view of the workpiece. If the workpiece is fastened to a turntable which turns on a rotational axis, a counterclockwise turn from the point of view of the workpiece is accomplished by turning the turntable in a direction that (for most common machine configurations) looks clockwise from the point of view of someone standing next to the machine.

7.1.4 Scaling Input

It is possible to set-up scaling factors for each axis. These will be applied to the values of X, Y, Z, A, I, J and R words whenever these are entered. This allows the size of features machined to be altered and mirror images to be created – by use of negative scale factors.

The scaling is the first thing done with the values and things like feed rate are always based on the scaled values.

The offsets stored in tool and fixture tables are not scaled before use. Scaling may, of course, have been applied at the time the values were entered (say using G10).

32426 Rev C1-1 7-1 Using Tormach PCNC 770

Programming language reference

7.1.5 Controlled Point

The controlled point is the point whose position and rate of motion are controlled. When the tool length offset is zero (the default value), this is a point on the spindle axis (often called the gauge point) that is some fixed distance beyond the end of the spindle, usually near the end of a tool holder that fits into the spindle. The location of the controlled point can be moved out along the spindle axis by specifying some positive amount for the tool length offset. This amount is normally the length of the cutting tool in use, so that the controlled point is at the end of the cutting tool.

7.1.6 Coordinated Linear Motion

To drive a tool along a specified path, a machining system must often coordinate the motion of several axes. We use the term “coordinated linear motion” to describe the situation in which, nominally, each axis moves at constant speed and all axes move from their starting positions to their end positions at the same time. If only the X-, Y- and Z-axes (or any one or two of them) move, this produces motion in a straight line, hence the word “linear” in the term. In actual motions, it is often not possible to maintain constant speed because acceleration or deceleration is required at the beginning and/or end of the motion. It is feasible, however, to control the axes so that, at all times, each axis has completed the same fraction of its required motion as the other axes. This moves the tool along the same path and we also call this kind of motion coordinated linear motion.

Coordinated linear motion can be performed either at the prevailing feed rate or at rapid traverse rate. If physical limits on axis speed make the desired rate unobtainable, all axes are slowed to maintain the desired path.

7.1.7 Feed Rate

The rate at which the controlled point or the axes move is nominally a steady rate which may be set by the user. In the Interpreter, the interpretation of the feed rate is as follows unless inverse time feed rate (G93) mode is being used:

• For motion involving one or more of the linear axes (X, Y, Z and optionally A, B, C),

without simultaneous rotational axis motion, the feed rate means length units per minute along the programmed linear XYZ(ABC) path.

• For motion involving one or more of the linear axes (X, Y, Z and optionally A, B, C), with

simultaneous rotational axis motion, the feed rate means length units per minute along the programmed linear XYZ(ABC) path combined with the angular velocity of the rotary axes multiplied by the appropriate axis Correction Diameter multiplied by pi, where

π = 3.14152 (i.e., the declared “circumference” of the part).

• For motion of one rotational axis with X-, Y- and Z-axes not moving, the feed rate means

degrees per minute rotation of the rotational axis.

• For motion of two or three rotational axes with X-, Y- and Z-axes not moving, the rate is

applied as follows: Let dA, dB and dC be the angles in degrees through which the A-, Band C-axes, respectively, must move. Let D = sqrt (dA2 + dB2 + dC2). Conceptually, D is a measure of total angular motion, using the usual Euclidean metric. Let T be the amount of time required to move through D degrees at the current feed rate in degrees per minute. The rotational axes should be moved in coordinated linear motion so that the elapsed time from the start to the end of the motion is T plus any time required for acceleration or deceleration.

7.1.8 Arc Motion

Any pair of the linear axes (XY, YZ and XZ) can be controlled to move in a circular arc in the plane of that pair of axes. While this is occurring, the third linear axis and the rotational axes can be controlled to move simultaneously at effectively a constant rate. As in coordinated linear

Using Tormach PCNC 770 7-2 32426 Rev C1-1

motion, the motions can be coordinated so that acceleration and deceleration do not affect the path.

If the rotational axes do not move, but the third linear axis does move, the trajectory of the controlled point is a helix.

The feed rate during arc motion is as described in Feed Rate above. In the case of helical motion, the rate is applied along the helix. Beware as other interpretations are used on other systems.

7.1.9 Coolant

Flood coolant and mist coolant may each be turned on independently. They are turned off together.

7.1.10 Dwell

A machining system may be commanded to dwell (i.e., keep all axes unmoving) for a specific amount of time. The most common use of dwell is to break and clear chips or for a spindle to get up to speed. The units in which you specify Dwell are either seconds or Milliseconds depending on the setting on Configure>Logic.

7.1.11 Units

Units used for distances along the X-, Y- and Z-axes may be measured in millimeters or inches. Units for all other quantities involved in machine control cannot be changed. Different quantities use different specific units. Spindle speed is measured in revolutions per minute. The positions of rotational axes are measured in degrees. Feed rates are expressed in current length units per minute, or in degrees per minute, as described above.

Programming language reference

Warning: We advise you to check very carefully the system’s response to changing units while tool and fixture offsets are loaded into the tables, while these offsets are active and/or while a part-program is executing

7.1.12 Current Position

The controlled point is always at some location called the “current position” and the Control Software always knows where that is. The numbers representing the current position are adjusted in the absence of any axis motion if any of several events take place:

• Length units are changed (see Warning above);

• Tool length offset is changed;

• Coordinate system offsets are changed.

7.1.13 Selected Plane

There is always a “selected plane,” which must be the XY-plane, the YZ-plane or the XZ-plane of the machining system. The Z-axis is, of course, perpendicular to the XY-plane, the X-axis to the YZ-plane and the Y-axis to the XZ-plane.

7.1.14 Tool Table

Zero or one tool is assigned to each slot in the tool table.

7.1.15 Path Control Modes

The machining system may be put into any one of two path control modes: (1) exact stop mode, (2) constant velocity mode. In exact stop mode, the machine stops briefly at the end of each programmed move. In constant velocity mode, sharp corners of the path may be rounded

32426 Rev C1-1 7-3 Using Tormach PCNC 770

Programming language reference

slightly so that the feed rate may be kept up. These modes are to allow the user to control the compromise involved in turning corners because a real machine has a finite acceleration due to the inertia of its mechanism.

Exact stop does what it says. The machine will come to rest at each change of direction and the tool will therefore precisely follow the commanded path.

Constant velocity will overlap acceleration in the new direction with deceleration in the current one in order to keep the commanded feed rate. This implies a rounding of any corner but faster and smoother cutting. This is particularly important in routing and plasma cutting. The lower the acceleration of the machine axes, the greater will be the radius of the rounded corner.

In Plasma mode (set on Configure Logic dialog) the system attempts to optimize corner motion for plasma cutting by a proprietary algorithm.

It is also possible to define a limiting angle so that changes in direction of more than this angle will always be treated as Exact Stop even though Constant Velocity is selected. This allows gentle corners to be smoother but avoids excessive rounding of sharp corners even on machines with low acceleration on one or more axes. This feature is enabled in the Configure Logic dialog and the limiting angle is set by a DRO. This setting will probably need to be chosen experimentally depending on the characteristics of the machine tool and, perhaps, the toolpath of an individual job.

7.2 Interpreter Interaction with Controls

7.2.1 Feed and Speed Override controls

The CS has commands which enable (M48) or disable (M49) the feed and speed override switches. It is useful to be able to override these switches for some machining operations. The idea is that optimal settings have been included in the program and the operator should not change them.

7.2.2 Block Delete Control

If the block delete control is ON, lines of code which start with a slash (the block delete character) are not executed. If the switch is off, such lines are executed.

7.2.3 Optional Program Stop Control

The optional program stop control works as follows. If this control is ON and an input line contains an M01-code, program execution is stopped at the end on the commands on that line until the Cycle Start button is pushed.

7.3 Tool File

The CS maintains a tool file for each of the 256 tools which can be used. Each data line of the file contains the data for one tool. This allows the definition of the tool

length (Z-axis), tool diameter (for milling) and tool tip radius (for turning).

7.4 Part-programs Language

7.4.1 Overview

The language is based on lines of code. Each line (also called a “block”) may include commands to the machining system to do several different things. Lines of code may be collected in a file to make a program.

Using Tormach PCNC 770 7-4 32426 Rev C1-1

A typical line of code consists of an optional line number at the beginning followed by one or more “words.” A word consists of a letter followed by a number (or something that evaluates to a number). A word may either give a command or provide an argument to a command. For example, G1 X3 is a valid line of code with two words. “G1” is a command meaning “move in a straight line at the programmed feed rate,” and “X3” provides an argument value (the value of X should be 3 at the end of the move). Most commands start with either G (General) or M (Miscellaneous). The words for these commands are called “G-codes” and “M-codes.”

The language has two commands (M2 or M30), either of which ends a program. A program may end before the end of a file. Lines of a file that occur after the end of a program are not to be executed in the normal flow so will generally be parts of subroutines.

7.4.2 Parameters

The CS maintains an array of 10,320 numerical parameters. Many of them have specific uses. The parameters that are associated with fixtures are persistent over time. Other parameters will be undefined when The CS is loaded. The parameters are preserved when the interpreter is reset. Parameters 1 to 1000 can be used by the code of part-programs.

7.4.3 Coordinate Systems

The machining system has an absolute coordinate system and 254 work offset (fixture) systems.

Programming language reference

You can set the offsets of tools by G10 L1 P~ X~ Z~. The “P word” defines the tool number to be set.

You can set the offsets of the fixture systems using G10 L2 P~ X~ Y~ Z~ A~ B~ C~. The P word defines the fixture to be set. The X, Y, Z, etc. words are the coordinates for the origin of the axes in terms of the absolute coordinate system.

You can select one of the first seven work offsets by using G54, G55, G56, G57, G58 or G59. Any of the 254 work offsets can be selected by G59 P~ (e.g., G59 P23 would select fixture

23). The absolute coordinate system can be selected by G59 P0. You can offset the current coordinate system using G92 or G92.3. This offset will then be

applied on top of work offset coordinate systems. This offset may be cancelled with G92.1 or G92.2.

You can make straight moves in the absolute machine coordinate system by using G53 with either G0 or G1.

7.5 Formatting Code Lines (Block)

A permissible line of input code consists of the following, in order, with the restriction that there is a maximum (currently 256) to the number of characters allowed on a line.

• Optional block delete character, which is a slash "/"

• Optional line number

• Any number of words, parameter settings and comments

• End of line marker (carriage return or line feed or both)

Any input not explicitly allowed is illegal and will cause the Interpreter to signal an error or to ignore the line.

Currently programs are limited to 999,999 lines of code. Spaces and tabs are allowed anywhere on a line of code and do not change the meaning of the

line, except inside comments. This makes some strange-looking input legal. For example, the line g0x +0. 12 34y 7 is equivalent to g0 x+0.1234 y7

Blank lines are allowed in the input. They will be ignored.

32426 Rev C1-1 7-5 Using Tormach PCNC 770

Programming language reference

Input is case insensitive, except in comments; thus, any letter outside a comment may be in upper or lower case without changing the meaning of a line.

Letter Meaning

A A-axis of machine B B-axis of machine C C-axis of machine D tool radius compensation number F feed rate G general function (see Table 5) H tool length offset index I X-axis offset for arcs

X offset in G87 canned cycle

J Y-axis offset for arcs

Y offset in G87 canned cycle

K Z-axis offset for arcs

Z offset in G87 canned cycle

number of repetitions in canned cycles/subroutines

key used with G10 M miscellaneous function (see Table 7) N line number O Subroutine label number P dwell time in canned cycles

dwell time with G4

key used with G10

tapping depth in M871 – M874 Q feed increment in G83 canned cycle

repetitions of subroutine call R arc radius

canned cycle retract level S spindle speed T tool selection U Synonymous with A V Synonymous with B W Synonymous with C X X-axis of machine Y Y-axis of machine Z Z-axis of machine

Figure 7.1 – Word initial letters

7.5.1 Line Number

A line number is the letter N followed by an integer (with no sign) between 0 and 99,999,999 written without commas. Line numbers may be repeated or used out of order, although normal practice is to avoid such usage. A line number is not required to be used (and this omission is common) but it must be in the proper place if it is used.

Using Tormach PCNC 770 7-6 32426 Rev C1-1

7.5.2 Subroutine Labels

A subroutine label is the letter O followed by an integer (with no sign) between 0 and 99999 written with no more than five digits (000009 is not permitted, for example). Subroutine labels may be used in any order but must be unique in a program. Nothing else except a comment should appear on the same line as a subroutine label. Note that line numbers are not permitted with an O word in the current release of the software.

7.5.3 Word

A word is a letter other than N or O followed by a real value. Words may begin with any of the letters (figure 7.1). The table includes N and O for

completeness, even though, as defined above, line numbers are not words. Several letters (I, J, K, L, P and R) may have different meanings in different contexts.

A real value is some collection of characters that can be processed to come up with a number. A real value may be an explicit number (such as 341 or -0.8807), a parameter value, an expression or a unary operation value. Definitions of these follow immediately. Processing characters to come up with a number is called “evaluating.” An explicit number evaluates to itself.

7.5.3.1 Number

The following rules are used for (explicit) numbers. In these rules a digit is a single character between 0 and 9.

Programming language reference

• A number consists of (1) an optional plus or minus sign, followed by (2) zero to

many digits, followed, possibly, by (3) one decimal point, followed by (4) zero to many digits – provided that there is at least one digit somewhere in the number.

• There are two kinds of numbers: integers and decimals. An integer does not have a

decimal point in it; a decimal does.

• Numbers may have any number of digits, subject to the limitation on line length.

Only about seventeen significant figures will be retained, however (enough for all known applications).

• A non-zero number with no sign as the first character is assumed to be positive.

Notice that initial (before the decimal point and the first non-zero digit) and trailing (after the decimal point and the last non-zero digit) zeros are allowed but not required. A number written with initial or trailing zeros will have the same value when it is read as if the extra zeros were not there.

Numbers used for specific purposes by the Control Software are often restricted to some finite set of values or some to some range of values. In many uses, decimal numbers must be close to integers; this includes the values of indexes (for parameters and carousel slot numbers, for example), M-codes and G-codes multiplied by ten. A decimal number which is supposed to be close to an integer is considered close enough if it is within 0.0001 of an integer.

7.5.3.2 Parameter Value

A parameter value is the hash character # followed by a real value. The real value must evaluate to an integer between 1 and 10320. The integer is the parameter identification number. Think of it as the number of a pigeon-hole and distinguish this from its real value which is whatever number is stored in it.

The # character takes precedence over other operations, so that, for example, #1+2 means the number found by adding 2 to the value of parameter 1, not the value found in parameter 3. Of course, #[1+2] does mean the value found in parameter 3. The # character may be repeated; for example ##2 means the value of the parameter whose index is the (integer) value of parameter 2.

32426 Rev C1-1 7-7 Using Tormach PCNC 770

Programming language reference

7.5.3.3 Expressions and Binary Operations

An expression is a set of characters starting with a left bracket ([) and ending with a balancing right bracket (]). In between the brackets are numbers, parameter values, mathematical operations and other expressions. An expression may be evaluated to produce a number. The expressions on a line are evaluated when the line is read, before anything on the line is executed. An example of an expression is: [1+acos[0]-[#3**[4.0/2]]]

Binary operations appear only inside expressions. Nine binary operations are defined. There are four basic mathematical operations: addition (+), subtraction (-), multiplication (*) and division (/). There are three logical operations: non-exclusive or (OR), exclusive or (XOR) and logical and (AND). The eighth operation is the modulus operation (MOD). The ninth operation is the “power” operation (**) of raising the number on the left of the operation to the power on the right.

The binary operations are divided into three groups. The first group is: power. The second group is: multiplication, division and modulus. The third group is: addition, subtraction, logical non-exclusive or, logical exclusive or and logical. If operations are strung together (for example in the expression [2.0/3*1.5-5.5/11.0]), operations in the first group are to be performed before operations in the second group and operations in the second group before operations in the third group. If an expression contains more than one operation from the same group (such as the first / and * in the example), the operation on the left is performed first. Thus, the example is equivalent to: [((2.0/3)*1.5)-(5.5/11.0)] which simplifies to [1.0-0.5] which is 0.5.

The logical operations and modulus are to be performed on any real numbers, not just on integers. The number zero is equivalent to logical false and any non-zero number is equivalent to logical true.

7.5.3.4 Unary Operation Value

A unary operation value is either “ATAN” followed by one expression divided by another expression (for example ATAN[2]/[1+3]) or any other unary operation name followed by an expression (for example SIN[90]). The unary operations are: ABS (absolute value), ACOS (arc cosine), ASIN (arc sine), ATAN (arc tangent), COS (cosine), EXP (e raised to the given power), FIX (round down), FUP (round up), LN (natural logarithm), ROUND (round to the nearest whole number), SIN (sine), SQRT (square root) and TAN (tangent). Arguments to unary operations which take angle measures (COS, SIN and TAN) are in degrees. Values returned by unary operations which return angle measures (ACOS, ASIN and ATAN) are also in degrees.

The FIX operation rounds towards the left (less positive or more negative) on a number line, so that FIX[2.8]=2 and FIX[-2.8]=-3, for example. The FUP operation rounds towards the right (more positive or less negative) on a number line; FUP[2.8]=3 and FUP[-2.8]=-2, for example.

7.5.4 Parameter Setting

A parameter setting is the following four items one after the other:

• a pound character # ;

• a real value which evaluates to an integer between 1 and 10320;

• an equal sign = ;

• a real value.

• For example “#3 = 15” is a parameter setting meaning “set parameter 3 to 15.”

A parameter setting does not take effect until after all parameter values on the same line have been found. For example, if parameter 3 has been previously set to 15 and the line #3=6 G1

Using Tormach PCNC 770 7-8 32426 Rev C1-1

Programming language reference

x#3 is interpreted, a straight move to a point where x equals 15 will occur and the value of parameter 3 will be 6.

7.5.5 Comments and Messages

Printable characters and white space inside parentheses are considered a “comment.” A left parenthesis always starts a comment. The comment ends at the first right parenthesis found thereafter. Once a left parenthesis is placed on a line, a matching right parenthesis must appear before the end of the line. Comments may not be nested; it is an error if a left parenthesis is found after the start of a comment and before the end of the comment. Here is an example of a line containing a comment: G80 M5 (stop motion)

The remainder of the line is treated as a comment. Comments do not cause the machining system to do anything. A comment contains a message if MSG, appears after the left parenthesis and before any other

printing characters. Variants of MSG, which include white space and lower case characters, are allowed. Note the comma which is required. The rest of the characters before the right parenthesis are considered to be a message to the operator. Messages are displayed on screen in the “Error” intelligent label.

7.5.6 Item Repeats

A line may have any number of G words, but two G words from the same modal group may not appear on the same line.

A line may have zero to four M words. Two M words from the same modal group may not appear on the same line.

For all other legal letters, a line may have only one word beginning with that letter. If a parameter setting of the same parameter is repeated on a line, #3=15 #3=6, for example,

only the last setting will take effect. It is silly, but not illegal, to set the same parameter twice on the same line.

If more than one comment appears on a line, only the last one will be used; each of the other comments will be read and its format will be checked, but it will be ignored thereafter. It is expected that putting more than one comment on a line will be very rare.

7.5.7 Item Order

The three types of item whose order may vary on a line (as given at the beginning of this section) are word, parameter setting and comment. Imagine that these three types of item are divided into three groups by type.

The first group (the words) may be reordered in any way without changing the meaning of the line.

If the second group (the parameter settings) is reordered, there will be no change in the meaning of the line unless the same parameter is set more than once. In this case, only the last setting of the parameter will take effect. For example, after the line #3=15 #3=6 has been interpreted, the value of parameter 3 will be 6. If the order is reversed to #3=6 #3=15 and the line is interpreted, the value of parameter 3 will be 15.

If the third group (the comments) contains more than one comment and is reordered, only the last comment will be used.

If each group is kept in order or reordered without changing the meaning of the line, then the three groups may be interleaved in any way without changing the meaning of the line. For example, the line g40 g01 #3=15 (so there!) #4=-7.0 has five items and means

32426 Rev C1-1 7-9 Using Tormach PCNC 770

Programming language reference

The modal groups for G

codes are

The modal groups for M

codes are:

In addition to the above modal groups, there is a group for non

modal

exactly the same thing in any of the 120 possible orders – such as #4=-7.0 g01 #3=15 g40 (so there!) – for the five items.

7.5.8 Commands and Machine Modes

The Control Software has many commands that cause a machining system to change from one mode to another. The mode stays active until some other command changes it implicitly or explicitly. Such commands are called “modal.” For example, if coolant is turned on, it stays on until it is explicitly turned off. The G-codes for motion are also modal. If a G1 (straight move) command is given on one line, for example, it will be executed again on the next line if one or more axis words is available on the line, unless an explicit command is given on that next line using the axis words or canceling motion.

“Non-modal” codes have effect only on the lines on which they occur. For example, G4 (dwell) is non-modal.

7.6 Modal Groups

Modal commands are arranged in sets called “modal groups,” and only one member of a modal group may be in force at any given time. In general, a modal group contains commands for which it is logically impossible for two members to be in effect at the same time (e.g., measure

• group 1 = {G00, G01, G02, G03, G38.2, G80, G81, G82, G84, G85,

G86, G87, G88, G89} motion

• group 2 = {G17, G18, G19} plane selection

• group 3 = {G90, G91} distance mode

• group 5 = {G93, G94} feed rate mode

• group 6 = {G20, G21} units

• group 7 = {G40, G41, G42} cutter radius compensation

• group 8 = {G43, G49} tool length offset

• group 10 = {G98, G99} return mode in canned cycles

• group 12 = {G54, G55, G56, G57, G58, G59, G59.xxx} coordinate

system selection

• group 13 = {G61, G61.1, G64} path control mode ♦ group 4 = {M0, M1, M2, M30} stopping

♦ group 6 = {M6} tool change ♦ group 7 = {M3, M4, M5} spindle turning ♦ group 8 = {M7, M8, M9} coolant (special case: M7 and M8 may be

active at the same time)

♦ group 9 = {M48, M49} enable/disable feed and speed override controls

G-codes:

♦ group 0 = {G4, G10, G28, G30, G53, G92, G92.1, G92.2, G92.3}

Figure 7.2 – Modal groups

in inches vs. measure in millimeters). A machining system may be in many modes at the same time, with one mode from each modal group being in effect (figure 7.2).

For several modal groups, when a machining system is ready to accept commands, one member of the group must be in effect. There are default settings for these modal groups. When the machining system is turned on or otherwise re-initialized, the default values are automatically in effect.

Using Tormach PCNC 770 7-10 32426 Rev C1-1

Group 1, the first group on the table, is a group of G-codes for motion. One of these is always in effect. That one is called the current motion mode.

It is an error to put a G-code from group 1 and a G-code from group 0 on the same line if both of them use axis words. If an axis word-using G-code from group 1 is implicitly in effect on a line (by having been activated on an earlier line) and a group 0 G-code that uses axis words appears on the line, the activity of the group 1 G-code is suspended for that line. The axis wordusing G-codes from group 0 are G10, G28, G30 and G92.

The Control Software displays the current mode at the top of each screen.

7.7 G-codes

G-codes of the CS input language are shown in figure 7.3 and are described in more detail in this section.

The descriptions contain command prototypes, set in courier type. In the command prototypes, the tilde (~) stands for a real value. As described earlier, a real

value may be (1) an explicit number, 4.4, for example, (2) an expression, [2+2.4], for example, (3) a parameter value, #88, for example or (4) a unary function value, acos[0], for example.

In most cases, if axis words (any or all of X~, Y~, Z~, A~, B~, C~, U~, V~, W~) are given, they specify a destination point. Axis numbers relate to the currently active coordinate system, unless explicitly described as being in the absolute coordinate system. Where axis words are optional, any omitted axes will have their current value. Any items in the command prototypes not explicitly described as optional are required. It is an error if a required item is omitted.

Programming language reference

U, V and W are synonyms for A, B and C. Use of A with U, B with V, etc. is erroneous (like using A twice on a line). In the detailed descriptions of codes U, V and W are not explicitly mentioned each time but are implied by A, B or C.

In the prototypes, the values following letters are often given as explicit numbers. Unless stated otherwise, the explicit numbers can be real values. For example, G10 L2 could equally well be written G[2*5] L[1+1]. If the value of parameter 100 were 2, G10 L#100 would also mean the same. Using real values which are not explicit numbers as just shown in the examples is rarely useful.

If L~ is written in a prototype the “~” will often be referred to as the “L number.” Similarly the “~” in H~ may be called the “H number,” and so on for any other letter.

If a scale factor is applied to any axis then it will be applied to the value of the corresponding X, Y, Z, A/U, B/V, C/W word and to the relevant I, J, K or R words when they are used.

7.7.1 Rapid Linear Motion – G00

(a) For rapid linear motion, program: G0 X~ Y~ Z~ A~ where all the axis words are optional, except that at least one must be used. The G00 is optional if the current motion mode is G0. This will produce coordinated linear motion to the destination point at the current traverse rate (or slower if the machine will not go that fast). It is expected that cutting will not take place when a G00 command is executing.

(b) If G16 has been executed to set a Polar Origin then for rapid linear motion to a point described by a radius and angle G0 X~ Y~ can be used. X~ is the radius of the line from the

G16 polar origin and Y~ is the angle in degrees measured with increasing values counterclockwise from the 3 o’clock direction (i.e., the conventional four quadrant conventions).

Coordinates of the current point at the time of executing the G16 are the polar origin.

32426 Rev C1-1 7-11 Using Tormach PCNC 770

Programming language reference

Summary of G

codes

G00 Rapid positioning

G01 Linear interpolation

G02 Clockwise circular/helical interpolation

G03 Counterclockwise circular/helical interpolation

G04 Dwell

G10 Coord

inate system origin setting

G12 Clockwise circular pocket

G13 Counterclockwise circular pocket

G15/G16

Polar Coordinate moves in G00 and G01

G17 XY Plane select

G18 XZ plane select

G19 YZ plane select

G20/G21

Inch/millimeter unit

G28 Return home

G28.1 Reference axes

G30 Return home

G31 Straight probe

G40 Cancel cutter radius compensation

G41/G42

Start cutter radius compensation left/right

G43 Apply tool length offset (plus)

G49 Cancel tool length offset

G50 Reset all scale factors to 1.0

G51 Set axis data input scale factors

G52 Temporary coordinate system offsets

G53 Move in absolute machine coordinate system

G54 Use fixture offset 1

G55 Use fixture offset 2

G56-58 Use fixture offset 3, 4, 5

G59 Use fixture offset 6 / use general fixt

ure number

G61/G64

Exact stop/Constant Velocity mode

G68/G69

Coordinate system rotation

G73 Canned cycle

- peck drilling

G80 Cancel motion mode (including canned cycles)

G81 Canned cycle

–

drilling

G82 Canned cycle

– drilling with dwell

G83 Canned c

ycle

– peck drilling

G85 Canned cycle

– boring, no dwell, feed out

G86 Canned cycle

– boring, spindle stop, rapid out

G88 Canned cycle

– boring, spindle stop, manual out

G89 Canned cycle

– boring, dwell, feed out

G90 Absolute distance mode

G91 Increm

ental distance mode

G92 Offset coordinates and set parameters

G92.x

Cancel G92 etc.

G93 Inverse time feed mode

G94 Feed per minute mode

G95 Feed per rev mode

G98 Initial level return after canned cycles

G99 R-point level return after canned cycles

It is an error if all axis words are omitted.

Using Tormach PCNC 770 7-12 32426 Rev C1-1

Figure 7.3 – Table of G-codes

Programming language reference

If cutter radius compensation is active, the motion will differ from the above; see Cutter Compensation. If G53 is programmed on the same line, the motion will also differ; see Absolute Coordinates.

The G00 command is used to move the tool quickly from one point to another without cutting, thus allowing for quick tool positioning.

Depending on where the tool is located, there are two basic rules to follow for safety’s sake:

If the Z value represents a cutting move in the negative direction, the X and Y axes should be executed first.

If the Z value represents a move in the positive direction, the X and Y axes should be executed last.

Example: N25 G00 X2.5 Y4.75 (Rapid to X2.5,Y4.75)

N30 Z0.1 (Rapid down to Z0.1)

7.7.2 Linear Motion at Feed Rate – G01

(a) For linear motion at feed rate (for cutting or not), program: G01 X~ Y~ Z~ A~, where all the axis words are optional, except that at least one must be used. The G01 is optional if the current motion mode is G01. This will produce coordinated linear motion to the destination point at the current feed rate (or slower if the machine will not go that fast). (b) If G16 has been executed to set a polar origin then linear motion at feed rate to a point described by a radius and angle G00 X~ Y~ can be used. X~ is the radius of the line from the G16 polar origin and Y~ is the angle in degrees measured with increasing values counterclockwise from the 3 o’clock direction (i.e., the conventional four quadrant conventions).

Note that the G00 rapid move should have two distinct movements to ensure that vertical moves are always separate from horizontal moves. In a typical rapid move toward the part, the tool first rapids in the flat, horizontal XY plane. Then, it feeds down in the Z axis. When rapiding out of a part, the G00 command always goes up in the Z axis first, then laterally in the XY plane.

As this diagram shows, if the basic rules are not followed, an accident can result. Improper use of G00 often occurs because clamps are not taken into consideration. Following the basic rules will reduce any chance of error.

Coordinates of the current point at the time of executing the G16 are the polar origin. It is an error if all axis words are omitted.

32426 Rev C1-1 7-13 Using Tormach PCNC 770

Programming language reference

If cutter radius compensation is active, the motion will differ from the above; see Cutter Compensation. If G53 is programmed on the same line, the motion will also differ; see Absolute Coordinates.

Linear Interpolation, or straightline feed moves, on the flat XY plane (no Z values are specified).

(Sample Program G01EX2:) (Workpiece Size: X4, Y3, Z1) (Tool: Tool #3, 3/8" Slot Drill) (Tool Start Position: X0, Y0, Z1)

N2 G90 G80 G40 G54 G20 G17 G50 G94 G64 (safety block) N5 G90 G20 (Block #5, absolute in inches) N10 M06 T3 G43 H3 (Tool change to Tool #3) N15 M03 S1250 (Spindle on CW at 1250 rpm) N20 G00 X1.0 Y1.0 (Rapid over to X1,Y1) N25 Z0.1 (Rapid down to Z0.1) N30 G01 Z-0.125 F5 (Feed down to Z–0.125 at 5 ipm) N35 X3 Y2 F10 (Feed diagonally to X3,Y2 at 10 ipm) N40 G00 Z1.0 (Rapid up to Z1) N45 X0.0 Y0.0 (Rapid over to X0,Y0) N50 M05 (Spindle off) N55 M30 (Program end)

G01 command, using multi-axis feed moves. All diagonal feed moves are a result of a G01 command, where two or more axes are used at once.

In the sample program, several different examples of the G01 command are shown:

1. The first G01 command (in N30) instructs the machine to plunge feed the tool below the

surface of the part by 0.125 in. at a feedrate of 5 in./min.

2. N35 is a two-axis (X and Y) diagonal feed move, and the linear feedrate is increased to

10 ipm.

Note: Because there is contact between the cutting tool and the workpiece, it is imperative that the proper spindle speeds and feedrates be used. It is the programmer’s responsibility to ensure acceptable cutter speeds and feeds.

7.7.3 Arc at Feed Rate – G02 and G03

A circular or helical arc is specified using either G02 (clockwise arc) or G03 (counterclockwise arc). The axis of the circle or helix must be parallel to the X-, Y- or Z-axis of the machine coordinate system. The axis (or, equivalently, the plane perpendicular to the axis) is selected with G17 (Z-axis, XY-plane), G18 (Y-axis, XZ-plane) or G19 (X-axis, YZ-plane). If the arc is circular, it lies in a plane parallel to the selected plane.

Using Tormach PCNC 770 7-14 32426 Rev C1-1

tormach P 770 Operator’s Guide

Specifications and Main Features

Frequently Asked Questions

User Manual

1. Preface

1.1 Safety

1.1.1 Electrical Safety

1.1.2 General Operating Safety

Safety Publications

Safety Precautions

1.2 Personal CNC Concept

1.3 Performance Expectations

1.3.1 Cutting Ability

1.3.2 Understanding Accuracy

1.3.3 Resolution, Accuracy and Repeatability of the PCNC

1.4 Scope and Intellectual Property

1.5 Nomenclature

2. Preparation

2.1 Planning for Your PCNC

2.1.1 Electrical Connection

2.1.2 Location and Mounting

2.1.3 Computer Mounting Arrangement

2.1.4 Learning and Training

2.2 Receiving, Unpacking and Checking Shipment

2.2.1 Moving the Crate

2.2.2 Uncrating and Inspection

2.3 Mounting the PCNC

2.3.1 Lifting onto Stand

2.3.1.1 Lifting from Below

2.3.1.2 Lifting from Above

2.3.2 Fixing to Stand

2.3.3 Installing central lubrication pump

2.3.4 Accessories

2.4 Power to the PCNC

2.5 Power for Machine Accessories

2.6 Tormach Machine Controller and Software Installation

2.6.1 Control Computer

2.6.2 Setting Up Your Controller

2.6.2.1 Positioning the Controller

2.6.2.2 Keyboard and Mouse

2.6.2.3 Display

2.6.2.4 Speaker and Microphone Connections

2.6.2.5 Power Connections

2.6.3 Operating the Controller

2.6.3.1 About the Operating System

2.6.3.2 Starting the controller

2.6.3.3 Stopping the controller

2.6.3.4 Mach3 License Installation

2.6.4 Machine Controller Maintenance and Configuration

2.6.4.1 Login and Software Installation

2.7 Connecting and Running the PCNC

2.7.1 Main Switch and Control Panel

2.7.2 Changing the Spindle Speed Range

2.7.3 Computer Control of the Spindle and Coolant

2.7.4 MDI for Entering G- and M-code Commands

2.7.5 Jogging the Axes

2.8 Summary

3. Making Your First Part

3.1 Coordinates

3.1.1 Referencing the Machine

3.2 Loading a Demonstration Program

3.3 Running the Demonstration Part-program

3.3.1 Part Material

3.3.2 Setting Work Offsets

3.3.3 Cutting in Air

3.3.4 Cutting the Actual Part

3.3.5 Summary

4. Routes from an Idea to a Part

4.1 Controlling the PCNC

4.2 Choosing the Appropriate Design Software

4.3 Software for CAD/CAM

4.3.1 3D CAD

4.3.2 2D CAD

4.3.3 CAM

4.3.4 Running the G-code

4.3.5 CAD/CAM Systems

4.4 Programming with Wizards

4.4.1 Machining Wizard Concept

4.4.1.1 Selecting and Running a Wizard

4.4.1.2 Standard Wizard Features