Page 1
Southwestern Industries, Inc.
2615 Homestead Place
Rancho Dominguez, CA 90220-5610 USA
T | 310-608-4422 |F | 310-764-2668
Service Department: 800.367.3165
Document: 26728
Version: 051013
TRAK
Programming, Safety, and Operating Manual
LPM
®
e-mail: sales@southwesternindustries.com | service@southwesternindustries.com | web: southwesternindustries.com
Page 2
Copyright 2013, Southwestern Industries, Inc. All rights are reserved. No part of this publication may be reproduced, stored in a retrieval system, or transmitted, in any form or by any means, mechanical, photocopying, recording or otherwise, without the prior written permission of Southwestern Industries, Inc.
While every effort has been made to include all the information required for the purposes of this
guide, Southwestern Industries, Inc. assumes no responsibility for inaccuracies or omission and
accepts no liability for damages resulting from the use of the information contained in this guide.
All brand names and products are trademarks or registered trademarks of their respective holders.
Page 3
i
Southwestern Industries, Inc.
TRAK 2OP Installation, Maintenance, Service & Part List Manual
Table of Contents
1.0 Introduction
1.1 Manual Organization 1
2.0 Safety
2.1 Safety Publications 3
2.2 Danger, Warning, Caution and Note
Labels and Notices Used in this Manual
2.3 Safety Precautions
3.0 Description 10
3.1 Control Specification
3.1.1 ProtoTRAK PMX Hardware Specifications
3.1.2 ProtoTRAK PMX Software Specifications
3.1.3 ProtoTRAK PMX Control Options
3.1.4 DXF File Converter Option
3.1.5 CAM Out Option
3.1.6 How to Buy Software Options
3.2 Display Pendant
3.2.1 Program Panel
3.2.2 Run Panel
3.2.3 Pendant Right Side
3.3 Machine Description
3.3.1 Overall Machine Dimensions
3.3.2 Machine Specifications
3.3.3 Maximum Spindle Torque and Horsepower
3.3.4 Electrical Cabinet
3.3.5 Computer Module
3.3.6 Servo Motors
3.3.7 Servo Drives
3.3.8 Spindle
3.3.9 Spindle Motor & Drive
3.3.10 Automatic Draw Bar Assembly
3.3.11 Retention Knobs
3.3.12 Tool Changer
3.3.13 Drive Train, Axes
3.3.14 Worktable
3.3.15 Limit/Home Switches
3.3.16 Lubrication System
3.3.17 Coolant and Coolant Wash System
3.3.18 Pneumatic System
3.3.19 Enclosure Doors
3.3.20 Beacon Lights
3.3.21 Chip Removal System
3.3.22 Work Lamps
4.0 Basic Operation 27
4.1 Machine and Control Power On
4.2 Control and Power Off
4.2.1 Energizing the Servos
4.2.2 Homing the Machine
4.2.3 Warming Up the Machine
4.2.4 Current and Staged Control Views
4.3 Spindle Operation
4.4 Electronic Handwheel
4.4.1 Manual Axis Movement
4.4.2 Feed Override
4.4.3 Spindle Override
4.5 Multiple Uses of the GO Button
4.6 Multiple Uses of the STOP Button
4.7 Emergency Stop
4.8 Enclosure
4.8.1 Front Door
4.8.2 Side Doors
4.8.3 Positioning the Control Panel
4.9 Coolant
4.9.1 Coolant ON/OFF
4.9.2 Coolant Wash
4.9.3 Coolant Hose
4.9.4 Checking Coolant Levels
4.10 Air
4.10.1 Air Hose
4.10.2 Air Blast
4.10.3 Checking Air Pressure
4.11 Chip Removal
4.11.1 Auger Operation
4.12 ATC Operation
4.12.1 Advancing the Carousel
4.12.2 Manual Tool Load and Unload
4.13 Lubrication
4.14 Help Functions
4.14.1 Math Helps
5.0 Definitions, Terms & Concepts 34
5.1 ProtoTRAK PMX CNC Axis Conventions
5.2 Part Geometry and Tool Path Programming
5.3 Planes and Vertical Planes
5.4 Absolute and Incremental Reference
5.5 Referenced and Non-Referenced Data
5.6 Incremental Reference Position in Programming
5.7 Tool Diameter Compensation
5.8 Tool Diameter Compensation When Contouring in
Z with Part Geometry
5.9 Connective Events
5.10 Conrad
5.11 Memory and Storage
5.12 Current and Staged Views
6.0 DRO Mode 42
6.1 Entering Dimensions
6.2 Reference Locations
6.3 Power Feed
6.4 GO TO
6.5 Return to Absolute Zero
6.6 Spindle Operation
6.7 Axis Motion in the DRO Mode
Page 4
ii
Southwestern Industries, Inc.
TRAK 2OP Installation, Maintenance, Service & Part List Manual
7.0 Program Mode Part 1: Getting 46
Started & General Information
7.1 Programming Overview
7.2 Enter Program Mode
7.3 Program Header Screen
7.3.1 Program Name
7.3.2 General Program Options
7.3.3 Program Header Softkeys
7.4 Assumed Inputs
7.5 Z Rapid Positioning
7.6 Softkeys within Events
7.7 Programming Events
7.8 Editing Data While Programming
7.9 LOOK
8.0 Program Mode Part 2: 54
Program Events
8.1 POSN: Position Events
8.2 DRILL Events
8.3 BOLT HOLE Events
8.4 MILL Events
8.5 ARC Events
8.6 POCKET Events
8.6.1 Circular Pocket
8.6.2 Rectangular Pocket
8.6.3 Irregular Pocket
8.6.4 Tool Path in Pocket Events
8.6.5 Zigzag Z Depth Cuts
8.6.6 Conrad in Pocket Events
8.6.7 Bottom Finish Cut
8.6.8 Face Mill Event
8.7 ISLAND Events
8.7.1 Circular Island
8.7.2 Rectangular Island
8.7.3 Irregular Island
8.8 PROFILE Events
8.8.1 Circle Profile
8.8.2 Rectangular Profile
8.8.3 Irregular Profile
8.9 HELIX Events
8.10 Subroutine Events
8.10.1 REPEAT
8.10.2 MIRROR
8.10.3 ROTATE Z Axis
8.11 COPY Events
8.11.1 Copy Drill to Tap
8.12 THREAD MILL Event
8.13 PAUSE Events
8.14 TAP Events
8.14.1 Tapping Notes & Recommendations
8.15 ENGRAVE Event
8.16 Auxiliary (AUX) Functions Event
9.0 Program Mode Part 3: 79
The Auto Geometry Engine (A.G.E)
Programming
9.1 Starting the A.G.E.
9.2 A.G.E. Mill Prompts
9.3 A.G.E. Arc Prompts
9.4 Skipping Over Prompts
9.5 The OK/NOT OK Flag
9.6 Ending A.G.E.
9.7 Guessing Data
9.8 LOOK and Guess
9.9 Calculated Data
9.10 Arcs and Conrads
9.11 Tangency
10.0 Edit Mode 86
10.1 Delete Events
10.2 Spreadsheet Editing
10.2.1 Selecting Data to be displayed on the Search Edit Table
10.2.2 Sorting Data
10.2.3 Making Global Changes to Data
10.3 Erase Program
10.4 Clipboard
10.5 G-Code Editor
10.6 Update GCD
10.7 Next Program
11.0 Program Set Up Mode 98
11.1 Part / Fixture Management
11.1.1 PICTURE
11.1.2 NOTES
11.1.3 GO TO
11.1.4 Z SAFETY
11.1.5 Part/Fixture Management LOOK
11.2 Tool Management
11.2.1 TOOL CRIB
11.2.2 REMOVE TOOL
11.2.3 NOTES
11.2.4 DISABLE LOC
11.3 TOOL PATH
11.3.1 Softkeys in Tool Path
11.4 Run Strategy
11.5 Tool Recon (Reconciliation)
12.0 Machine Set Up Mode 114
12.1 Tool Loading
12.1.1 Tool Status Box
12.1.2 Tool Loading Table
12.1.3 REMOVE TOOL
12.1.4 ADD TOOL
12.1.5 CALL TOOL
12.1.6 RETURN TOOL
12.1.7 RESET ATC
12.2 Checklist
12.3 Service Codes
13.0 Run Mode 122
13.1 Run Mode Screen
13.2 Starting to Run
13.2.1 Starting to Run – Single Program
13.2.2 Starting to Run – Master Program
13.3 Program Run
13.4 TRAKING
13.5 Program Run Messages
13.6 STOP
Page 5
iii
Southwestern Industries, Inc.
TRAK 2OP Installation, Maintenance, Service & Part List Manual
13.7 Feedrate and Speed Overrides
13.8 Data Errors
14.0 Program In/Out Mode 126
14.0.1 Filenames and File Extensions
14.1 Softkey Selections in the Program In/Out Mode
14.2 Basic Navigation of Program In/Out Mode Screens
14.2.1 Basic Parts of the Program In/Out Mode Screens
14.2.2 Softkeys in the Program In/Out Mode Screens
14.3 Opening a File
14.3.1 Creating a Master Program
14.3.2 Preview Graphics
14.4 Saving Programs
14.5 Copying Programs
14.6 Deleting Programs
14.7 Renaming
14.8 Backing Up
14.9 Converters™
14.9.1 Activating Converters
14.9.2 Converting From a Different Format
into a ProtoTRAK PMX CNC
14.9.3 Converting From the ProtoTRAK PMX CNC to
a Different Format
14.10 ProtoTRAK and TRAK CNC Compatibility
14.10.1 File Formats
14.10.2 Opening .MX3 and .PT4 files on a
ProtoTRAK PMX CNC
14.10.3 Running ProtoTRAK PMX Files on ProtoTRAK
and TRAK CNC Controls
14.11 Running G Code Files (GCD)
14.11.1 G Codes Recognized by the ProtoTRAK PMX
GCD Converter
14.11.2 M Codes Supported by the ProtoTRAK PMX
CNC
14.11.3 Valid Characters for Word/Address Sequences
14.12 Networking
14.12.1 A Basic Peer-To-Peer Network
14.12.2 Assigning a Name and Selecting a Workgroup
14.12.3 Mapping Network Drive
14.12.4 General Information For Advanced Networks
14.13 CAD/CAM and Post Processors
14.13.1 Writing a Post Processor
14.13.2 Convertible G-Codes for CAM converter
14.13.3 Supported Addresses
14.13.4 Format Terms and Definitions
14.13.5 Accepted M Codes
15.0 4th Axis Option 156
15.1 4th Axis Specifications
15.2 Definitions, Terms, and Concepts
15.2.1 Direction of 4th axis
15.2.2 Feed rate
15.3 DRO Mode
15.3.1 JOG
15.3.2 GO TO
15.3.3 RETURN ABS 0
15.3.4 SET A
15.3.5 REF 4th Axis
15.4 PROG Mode
15.4.1 POSN
15.4.2 MILL 4 AXIS
15.4.3 ENGRAVE 4 AXIS
15.4.4 AUX Event
15.4.5 LOOK
15.5 PROG SETUP Modes
15.5.1 PART/FIX MGMT Screen
15.5.2 Tool Path
15.6 MACHINE SETUP Mode
15.6.1 SERV CODES Screen
15.6.2 4th AXIS ON / OFF
15.7 PROG I/O
15.7.1 4th Axis G-Code notes
15.8 4th Axis Setup Notes
Page 6
1
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
1.0 Introduction
Congratulations! Your TRAK LPM Milling Machine with the ProtoTRAK PMX CNC is
a brand new concept in smaller lot production. It combines the simplicity of the
ProtoTRAK programming method with innovative systems in tooling, workholding and
job management.
The TRAK LPM is more than a machine. It is a system of machining that helps you to
reduce set ups for smaller run production jobs.
This manual will describe the operation of the machine and the ProtoTRAK PMX CNC.
1.1 Manual Organization
Section 2 of this manual provides important safety information. It is highly
recommended that all operators of this product review this safety information.
Section 3 provides a description of the TRAK LPM and the ProtoTRAK PMX CNC.
Section 4 describes the operation of the milling machine and some basic operations of the
ProtoTRAK PMX CNC.
Section 5 defines some terms and concepts useful in learning to program and operate the
ProtoTRAK PMX CNC.
The ProtoTRAK PMX CNC is organized into seven Modes of operation that are
described in the following sections.
Section 6 DRO: Digital Readout and power feed operations.
Section 7 Programming, Part 1: covers some general programming information and
instructions on starting new programs.
Section 8 Programming, Part 2: Program Events - instructions for the canned cycles, or
events, used to program the ProtoTRAK PMX CNC.
Section 9 Programming, Part 3: the A.G.E., or Auto Geometry Engine, so powerful it gets
its own section.
Section 10 Edit: for routines to make large-scale changes to programs in current memory,
including the powerful Spreadsheet Editing®
Section 11 Program Set Up: Where you can do those set up operations that are possible
with the machine running a different job.
Page 7
2
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Section 12 Machine Set Up: The few operations you must do with the machine idle as
you make the final preparations to run your new job. Also includes the powerful
Checklist so that you can be sure you haven’t overlooked anything.
Section 13 Run: Instructions on running a program to machine your part.
Section 14 Program In/Out: Storing and managing your programs as well as creating a
Master Program.
Section 15 4th Axis Option: Instructions on how to run and program a 4th axis option.
Page 8
3
Southwestern Industries, Inc.
TRAK LPM Installation, Maintenance, Service, & Part List Manual
2.0 Safety
The safe operation of the LPM depends on its proper use and the precautions taken by each
operator.
Read and study this manual and the LPM Programming, Operating, and Care Manual. Be
certain every operator understands the operation and safety requirements of this
machine
Never run the machine with enclosure doors open
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 tool or workpiece.
Never wear gloves, rings, watches, long sleeves, neckties, jewelry, or other loose items
when operating or around the machine.
Use adequate point of operation safeguarding. It is the responsibility of the employer to
provide and ensure point of operation safeguarding per OSHA 1910.212 - Machining
centers.
2.1 Safety Publications
Refer to and study the following publications for assistance in enhancing the safe use of this
machine.
Safety Requirements for Machining Centers and Automatic, Numerically Controlled
Milling, Drilling and Boring Machines (ANSI B11.23-2002) (R2007). Available from The
American National Standards Institute, 1819 L Street N.W., Washington D.C. 20036
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 0210.
2.2 Danger, Warning, Caution, and Note Labels & Notices
As Used In This Manual
DANGER - Immediate hazards that will result in severe personal injury or death. Danger labels
on the machine are red in color.
WARNING - Hazards or unsafe practices that
damage to the equipment. Warning labels on the machine are orange in color.
CAUTION - Hazards or unsafe practices, which
equipment/product damage. Caution labels on the machine are yellow in color.
NOTE - Call attention to specific issues requiring special attention or understanding.
HELPFUL TIP- A technique or tool that can aid you.
before
its use.
could
result in severe personal injury and/or
could
result in minor personal injury or
Page 9
4
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Safety & Information Labels Used On The
LPM Milling Machine
It is forbidden by OSHA regulations and by law to deface, destroy or
remove any of these labels
Page 10
5
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Page 11
6
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Page 12
7
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Page 13
8
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
2.3 Safety Precautions
1. Do not operate this machine before the LPM Installation, Maintenance, Service and
Parts List Manual, Operating & Care Manual have been studied and understood.
2. Do not run this machine without knowing the function of every control key, button, knob,
or handle. Ask your supervisor or a qualified instructor for help when needed.
3. Protect your eyes. Wear approved safety glasses (with side shields) at all times.
4. Don't get caught in moving parts. Before operating this machine remove all jewelry
including watches and rings, neckties, and any loose-fitting clothing.
5. Keep your hair away from moving parts. Wear adequate safety headgear.
6. Protect your feet. Wear safety shoes with oil-resistant, anti-skid soles, and steel toes.
7. Take off gloves before you start the machine. Gloves are easily caught in moving parts.
8. Remove all tools from the machine before you start. Loose items can become dangerous
flying projectiles.
9. Never operate a milling machine after consuming alcoholic beverages, or taking strong
medication, or while using non-prescription drugs.
10. Protect your hands. Stop the machine spindle and ensure that the CNC control is in the
stop mode:
Before changing tools
Before changing parts
Before you clear away the chips, oil or coolant. Always use a chip scraper or brush.
Do not used compressed air to clean the machine.
Before you make an adjustment to the part, fixture, coolant nozzle or take
measurements.
Do not attempt to disable any safety interlock. Never reach around a safeguard.
11. Protect your eyes and the machine as well.
12. Disconnect power to the machine before you change belts, pulley, and gears.
13. Keep work areas well lighted. Ask for additional light if needed.
14. Do not lean on the machine while it is running.
15. Prevent slippage. Keep the work area dry and clean. Remove the chips, oil, coolant and
obstacles of any kind around the machine.
16. Avoid getting pinched in places where the table, saddle or spindle head create "pinch
points" while in motion.
17. Securely clamp and properly locate the workpiece in the vise, on the table, or in a fixture.
Use stop blocks to prevent objects from flying loose. Use proper holding clamping
attachments and position them clear of the tool path.
18. Use correct cutting parameters (speed, feed, depth, and width of cut) in order to prevent
tool breakage due to premature wear.
Page 14
9
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Warning
Retention knobs come in a wide variety of designs, however they often look similar and appear to
be interchangeable, but they are not. Use only the knob that the LPM is designed to use. The use
of the incorrect knob, or the incorrect usage of a knob, may result in injury or property damage.
To ensure the correct knob is chosen, please refer to section 3.3.11, Machine Major
Subassemblies section of this manual
19. Use proper cutting tools for the job. Pay attention to the rotation of the spindle: As
viewed from above, left hand tool for counterclockwise rotation of spindle, and right
hand tool for clockwise rotation of spindle.
20. To prevent damage to the workpiece or the cutting tool, never start the machine
(including the rotation of the spindle) if the tool is in contact with the part.
21. Check the direction (+ or -) of movement of the table when using the jog feature,
clockwise rotation of the EHW moves the axis in the positive direction, counterclockwise
in the negative direction.
22. Don't use dull or damaged cutting tools. They break easily and become airborne.
Inspect the sharpness of the edges, and the integrity of cutting tools and their holders.
Use proper length for the tool.
23. Inspect the retention knobs for damage or excessive wear before each use.
24. Large overhang on cutting tools when not required result in accidents and damaged
parts.
25. Prevent fires. When machining certain materials (magnesium, etc.) the chips and dust
are highly flammable. Obtain special instruction from your supervisor before machining
these materials.
26. Prevent fires. Keep flammable materials and fluids away from the machine and hot,
flying chips.
Page 15
10
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
3.0 Description
This section will provide an overview of features and specifications found on the TRAK
LPM.
3.1 Control Specifications
The new ProtoTRAK PMX CNC retains the basic operations strategies found in all other
models of ProtoTRAK and TRAK CNCs.
3.1.1 ProtoTRAK PMX Hardware Specifications
Jog wheel for TRAKing and positioning
12.1” color active-matrix screen
Industrial-grade Celeron® processor
512 MB Ram
4 User USB connectors
Override of program feedrate
LED status lights built into display
RJ45 Port with 10/100 Ethernet
Override of program spindle speed
4th axis interface
Program storage via a USB flash drive installed in a port in the electrical cabinet.
3.1.2 ProtoTRAK PMX Software Specifications
Software Features - General Operation:
• Clear, uncluttered screen display
• Prompted data inputs
• English language – no codes
• Soft keys - change within context
• Windows® operating system
• Color graphics with adjustable views
• Inch/mm selectable
• Convenient modes of operation
• Absolute Home location
• Spindle load indicator
• Reference to ball lock locations on table
• Dimension reference indicator
• Selectable view between Current and Staged programs
DRO Mode features:
• Incremental and absolute dimensions
• Jog with selectable feed rates
• Powerfeed X, Y or Z
• Servo return to 0 absolute
• Go To Dimensions from convenient reference
• Spindle speed setting with manual override
• Selectable handwheel resolution
Page 16
11
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
• Convenient choice of dimensional references:
Machine Home, Part Zero, Abs Zero and Ball Lock locations
Program Mode Features
• Auto Geometry Engine
• Geometry-based programming
• Tool Path programming
• Scaling of print data
• Multiple fixture offsets
• Programming of Auxiliary Functions
• Event Comments
• Three-axis Geometry conversational programming
• Incremental and absolute dimensions
• Automatic diameter cutter comp
• Circular interpolation
• Linear interpolation
• Look –graphics with a single button push
• List step – graphics with programmed events displayed
• Alphanumeric program names
• Program data editing
• Program pause
• Conrad – automatic corner radius
• Programmable spindle speeds
• Math helps with graphical interface
• Auto load of math solutions
• Tool step over adjustable for pocket routines
• Pocket bottom finish pass
• Selectable ramp or plunge cutter entry
• Subroutine repeat of programmed events
• Nesting
• Rotate about Z-axis for skewing data
• Mirror of programmed events
• Copy
• Copy rotate
• Copy mirror
• Tool data entry in event programming
• Selectable retract in Bore operations
Auxiliary Functions
• Coolant on/off
• Air on/off
• Pulse indexer
• Part change table position
Canned Cycles
• Position
Page 17
12
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
• Drill
• Bolt Hole
• Mill
• Arc
• Circle pocket
• Rectangular pocket
• Irregular Pocket
• Circular profile
• Rectangular profile
• Irregular Profile
• Circle Island
• Rectangular Island
• Irregular Island
• Helix
• Thread milling
• Engrave
• Tapping
• Face Mill
Edit Mode Features
• Delete events
• Erase program
• Spreadsheet editing
• Global data change
• G-Code editor
• Clipboard to copy events between programs
• Move between subprograms in a master program
Program Set Up Mode Features
• Program diagnostics
• Advanced tool library
• Tool names
• Tool length offset with modifiers
• Tool diameters with modifiers
• Tool path graphics with adjustable views
• Program run time estimation clock
• Convenient part/fixture management screen
• Fixture offsets
• Part offsets within fixture
• Convenient manual tool handling when tools required exceed ATC capacity
• Photo storage and display
• Notes
• Z Safety Dimension to prevent crashes
• Tool Crib
• Tool by Tool or Part by Part run strategy
• Convenient Tool Reconciliation between programs and ATC
Page 18
13
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
• Convenient ATC capacity
Machine Set Up Mode Features
• Advanced diagnostic routines
• Software travel limits set in the factory
• Prompted Tool loading and ATC Management
• Checklist to assure nothing is forgotten
• Single key press to get to step needing attention
Run Mode Features
• TRAKing
• 3D CAM file program run
• 3D G code file run with tool comp
• Real time run graphics with tool icon
• Countdown clock for total part cycle time or manual tool change
• Error alarms prevent Run when set up steps are skipped
• Work on Staged programs while Current program runs
Program In/Out Mode Features
• CAM program converter
• Converter for prior-generation ProtoTRAK programs
• DXF/DWG file converter (Optional)
• Selection of file storage locations
• Automatic file back-up routine
• Preview graphics for unopened files
• Networking
• Create Master routine for combining programs
• Transfer of Staged program to Current
• Tool reconciliation for Master Programs
3.1.3 ProtoTRAK PMX Control Options
The DXF File Converter Option
• Import and convert CAD data into ProtoTRAK programs
• DXF or DWG files
• Chaining
• Automatic Gap Closing
• Layer control
• Easy, prompted process you can do right at the machine
CAM Out Converter Option
• Save ProtoTRAK files as CAM files for running on different controls
3.1.4 DXF File Converter Option
The DXF File Converter Option gives you powerful capability for quickly and easily
translating DXF and DWG files into ProtoTRAK programs. If you work with CAD
drawings, we highly recommend that you get a demo of the DXF file converter.
Page 19
14
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
To tell if the DXF File Converter is active on your ProtoTRAK PMX CNC, go to the
options screen using Service Code #318. If the AutoCAD DXF option is in black letters,
it is activated. If it is in gray letters, you will need to purchase the option to activate it.
The DXF Option consists of an Activation Password, and may require an additional
software update. To download the latest version of our DXF software, go to our website
at www.southwesternindustries.com then click ‘Support & Software’ for current
ProtoTRAK CNC, and follow the instructions for downloading the software via a USB
flash drive. See Section 3.1.6 below for instructions on ordering and obtaining your
Activation Password.
The DXF Option has its own manual which is shipped with the software. You may also
view a copy of the manual on our web site.
3.1.5 CAM Out Option
Note: CAM file run by bringing a CAM file into the ProtoTRAK PMX is a standard
feature.
The CAM out Option gives you the ability to create or modify a program using the easy,
intuitive ProtoTRAK interface and then convert that program into a CAM file or G Code
file to use to run other CNCs.
Note: you do not need the CAM Out option to share programs between ProtoTRAK
CNCs.
To tell if the CAM Out feature is active on your ProtoTRAK PMX CNC, go to the
options screen using Service Code #318. If the CAM Out option is in black letters, it is
activated. If it is in gray letters, you will need to purchase the option to activate it.
The software for the CAM Out Option requires an Activation Password for you to use.
See Section 3.1.6 below for instructions on ordering and obtaining your Activation
Password.
3.1.6 How To Buy Software Options
If you did not buy the software options described above with your machine, you may
purchase them later. In order to use these options, a Software Activation Password is
required. These passwords are unique to your ProtoTRAK PMX CNC.
Software Options are not free. You may call your local Southwestern Industries Sales
Representative or Southwestern Industries Inside Sales at 310-608-4422 for a price
quotation.
1. We recommend that you install the latest version of the ProtoTRAK PMX master
software before installing the newest option. See our web site at
www.southwesternindustries.com for software downloads.
Page 20
15
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
2. Go to the ProtoTRAK PMX CNC on which the option is to be installed, use Service
Code 318 to go to the Software Options Screen.
3. Highlight the option you wish to install and press the softkey labeled INSTALL.
4. A screen will appear that advises you how to purchase the option. Near the bottom of
the screen there will be a Hardware Key Serial Number and an Option Serial Number.
Write down both of these numbers.
5. Call your Southwestern Industries Sales Representative or the Southwestern Industries
Order Desk with your purchase order number and the numbers you wrote down in step 4
above.
6. When you receive your Password Activation Number, input it into the ProtoTRAK
where indicated on the screen obtained in step 2 above. Some options require you to
reboot the ProtoTRAK to activate.
7. Refer to the appropriate section of this manual for instructions on using your new
features.
3.2 Display Pendant
The display pendant is integrated into the TRAK LPM on the front right side of the
machine enclosure. The pendant may swing out 80º for your convenience and may be
locked in place at 45º and 80º.
3.2.1 Program Panel
The Program Panel is the upper panel on the front of the Pendant.
INC SET: loads incremental dimensions and general data
ABS SET: loads absolute dimensions and general data
Page 21
16
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
RESTORE: clears an entry, aborts a keying procedure
INC/ABS: switches all or one axis from incremental to absolute or absolute to
incremental position
IN/MM: causes Inch to Metric or Metric to Inch conversion of displayed data
LOOK: part graphics in Program Mode
MODE: to change from one mode of operation to another
CURSOR: moves cursor of highlight in tables, lists or choices and pages between event.
BACK: shifts LCD screen to previous display
HELP: display help information, Math Help or additional functions. Active for
additional functions when the help symbol (a blue question mark) is displayed on the
screen next to the HELP key.
C/S: switches Program Panel from current (the part program you are running) to staged (a
different part program you are preparing to run in the future) and back. You can tell if
you are in current or staged by the color of the Soft Keys: white Soft Keys tell you that
you are in the Staged View.
Keyboard Soft Keys:
Beneath the display are 10 keys that are labeled with arrows. These keys are called
software programmable or soft keys. A description of the function or use of each of these
keys will be shown at the bottom of the display directly above each key. If, at any time,
there is no description above a key, that key will not operate.
Sometimes the description or function of the key is visible but grayed out. This indicates
that the particular function is not available because of some other condition. For example,
if a program is not loaded into memory, then the softkey in Edit mode will be gray.
Emergency Stop Switch
The emergency stop (E-stop) switch kills all power to the spindle and ProtoTRAK's
servomotors. The computer and pendant remain powered. To resume working from an
emergency stop, you must twist to release the emergency stop button and press the green
energize servos button.
The Liquid Crystal Display (LCD)
The display of the ProtoTRAK SMX CNC is a 12.4" active-matrix color LCD. The very
top is the Status Line that shows the overall status of the ProtoTRAK SMX CNC.
Status line information includes:
Current Mode
Current program part number
Current tool number
Whether the X, Y and Z dimensions are in inch or millimeter (mm).
Just above the soft keys is a data input line that appears when an input is required.
Page 22
17
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
3.2.2 Run Panel
The Run Panel is the lower panel on the front of the pendant.
Spindle Keys
FWD: turns the spindle on in the forward direction in DRO Mode
OFF: turns the spindle off in the DRO Mode
REV: turns the spindle on in the reverse direction in the DRO mode
Feed Keys
GO: initiates axis motion in DRO Mode or during a stop condition in Run Mode
STOP: halts axis motion
Electronic Hand Wheel Keys
Electronic Hand Wheel: used to control X, Y, Z axis positioning, spindle rpm override,
and axis feed override. There are 100 positions or detents per revolution.
SPINDLE OVERRIDE: enables handwheel to control spindle rpm override from 0 to 150
percent in 2% increments.
FEED OVERRIDE: enables handwheel to control axis feed override from 0 to 150
percent in 2% increments.
EHW: enables handwheel to control positioning along X, Y, Z axes.
X, Y, Z: selects axis to be controlled by Electronic Handwheel.
.0001in / .002mm: selects incremental axis motion per handwheel detent. One revolution
equals (.0001in x 100) 0.01in.
.001in / .02mm: selects incremental axis motion per handwheel detent. One revolution
equals (.001in x 100) 0.1in.
.01in / .2mm: selects incremental axis motion per handwheel detent. One revolution
equals (.01in x 100) 1.0in.
FAST: selects fast axis motion for coarse movement up to 300 ipm.
Auxiliary Function Keys
COOLANT: press to turn coolant on (ON LED is lit). Press again to turn coolant on
(AUTO LED is lit) when commanded by the program in Run Mode. Press again to turn
coolant off.
Page 23
18
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
AIR: controls air blast from spindle to help clear chips. Press to turn air on (ON LED is
lit). Press again to turn air on (AUTO LED is lit) when commanded by the program in
Run Mode. Press again to turn air off.
WASH: press to activate chip wash to help move chips down to the chip auger location.
DOOR LOCK: activates the door lock mechanism whenever a program or other
automatic move is running. The LED light on the key is on when the door lock
mechanism is active (it is possible for the door to be locked without the light being on).
CHIP REMOVAL: press Forward (FWD) to activate chip auger, press again to turn off.
Press and hold Reverse (REV) to drive chip auger in reverse to help clear jams (make
sure FWD is off).
ATC INDEX: press forward (FWD) to index the automatic tool changer carousel forward
by one tool. Press Reverse (REV) to index the automatic tool changer carousel
backwards by one tool. The door must be closed.
3.2.3 Pendant Right Side
Inset on the right side of the pendant are four USB ports for the thumb drive, keyboard,
mouse, etc. Above these is a green Servo On button that must be pressed to activate
machine motion following power start up or after the E Stop button is pressed.
Page 24
19
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
3.3 Machine Description
Page 25
20
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
3.3.1 Overall Machine Dimensions
Width of LPM without chip cart and auger chute 89.75”
Depth of LPM 88”
Height of LPM with head all the way up 103”
Width of LPM with chip cart and side doors open 157”
Minimum height to fit LPM through doorway (Z cable carrier collapsed) 85”
Machine weight 7650 lbs.
3.3.2 Machine Specifications
Table Dimensions
Table size 35.38” X 19.63”
Number of tee slots and pitch 5 @ 100 mm
Tee slot width 0.710” or 18 mm
Table maximum load 1000 lbs.
Ball Lock ® hold down force 2250 lbs @ 35 in/lbs of
torque
Travel
X-axis 31”
Y-axis 18.5”
Z-axis 21”
Maximum distance from spindle nose table surface 24”
Minimum distance from spindle nose table surface 3.375”
Maximum swing clearance from spindle center to column 19.25”
Maximum Rapid speed X-axis, inches per minute 800
Maximum Rapid speed Y-axis, inches per minute 800
Maximum Rapid speed Z-axis, inches per minute 700
Spindle
Tool holder type CAT40
Spindle nose diameter 2.75
Maximum RPM 8000
Automatic Tool Changer
Tool Capacity 16
Maximum tool weight including holder 15 lbs
Maximum tool diameter 3.14
Carousel speed .8 sec from station to station
Tool selection system Bi-directional/ shortest path
Retention knob See section 3.3.11
Air Requirements
Pressure 90 psi
Quality Air dried/ water separator upstream of the LPM
Page 26
21
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
3.3.3 Maximum Spindle Torque and Horsepower
0
10
20
30
40
50
60
0 2000 4000 6000 8000
Torque (ft-lbs)
RPM
Torque vs RPM
Continuous Torque
Peak Torque
0
2
4
6
8
10
12
14
16
0 2000 4000 6000 8000
HP
RPM
HP vs RPM
Continuous HP
Peak HP
The following graphs illustrate the continuous and peak torque vs. RPM and horsepower
vs. RPM for the LPM machine at the spindle. Peak torque and horsepower values can
only be attained for a short period of time before the spindle drive will fault out to protect
the motor.
Page 27
22
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Note - Maximum work capacities are dependent on a lot of variables that cannot be
Warning!
The spindle unit is not field serviceable. If the bearings go bad the
entire spindle cartridge will be replaced.
controlled by the machine manufacturer. Each one of the following will have an impact
on the above numbers: speeds, feeds, cutter, cutter sharpness, material, setup, coolant and
machine adjustments.
3.3.4 Electrical Cabinet
The electrical cabinet is found at the rear of the LPM on the right side. The electrical
cabinet contains the main control hardware for the machine. The main components are as
follows: computer module, AC spindle drive, servo drives, input/output modules, relays
and contactors.
3.3.5 Computer Module
The computer module is the heart and soul of the machine. All of the inputs and outputs
are feed through this module. The computer module controls the program panel, run
panel, AC spindle drive, servo drives, motor signals and feedback and input/output
modules. Inside of the computer module is a motherboard, motion control board and an
applications board along with a power supply.
The computer module also contains 4 more USB ports and a network port. We ship the
machine with 3 USB ports having something plugged into them. The 3 USB ports
contain the following: machine option key, a D drive for part storage and an overlay
interface USB cable. The network port is available to the user if they want to network the
control to an offline computer or network.
3.3.6 Servo Motors
The LPM can run up to 4 axis motors. The 4th motor would be used to control a 4th axis
indexer. The motors used on the X and Y axis are rated for 4.2 ft/lbs of torque. The Z
axis motor is rated at 8.11 ft/lbs and also contains a mechanical brake the holds the head
in position when the power is turned off to the machine.
3.3.7 Servo Drives
The LPM can also contain up to 4 servo drives. The 4th amp would be used to control a
4th axis indexer or rotary table. The servo drives receive signals from the computer
module, which in turn send signals to the servo motors.
3.3.8 Spindle
The spindle is contained within a cartridge and CAT 40 tool holders must be used. The
spindle bearings are permanently lubricated and require no additional attention by the
user. The spindle is also air cooled, and has an air purge system that is automatically
activated during the tool change sequence, it blows air down the spindle to prevent chips
from being trapped between the holder and spindle taper.
Page 28
23
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Warning!
Retention knobs come in a wide variety of designs, however they often look
similar and appear to be interchangeable, but they are not. Use only the knob
that the LPM is designed to use. The use of the incorrect knob, or the incorrect
use of a knob, may result in injury and/or damage to the mechanism.
3.3.9 Spindle Motor & Drive
The spindle motor is 10 HP and drives the spindle via a timing belt. The ratio between
the spindle and spindle motor is 1 to 1. The RPM range for this machine is 150 to 8000
RPM.
3.3.10 Automatic Draw Bar Assembly
The automatic drawbar is an assembly consisting of an air cylinder and an actuator that
unclamps the tool. Tooling is changed by means of the Automatic Tool Changer (ATC),
or can be done manually by pressing and holding the “Unclamp” button. Tools are
clamped when the button is released. A clamping force of approximately 1500 lbs is
generated to clamp the toolholder to the spindle. The Automatic Draw Bar Assembly uses
full system air and requires no adjustment. The air cylinder that does the clamping and
unclamping is lubricated with a small cup. Make sure to check the oil level in this cup on
a regular basis.
3.3.11 Retention Knobs
The LPM uses CAT40 retention knobs as shown below. Tightening to the proper torque
value is important for all retention knobs. Please see the retention knob manufacturer for
the proper torque.
Retention knobs
Page 29
24
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
3.3.12 Tool Changer
The tool changer is an armless carousel type automatic tool changer that has a capacity of
16 tools. The carousel is mechanically indexed by means of a Geneva mechanism. The
position of the carousel is controlled by a signal from Home Position Sensor. As an
additional safety feature, the ATC also has Tool Detect Sensor at the “ready position”.
This means if a tool is sitting in this position and the control tries to put the tool in the
spindle into this spot, an error will be generated by the control.
3.3.13 Drive Train, Axes
Each axis (X, Y and Z) rides on precision linear guideways, with four preloaded
recirculating ball carriages. Each axis is moved via an 8 mm pitch ballscrew. The axis
motors direct drive the ballscrew.
3.3.14 Worktable
The LPM table utilizes Ball Lock® technology as well as conventional T-bolt
construction. Each Ball Lock mechanism has a hold-down force of 2250 lbs when 35
in/lbs of torque is applied to the screw. The software on the LPM is based on these ball
locks as we ask the user which ball lock location they wish to run the part on. The 3
locations are called ball lock A, B and C.
3.3.15 Limit/Home Switches
Each axis has a limit switch, which serve two purposes, to protect the LPM in the event
of an over-travel situation in either the positive or negative direction, and secondly for the
purpose of homing the machine. The following table describes where the cams are that
trigger the limit switches.
Page 30
25
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Limit Switch Cam Locations
Axis End
Location of Cam Bracket
Cam Location
X-axis Negative End
Left hand side of the table (front)
Upper channel
X-axis Positive End
Right hand side of the table (front)
Lower channel
Y-axis Negative End
On the base casting, beneath the saddle
(back)
Upper channel
Y-axis Positive End
On the base casting, beneath the saddle
(front)
Lower channel
Z-axis Negative End
On the column casting (upper)
Right hand channel
Z-axis Positive End
On the column casting (lower)
Left hand channel
ATC Home Position
Sensor
ATC shroud
Target bolt on the
carousel
ATC Sliding Body,
home
Bracket-Sliding Body Support, left
Sliding Body
ATC Sliding Body,
Advanced
Bracket-Sliding Body Support, right
Sliding Body
WARNING!
It is not recommended that the position of the limit switches be
changed. They are preset at the factory and should require no
additional adjustments. Should any major adjustments be required,
Service Codes 500, 501, 502 and 505 may need to be performed.
3.3.16 Lubrication System
The automatic lubricating system is a centralized system. It is located at the rear of the
machine. While the system is automatic, it is recommended that after long idle periods,
the machine be manually lubricated by pressing, holding (about five seconds) until the
system is charged, then releasing the square green button located on the lubricator, repeat
three to five times. The lubricating system delivers 2 shots of oil when the machine is
turned on at the disconnect switch, and 1 shot every 30 minutes while the machine is
running. The lubrication reservoir should be maintained on a daily basis, filling only
with high quality lubricating oil. All pneumatic components are lubricated by means of
an inline oiler.
3.3.17 Coolant and Coolant Wash System
The coolant and coolant wash system uses two pumps, one for providing coolant to the
work, and the other for washing the chips into the auger. Wash areas can be controlled by
the flexible coolant lines found at the base of the enclosure, both left and right-hand
sides. Coolant wash can also be done with the use of the hose and nozzle found on the
front exterior of the enclosure. The coolant feature must be turned on at the hard key on
the Run Panel.
The coolant tank holds approximately 55 gallons of coolant.
Page 31
26
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
CAUTION!
Always observe low air pressure and low oil level warnings.
CAUTION!
Do not attempt to disable or override the safety interlock.
WARNING!
Use extreme care when working with the auger, serious injury
could occur.
3.3.18 Pneumatic System
The machine requires a supply of compressed air between 85-100 psi with a
recommended air supply of ½” I.D. Air pressure to pneumatic components, the ATC
slide mechanism, air blast and air purge (internal spindle) can be controlled individually
by means of the adjusting valves located at the back of the LPM.
3.3.19 Enclosure Doors
The front door has an electro-mechanical safety interlock that must be engaged when
running a CNC program. If the door is opened during a machining operation, the
program will be shut down.
Do not open the door during a tool change. If you do this accidentally, see section 12.1.7
for instructions on resetting the ATC.
The enclosure is also equipped with left and a right latched and lockable access doors.
3.3.20 Beacon Lights
The machine has a beacon light attached to the top of the machine to give the user status
of what is going on. The lights perform as follows:
a. The green light is illuminated when the machine is running a program.
b. The yellow light is illuminated when operator input is required, like when a part
change needs to be done.
c. The red light is illuminated when an alarm has occurred.
3.3.21 Chip Removal System
The LPM uses an auger chip removal system. When the forward direction is chosen on
the run panel, the auger will displace chips into the chip cart. It can be run momentarily
in the reverse direction in order to free a jam.
3.3.22 Work Lamps
The LPM comes equipped with two fluorescent work lamps, which come on
automatically when the power is turned on.
Page 32
27
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
4.0 Basic Operation
Caution!
If the LPM has been sitting idle for long periods of time with the
power on, then you should manually lubricate the machine. See
section 3.3.16 for instructions.
This section covers the basic operation of the machine and control issues that apply to
more than one Mode or are not covered in the sections on the individual Modes.
4.1 Machine and Control Power On
To turn the ProtoTRAK PMX CNC on, turn on the main breaker on the rear control
cabinet.
The Windows operating system and the ProtoTRAK PMX CNC software will take a few
seconds to load from the system's flash memory. If you have connected the ProtoTRAK
SMX CNC to a network, it may take as long as 90 seconds for the communications to be
established. When complete, the ProtoTRAK PMX CNC Select Mode screen will appear.
4.2 Control and Power Off
IMPORTANT: the system must be turned off properly. First press the BACK hard key
until the SHUT DOWN soft key appears on the menu. Press the SHUT DOWN soft key
and a warning message will appear:
“Warning ProtoTRAK shutdown”
Press YES if you wish shut down the ProtoTRAK. The Microsoft Windows screen will
be displayed with the message “Windows is shutting down”. Do not turn off the Main
Breaker on the rear control cabinet until the screen goes black. If the CNC is not shut
down properly you may lose unsaved data such as programs or certain machine
configurations.
Note: When you turn the PROTOTRAK PMX CNC off, always wait a few seconds
before turning it back on.
4.2.1 Energizing The Servos
Power On turns on the Main system software, but not the X, Y, and Z servo motors. To
do this press the green SERVO ON button which is located on the right side of the
pendant. If this is not done and an attempt is made to move the machine an E-Stop error
message will appear. Pressing the SERVO ON button will erase this message.
4.2.2 Homing The Machine
Press the HOME SET soft key to send the machine to the Machine Home Position. The Z
axis will retract to tool change position and the carousel will rotate to position no. 1. Then
the X and Y axis will rapid to machine home. The machine may be operated in a manual
mode, but running a program without Homing the machine is prohibited. An error
Page 33
28
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
message “Machine has not been homed” will appear and can be cleared by performing
the Homing operation.
4.2.3 Warming Up The Machine
A proper warmup cycle is necessary to extend the life of the machine as well as
maintaining repeatability. Putting a cold spindle under load can produce premature
bearing failure. Warming up the spindle allows bearings, supports and shaft to reach their
designed dimensions through thermal expansion. Warming up the machine axis by
moving through its entire machine envelope ensures that lubrication reaches all areas of
the working envelope and helps to eliminate premature wear. In addition, thermal
expansion of the axis must be taken into consideration. At the beginning of machine
operation, thermal expansion is not stabilized and workpieces machined during this
period may not be finished accurately.
Once the machine is Homed you will be asked whether you want the machine to perform
a warm-up exercise program of 10 or 20 minutes. A dialogue box will appear if the YES
soft key is pressed. Follow the instructions that are listed on the screen.
Note: The Z axis must be set to a minimum height so the machine will clear any part or
fixturing.
The X and Y axis will move through a stroke of 17.0”and the Z axis will move from tool
change position to the position established in the procedure above. All three axis move at
150.00 inches per minute individually. The spindle will run at 500 rpm and a countdown
clock is displayed to show how much time is left in the cycle. When the cycle is
completed all operations may be performed on the machine.
4.2.4 Current And Staged Control Views
CURRENT MODE enables you to perform all manual and Run Mode operations and
view all the screens that pertain to these operations. In CURRENT MODE you can run a
part, use the Pulse generator to move the machine, load and unload tools, including many
other operations. In this mode the lettering in the soft key menu at the bottom of the
screen is black with a grey background.
STAGED MODE is a ProtoTRAK software feature that drastically reduces setup time for
the next part that is scheduled to run. While the machine is CURRENTLY running
production, the operator can write, edit, input or output programs, enter tool and fixture
offsets, and tool path can be verified. In STAGED MODE the lettering is blue with a
white background. Following is a list of modes the operator can use in STAGED MODE
that will not affect the CURRENT MODE of operation.
a. PROGRAMMING
b. PROGRAM SETUP
c. MACHINE SETUP(Checklist Only)
d. PROGRAM IN/OUT
e. EDIT
Page 34
29
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Operations that cannot be performed are:
a. DRO Mode
b. Tool load and unload
c. RUN
4.3 Spindle Operation
The three buttons on the front control, FORWARD, STOP, REVERSE, will operate the
spindle in DRO, Part Fixture Mgmt., and Run mode.
4.4 Electronic Handwheel
4.4.1 Manual Axis Movement
In DRO mode all axis can be moved by the Electronic Handwheel on the front control
panel. The center EHW button turns on the Hand Wheel and the operator can then choose
which axis to move. Inch or metric increments can be chosen by pressing the inch/mm
button on the front control panel in increments of .0001”/.002 mm, .0010”/.025mm,
.0100”/.25mm, and .1000”/2.54mm.
4.4.2 Feed Override
Feed override is located below the Electronic Handwheel. When this button is pressed the
operator can adjust the rapid rate and feed rate of the machine in 2% increments by
rotating the Electronic Hand Wheel clockwise or counterclockwise.
4.4.3 Spindle Override
Spindle override is located above the Electronic Handwheel. When this button is pressed
the operator can adjust the spindle rpm’s in 2% increments by rotating the Electronic
Hand Wheel clockwise or counterclockwise.
4.5 Multiple Uses Of The GO Button
a: Running a program.
b: Loading and unloading tools to and from the carousel
c: Positioning the machine in GO TO mode
d: Using the Power Feed mode
4.6 Multiple Uses Of The STOP Button
a: Stops axis movement when running a program
b: Stops axis movement in GO TO mode
c: Stops axis movement in Power Feed mode
d: Stops a tool change operation. This should only be done if the operator perceives there
to be a problem in the sequence (eg: calling a tool from the carousel with a tool still in the
spindle). Refer to Section 4.4 of the service manual to resume tool change operations.
This does not exit the user out of a program that is running. Pressing GO will resume
operation
Page 35
30
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
4.7 Emergency Stop
Press the button to shut off power to the spindle motor and axis motors. Rotate the switch
to release.
4.8 Enclosure
The LPM is fully enclosed enabling flood coolant and/or air blow aiding in efficient
machining of any workpiece. Three access doors permit easy chip removal and fixture
placement.
4.8.1 Front Door
The door is automatically locked during tool change operations. During RUN mode the
door can be opened. This will stop the spindle and all axis motion. Coolant and air blow
will be shut off. Operation can resume by closing the door and pressing GO. The DOOR
LOCK/UNLOCK hard key can be used to prevent the door from being opened during
RUN mode. When a program is finished running, the door will automatically unlock
permitting the operator to gain access to the inside of the machine. If the operator
resumes production (ig: pressing GO), the door will automatically lock until the cycle is
complete.
4.8.2 Side Doors
There are access doors located on both sides of the machine. Pressing the lower button on
the door latch releases the handle. Rotate the handle to open the door. When closing the
door simply push the handle in to close.
4.8.3 Positioning The Control Panel
A lock pin is located above the control panel. The panel can swivel in and out when the
pin is pulled out and locked at 45 and 80 degrees when the pin is pushed in.
4.9 Coolant
Oil or water soluble coolant is recommended for the machine. The coolant tank is self
contained and may be rolled out from under the machine for cleaning and machine
maintenance.
4.9.1 Coolant ON/OFF
The coolant ON//OFF button is located on the front control panel. Press the button for 1
sec. for manual coolant on and off. The coolant can also be turned on and off in auto
mode by holding the button for approximately 3 seconds. (ie: program auxiliary events).
4.9.2 Coolant Wash
The coolant wash button is located on the front control panel. When turned on coolant
flows through the base of the machine flushing chips into the auger.
Page 36
31
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
4.9.3 Coolant Hose
A coolant hose is supplied to aid in cleaning the machine of chips. The coolant pump
must be turned on to use this hose. To increase the pressure through the hose, turn off the
coolant valves located below the spindle.
4.9.4 Checking Coolant Levels
The coolant level should be higher than the baffles located near the coolant pumps and
can be checked visually.
4.10 Air
A single air line is required and located at the rear of the machine. A shut-off valve is
supplied below the main pressure gauge.
4.10.1 Air Hose
A hand air hose is located to the right of the front door and may be used anytime during
operation.
4.10.2 Air Blast
Two air lines are located below the spindle and can be turned on and off by a button on
the front control panel or by the program using an auxiliary event.
4.10.3 Checking Air Pressure
Two pressure gauges are located at the rear of the machine. One regulates the main
incoming pressure to the machine, the second regulates how much air runs through the
spindle bearing assembly keeping out contamination.
4.11 Chip Removal
Chips can be removed with the auger located in the lower front base of the machine.
Chips will exit through the chip spout located on the left side of the machine.
4.11.1 Auger Operation
The auger button is located on the front control panel and can rotate the auger forward or
reverse. To run the auger in reverse you need to hold the reverse button down. Reverse
would only be used in cases where the auger screw gets jammed. This might help free it
up.
If the auger gets jammed and the reverse feature does not free it up, then you should press
the E-stop and pull the coolant tank out towards the front of the machine so you will be
able to see where the auger is jammed. Free up the jammed material and then push the
tank back in place. Do not place your hand down in the chute when it is running or
power is on trying to free the jam. Never remove the chute when power is on.
We recommend the auger be run continuously when the parts you are cutting produce a
lot of chips. Failure to do so may cause chips to overflow into the coolant tank.
Page 37
32
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
4.12 ATC Operation
4.12.1 Advancing The Carousel
The tool carousel button is located on the front control panel and can rotate the carousel
clockwise or counterclockwise. The door must be closed in order for the carousel to
rotate.
4.12.2 Manual Tool Load and Unload
The green button located on the front of the spindle headstock is the clamp and unclamp
button. Manually loading and unloading tools can only be done with the door open.
4.13 Lubrication
The lubrication reservoir is located at the rear of the machine. The unit cycles
automatically when the control is on. A button is located on the front of the unit and
when pressed will pressurize the lubrication system. The pressure gauge will register a
value and the button should be released. Only when the button is released does oil get
supplied to all parts of the machine.
4.14 Help Functions
When a blue question mark appears next to the HELP hard key, that means special
functions or configuration settings are available for the current operation. For example, at
the program header with the highlight on the program name, the blue question mark
appears. Pressing the HELP key at that time will call up a table with alpha and special
characters you can use to name your program.
4.14.1 Math Helps
When the blue question mark does not appear, pressing HELP will initiate the Math
Helps.
The first Math Helps screen. Choose among the alternatives based on the information you
need to calculate.
Page 38
33
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Math Helps are powerful routines that enable you to use the data you have available to
calculate missing print data.
For example, Math Help type 28 enables you to solve an entire right triangle by giving
two known pieces of data. To exit from the Math Help, press the Mode key.
Math Help 28 In this example, by entering the length of line A and the value of angle G,
the other values are calculated
You may have the Math Help solutions load directly into your program. This saves you
from having to write down the solution and then key it in. While you are programming
the event that needs the data from Math Help, simply press the HELP key to start the
Math Help. Once a solution is obtained, you will have the following soft key selections:
LOAD BEGIN: will load the displayed solution into the event as the X and Y beginning.
LOAD END: will load the displayed solution into the event as the X and Y end.
LOAD CENTER: will load the displayed solution into the event as the X and Y center.
NEXT SOLUTION: when there is more than one solution to the problem, this will
display the alternative solutions.
EDIT: this allows you to go back to the data you entered in order to make changes. Once
you do this, the Resolve key will appear.
RESOLVE: press this to have the Math Help use the new data to give new solutions.
Page 39
34
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
5.0 Definitions, Terms & Concepts
5.1 ProtoTRAK PMX CNC Axis Conventions
Hint: It is much easier to program if you imagine the tool is moving and think of the tool
movement rather than focus on the machine table and saddle movement.
X Axis: positive X-axis motion is defined as the table moving to the left when facing the
mill. Consequently, measurement to the right is positive on the workpiece.
Y Axis: positive Y-axis motion is defined as the table moving toward you. Measurement
toward the machine (away from you) is positive on the workpiece.
Z Axis: positive Z-axis motion is defined as moving the head up. Measurement up is
also positive on the workpiece.
ProtoTRAK PMX CNC conventions in terms of tool movement.
The Z RAPID dimension is the position at which Z will stop rapid traversing and switch
to its programmed Z feedrate. Z motion will continue until Z End depth has been
reached.
5.2 Part Geometry and Tool Path Programming
The ProtoTRAK PMX CNC gives you ultimate flexibility in programming. Programs
that are entered through the ProtoTRAK PMX CNC system can be entered as either Part
Geometry or Tool Path.
Part Geometry programming is the popular programming style of the ProtoTRAK family
of products. This is done by defining the final geometry of the part, and the ProtoTRAK
PMX CNC has the job of figuring out the tool path from the part dimensions and the tool
set-up information. This is a great benefit compared to regular CNC because it doesn't
force the programmer to do the difficult job of defining tool path. A consequence of part
geometry programming is that the following are not allowed:
Page 40
35
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Connection of an incline plane and another event
Connection of two events that lie in different planes
Using Geometry Programming, it is impossible for the ProtoTRAK PMX CNC to
calculate a tool path for these cases without creating a problem: in cutting the geometry
desired in the first event, the tool ends up out of position for the next event. Resolving the
difference in tool position where the first event ends and the next event begins means
either the CNC calculates and makes an unprogrammed move, or it retracts the tool out
and then back into the part.
These cases are not encountered often, but when they are you have the option of using
Tool Path programming. In Tool Path programming you define the events the same way,
but all inputs are treated as tool center. It is your job to calculate and program the tool
path.
Programs generated by CAD/CAM systems are always generated as Tool Path programs.
5.3 Planes and Vertical Planes
A plane is any flat surface. If that surface lies flat on the table, it is the XY plane. That
is, if you move your finger along that surface or plane, you are moving in the X and/or Y
direction, but not in Z (or at least not until you pick your finger up). If you tilted that
surface (think of it as a piece of paper) straight up so that it faces the front of the
machine, it would be in the XZ plane. If you tilted it up so that it faced left or right, it
would be in the YZ plane.
A vertical plane is any plane (or surface) tipped up on its edge on the table (see below).
Unlike most CNC controls, the ProtoTRAK PMX CNC can machine arcs in any vertical
plane rather than just XZ or YZ.
Vertical planes.
Page 41
36
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
5.4 Absolute and Incremental Reference
The ProtoTRAK PMX CNC may be programmed and operated in either (or in a
combination) of absolute or incremental dimensions. An absolute reference from which
all absolute dimensions are measured (in DRO and program operation) can be set at any
point on or even off the workpiece.
To help understand the difference between absolute and incremental position, consider
the following example:
Each point has both an absolute and an incremental reference in the X-axis. The
ProtoTRAK PMX CNC allows you to program using either.
5.5 Referenced and Non-Referenced Data
Data is always loaded into the ProtoTRAK PMX CNC by using the INC SET or ABS
SET key. X, Y, Z positions are referenced data. In entering any X, Y, or Z position data,
you must note whether it is an incremental or absolute dimension and enter it
accordingly. All other information (non-referenced data), such as tool diameter, feedrate,
etc. is not a position and may, therefore, be loaded with either the INC SET or ABS SET
key. This manual uses the term SET when either INC SET or ABS SET may be used
interchangeably.
5.6 Incremental Reference Position in Programming
When X, Y, Z RAPID and Z data for the beginning position of any event are input as
incremental data, this increment must be measured from some known point in the
previous event. Following are the positions for each event type from which the
incremental moves are made in the subsequent event:
Position: X, Y and Z programmed
Drill: X, Y, Z RAPID, and Z END programmed
Bolt Hole: X CENTER, Y CENTER, Z RAPID and Z END programmed
Mill: X END, Y END, Z RAPID and Z END programmed
Arc: X END, Y END, Z RAPID and Z END programmed
Circle (POCKET or FRAME): X CENTER, Y CENTER, Z RAPID and Z END
programmed
Page 42
37
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Rectangle or Irregular (POCKET or PROFILE): X1 and Y1 corner, Z RAPID and Z
END programmed
Helix: The X END, Y END, Z RAPID, and Z END programmed.
Sub: The reference position as defined for the specific events above for the event prior to
the first event that was repeated.
A.G.E. Profile: The appropriate reference position as defined for the specific events
above for the last event that is programmed.
For example, if an ARC event followed a MILL event, a 2.0 inch incremental X BEG
would mean that in the X direction the beginning of the ARC event is 2.0 inches from the
end of the MILL event.
5.7 Tool Diameter Compensation
Tool diameter compensation allows the machined edges shown directly on the print to be
programmed instead of the center of the tool. The ProtoTRAK PMX CNC then
automatically compensates for the programmed geometry so that the desired results are
obtained.
Tool cutter compensation is always specified as the tool either right or left of the
workpiece while looking in the direction of the tool motion.
Examples of tool right.
Page 43
38
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Examples of tool left.
Tool center means no compensation either right or left. That is, the centerline of the tool
will be moved to the programmed points.
Hint: to determine tool left or right, imagine that you are sitting on the tool as it is
moving.
5.8 Tool Diameter Compensation when Contouring in Z with
Part Geometry
Left and right tool diameter offsets are always those projected into the XY plane. Tool
offsets in the Z direction are always up and assume the use of a ball end mill. When
contouring in the Z-axis, this up tool offset is always activated regardless of left, right,
center if programming Part Geometry. There is no Z-axis up tool offset applied when
programming Tool Path.
Special attention must always be paid to tool offsets when machining with a ball end mill.
The reason for this is that the tool diameter changes in the bottom part (that portion equal
to the tool radius) of the tool.
The tool is always positioned at the beginning of a milling operation so that the correct
point on the ball end of the tool is tangent to the beginning point, and offset perpendicular
to the machined edge by the radius of the tool. Consider the example below of milling a
ramp in the XZ plane from point B to point C.
Page 44
39
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Ball end mill position with respect to program points. Tool starts so end mill is tangent to
BC. R from center of tool is perpendicular to BC.
Note how the tool at the beginning point (point B) starts below (in the Z direction) point
B so that it can actually touch this point. If this were not true, a cusp would remain to the
left of point B.
Now consider a similar example milling from A to B to C in the XZ plane.
In order to respect the lines defined by the programmed points, the ball end mill never
touches point B. Tool starts centered over A offset up by the tool radius R. It moves right
until it is tangent to both AB and BC. Then moves to point C as in the first example
Note the Tool at B does not drop below the AB line and, therefore, never touches point B.
As a result, a fillet is formed at point B equal to the tool radius.
This second example of continuous machining from one cut (AB) to another (BC) with
full cutter compensation between requires the two cuts to be made with events which are
connective (see Section 5.9 or 5.10 for a more complete discussion of this requirement).
5.9 Connective Events
Connective events occur between two milling events (either Mill or Arc) when the X, Y,
and Z ending points of the first event are in the same location as the X, Y, and Z starting
points of the next event. In addition, the tool offset and tool number of both events must
be the same. And both events must lie in the XY plane or the same vertical plane (see
Section 5.2).
Page 45
40
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
5.10 Conrad
Conrad is a unique feature of the PROTOTRAK PMX CNC that allows you to program a
tangentially connecting radius between connective events, or tangentially connecting
radii for the corners of pockets and frames without the necessity of complex calculations.
For the figure below, you program an Arc event from X1, Y1 to X2, Y2 with tool offset
left, and another Arc event from X2, Y2 to X3, Y3 also with tool offset left. During the
programming of the first Arc event, the system will prompt for Conrad at which time you
input the numerical value of the tangentially connecting radius r=K3. The system will
calculate the tangent points T1 and T2 and direct the tool cutter to move continuously
from X1, Y1 through T1, r=k3, T2 to X3, Y3.
Figure 1
A Conrad is added between the two intersecting lines.
Note: Conrad must always be the same as or larger than the tool radius for inside
corners. If Conrad is less than the tool radius, and an inside corner is machined, the
ProtoTRAK PMX CNC will ignore the Conrad.
For the figure below, you program an Arc event from X1, Z1 to X2, Z2, and a Mill to X3,
Z3. During the programming of the Arc event, the system will prompt for Conrad at
which time you input the numerical value of the tangentially connecting radius r=k. The
system will calculate the tangent points T1 and T2 and direct the tool cutter to move
continuously from X1, Z1 through T1, r=k, T2 and on to X3, Z3.
Page 46
41
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
A Conrad is added between an arc and a line.
5.11 Memory and Storage
Computers can hold information in two ways. Information can be in current memory or
in storage. Current memory (also known as RAM) is where the ProtoTRAK PMX CNC
holds the operating system and any part program that is ready to run. While a program is
being written, it is in current memory.
For the ProtoTRAK PMX CNC, storage of programs is on a USB thumb drive or on a
networked drive. We strongly recommend you habitually back up programs.
5.12 Current and Staged Views
Current refers to a program or operation that is being done at the present moment on the
TRAK LPM. Staged refers to a program or operation that you intend to put on the
machine in the future. The ProtoTRAK PMX allows you to toggle back and forth
between these two states so that you can use labor better. Rather than have an operator
stand and watch a (current) job running, he can use the staged view of ProtoTRAK PMX
to do almost all the set up work for future jobs.
Page 47
42
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
6.0 DRO Mode
The ProtoTRAK PMX provides a large display of the position of each axis in DRO
Mode. This enables you to see the current position of your TRAK LPM and to make
adjustments easily. With the Power Feed capability you are able to make some simple
cuts easily. This screen in DRO mode typically is not used to establish part zero for
production. Refer to section 6.2 for information on the multiple reference locations that
are available to simplify machine setups.
DRO Mode
6.1 Entering Dimensions
Inch to MM or MM to Inch: Press IN/MM and note LCD screen status line.
Reset One Axis: Press X or Y or Z, INC SET. This zeros the incremental position in the
selected axis.
Preset: Press X or Y or Z, numeric data, INC SET to preset selected axis.
Reset Absolute Reference: Press X or Y or Z, ABS SET to set selected axis absolute to
zero at the current position.
Note: This will also reset the incremental dimension if the absolute position is being
displayed when it is reset.
Preset Absolute Reference: Press X or Y or Z, numeric data, ABS SET to set the selected
axis absolute to a preset location for the current machine position.
Page 48
43
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Note: This will also reset the incremental dimension and add the value that was just input
in the ABS screen, if the absolute position is being displayed when it is preset.
Recall Absolute Position of All Axes: Press INC/ABS. Note the dimension for each axis
is labeled INC or ABS. Press INC/ABS again to revert to the original reading.
Recall Absolute Position of One Axis: Press X or Y or Z, INC/ABS. Note the INC or
ABS label for each axis. Repeat to get selected axis back to original reading.
6.2 Reference Locations
The DRO Mode gives you the ability to manage your parts relative to several references.
This integrates the workholding system with the ProtoTRAK PMX operation in a secure
way that you can verify. That will give you the confidence to move swiftly through setups.
REF – Press this softkey to choose between the following reference locations:
ABS – the current absolute 0 reference. This displays the distance the machine is from
Part Zero.
BALL A – This displays the distance the machine is from the center of Ball Lock A and
the top of the table.
BALL B –This displays the distance the machine is from the center of Ball Lock B and
the top of the table.
Page 49
44
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
BALL C –This displays the distance the machine is from the center of Ball Lock C and
the top of the table.
HOME – This displays the distance the machine is from Machine Home and the top of
the table.
PART ABS – after pressing this softkey you will be prompted to type in the part number.
Type 0 for none, and parts 1 – 4 of the Master Program. If you do not have multiple parts
in a Master Program, your part is Part 1. The numbers you see will be referenced from
the absolute 0 of the part you choose. (If none is selected, there is no part Absolute 0
being referenced.) Your part’s absolute zero is determined by your fixture offset. See
section
6.3 Power Feed
The servo motors can be used as a power feed for the X, Y, and Z axis individually, or all
three simultaneously.
a. Press the POWER FEED soft key.
b. A message box will appear that shows the power feed dimensions. All power feed
moves are entered as incremental moves from the current position to the next position.
c. Enter a position by pressing the axis key, the distance to go and the +/- key (if
needed). Input the entry by pressing INC SET. For example, if you wanted to make a
power feed move of 2.00" of the table in the negative direction, you would enter: X, 2,
+/-, INC SET.
d. Initiate the power feed move by pressing GO.
e. The feedrate is automatically set to 10 ipm (or 254 mm per min). Press FEEDRATE
OVERRIDE button to adjust the feedrate from 0 % to 150 % of the 10 inch per minute
feedrate.
Note: In RUN mode feed override adjusts from 0% to 150% of the programmed feedrate.
f. Press STOP to halt power feed. Press GO to resume.
g. Repeat the process beginning at "c" above as often as you wish.
h. Press RETURN soft key to return to manual DRO operation.
6.4 GO TO
When you press the GO TO Softkey, you will get the following choices:
BALL A – will position the center of the spindle over Ball Lock position A. The Z axis
will move to the Tool Change height.
BALL B – will position the center of the spindle over Ball Lock position B. The Z axis
will move to the Tool Change height.
BALL C– will position the center of the spindle over Ball Lock position C. The Z axis
will move to the Tool Change height.
HOME – will position the center of the spindle over the machine Home location and the
Z axis all the way up.
POSITION – allows you to set a dimension in reference to your current X, Y or Z
Absolute position at which you want the machine to stop moving when you are moving
an axis with the Electronic Handwheel.
Page 50
45
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
6.5 Return to Absolute Zero
At any time during manual DRO operation you may automatically move the table to your
absolute zero location in X and Y by pressing the RETURN ABS 0 soft key. When you
do, the message window will read "Ready to Begin: Press Go when Ready”. Make sure
your tool is clear and press the GO key. The machine will move in rapid the Z axis to
tool change position and then move the table to your X and Y absolute zero position.
You will be at zero and in manual DRO operation. See Section 6.2, Reference Locations.
6.6 Spindle Operation
To set spindle speed press the SPIN SPEED softkey. The Data Input Line will prompt
“Spindle RPM”. Enter the RPM value (150-8000) and press SET. If the spindle was
already on when you began to enter the new speed, it will stay at the current speed until
you press the SET key.
You may override the spindle speeds with the SPINDLE OVERRIDE button above the
handwheel. Press the SPINDLE OVERRIDE button. Use the Handwheel to change the
spindle speed in 2% increments per pulse. Press the SPINDLE OVERRIDE button again
to turn off the override feature.
6.7 Axis Motion In The DRO Mode
Whenever using the GO TO and ABS 0 function, keep the following in mind:
When you press a location for positioning the machine, the message window will read:
"Ready to Begin: Press Go when Ready”
a. Make sure your tool is clear of any fixturing or workpiece.
b. The door must be closed before the machine will move.
c. The Z axis will retract to the tool change position before moving in X and Y.
Page 51
46
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
7.0 Program Mode Part 1: Getting Started & General
Information
7.1 Programming Overview
The ProtoTRAK PMX CNC makes programming easy by allowing you to program the
actual part geometry as defined by the print.
The basic strategy is to first fill in the initial program information in the Program Header
screen and then program the features of the part by selecting the soft key event types
(geometry) and then follow all instructions in the Data Input Line.
When an event is selected, all the prompts that need to be input will be shown on the
right side of the screen. The first prompt will be highlighted and also shown in the Data
Input Line. Input the dimension or data requested and press INC SET or ABS SET. For
X or Y dimension data it is very important to properly select INC SET or ABS SET. For
all other data either SET will do.
As data is being entered it will show in the Data Input Line. When SET, the data will be
transferred to the list of prompts in the right side of the screen, and the next prompt will
be shown in the Data Input Line.
When all data for an event has been entered, the entire event will be shifted to the left
side of the screen and the conversation line will ask you to select the next event.
7.2 Enter Program Mode
Press MODE, select PROGRAM soft key.
The ProtoTRAK PMX CNC will allow one program in the Current view and one
program in the Staged View. If there is already a program in the Current or Staged View,
entering the Program mode will allow you to edit or add to that program.
Page 52
47
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
The Program Mode Header Screen
7.3 Program Header Screen
The first screen you see when you enter the Program Mode is the Program Header
Screen. The Program Header Screen gives you options that apply to the entire program.
The softkey selections allow you to enter the program at any point.
The program name and general programming options you choose in the Program Header
Screen will be in the program as "Event 0".
7.3.1 Program Name
Programs written on the ProtoTRAK PMX CNC are usually named for the part that is to
be machined. When programs (or files) are named using the ProtoTRAK PMX CNC, the
name can be up to 25 characters long. Programs imported into the ProtoTRAK PMX
CNC may be longer. While 25 characters are allowed, the entire program name may not
be shown in the status line or the program header screen.
Program names can include numbers, letters, spaces and other characters.
Hint: do not use a period or / in program names. This will confuse the computer because
it uses these characters to store and classify programs.
Page 53
48
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
When the Program name prompt is highlighted, the Data Input Line will show "Program
Name:"
At this point you may:
Press number keys.
Press Help to access alpha keys and special characters in the ProtoTRAK PMX CNC.
Use a keyboard plugged into the ProtoTRAK PMX CNC to name the program.
Pressing the Help hard key when the Program Name is highlighted calls up alpha keys.
Program name input without a keyboard.
To use the alpha keys and special characters on the ProtoTRAK PMX CNC:
Use the CLEAR softkey to erase the entire line; the BACKSPACE softkey to erase
the last character or number.
Use the arrow softkeys to move around the table.
Once the character you want is highlighted, use the ENTER softkey to load the
character into the program name.
Use the blank space on the lower right of the table to insert a space into the program
name.
Once you finish entering the letters and special characters, press the END softkey.
This tells the ProtoTRAK PMX CNC that you are finished with the alpha table.
Numbers may still be added to the program name.
Page 54
49
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
When you are finished with the program name, press SET to enter it into the current
memory.
Note: It is not necessary to enter a part number. If none is entered and a GO TO soft key
is pushed, the system will assume a part number 0.
7.3.2 General Program Options
Use the cursor keys to select general programming options.
Scale: Allows a scale factor between .1 and 10. An input of 5 means the part will be 5
times as big as the programmed dimensions. A value of 1.0000 is assumed if nothing is
input.
Dwell Request: Allows you to input a dwell at the bottom of a drill bolt hole or bore
cycle for events you select. Select the appropriate YES or NO soft key. If you select
YES you will be prompted to input a dwell time in seconds from .1 to 99.9 when
appropriate to the event being programmed.
Event Comments: If you select "Yes" for event comments, you will have the opportunity
to insert a comment in each event. For Irregular Pocket and Irregular Profile events, you
will be able to enter a comment at the header event, but not for each A.G.E. Mill and
A.G.E. Arc event.
Comments appear in the Run Mode on the Data Input Line as the event begins to run.
Comments may be composed of letters, numbers and some symbols and may be up to 20
characters.
While programming the event with the Event Comments set to Yes, when the highlight is
on the Event Comments prompt, you may enter a comment using the same methods used
to enter a program name, as described above.
Dimension Definition: The ProtoTRAK PMX CNC gives you a choice in programming
either tool path or geometry. Part Geometry programming allows you to define the
geometry you want your part to have and then the CNC does the difficult job of
calculating tool path for you automatically. This is a great benefit for most parts most of
the time because it means that the CNC is doing the hard work of determining tool
position.
One restriction to part geometry programming is that for events to be connective, they
must lay on the same plane (see Section 5.3 for a definition of planes). For this reason,
the ProtoTRAK PMX CNC gives you the option of entering your own tool path. If you
wish to program the part by defining tool path yourself, you may choose the TOOL
PATH softkey. Otherwise, Part Geometry programming is assumed. Tool Path operates
under the same rules as standard RS274.
A program must be entirely written in Part Geometry or Tool Path programming, you
cannot combine the two methods in one program.
Page 55
50
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
7.3.3 Program Header Softkeys
The following softkeys are encountered in the Program Header Screen. The first five
listed below are always there. The last four appear when relevant to the general
programming option.
GO TO BEGIN: puts the Program Header on the left side of the screen and the Event #1
on the right side.
GO TO END: puts the last programmed event on the left side of the screen and the next
event to be programmed on the right side.
GO TO #: enter the event number you wish to go to and then press SET. Puts the
requested event number on the right side of the screen and the previous event number on
the left.
Note: for a new program that has no Events, all the GO TO selections will take you to the
beginning, with the program header information summarized on the left (as Event 0) and
the Select an Event options for Event 1 on the right.
YES and NO: YES and NO appear when the Dwell Request and the Event Comments are
highlighted. Choosing YES will give you prompts for using these options while you are
programming. You may return to the Program Header Screen at any time to choose or
cancel these prompts.
NEXT PART: appears when a Master Program is in memory. Pressing this allows you to
switch between the programs within the Master Program.
PART GEO: sets up the programming as Part Geometry.
TOOL PATH: sets up the programming as Tool Path.
7.4 Assumed Inputs
The ProtoTRAK PMX CNC will automatically program the following when you simply
press SET (either INC SET or ABS SET):
Tool Offset: On the first event with an offset, it will become CENTER. If it is not the
first event then it will enter the offset, which is the same as the last event if that event was
a Mill or Arc event
Feedrate: same as last event if that event was a Mill, Arc, Pocket, Frame, or Helix
Tool #: same as last event, or Tool #1 if the first event
DRILL OR BORE: Drill
# PECKS FOR DRILL: 1 peck
CONRAD: 0
You may change these assumed inputs by simply inputting the desired data when the
event is programmed.
7.5 Z Rapid Positioning
Between any two events the head will always move to the higher of the Z rapid of the
event just completed or the Z Rapid of the next event, unless the two events are
connective (see Section 5.9). Remember, when using part geometry programming, two
milling events are not connective unless they lie in the same plane.
Page 56
51
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
7.6 Softkeys within Events
Once a geometry (Event) such as MILL or BOLT HOLE is selected, the softkeys will
change.
Soft keys used while programming an event.
DATA BOTTOM: puts the Highlight on the last input.
INSERT EVENT: use this to insert a new event into the program. This new event will
take the place of the one that was on the right side of the screen when you pressed the
INSERT EVENT key. That previous event, and all the events that follow, increase their
event number by one. For example, if you started with a program of four events, if you
were to press the INSERT EVENT key while Event 3 was on the right side of the screen,
the previous Event 3 would become Event 4 and the previous Event 4 would become
Event 5. If you insert a Subroutine event, the event numbers will increase by one as
when you insert another kind of event. If you insert a copy event, the event numbers will
increase by the number of events that are copied.
DELETE EVENT: this will delete the event on the right side of the screen.
7.7 Programming Events
Once you press the appropriate GO TO soft key, you will begin to define your part as a
series of Events. For the ProtoTRAK PMX CNC, an Event is a geometry, or a feature of
a part.
Program Begin.
Page 57
52
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
In the figure above, the header screen has been completed and is on the left side. Select
an event type from the soft keys
When the MORE softkey is selected, the soft keys change to:
More events.
After an event type is selected from the softkeys, the prompts for that event will appear
on the right side of the screen. The data you need to enter to program the event will
appear in the Data Input Line. As soon as you enter one piece of data by pressing the
INC SET or ABS SET key, the next prompt will appear in the Data Input Line.
7.8 Editing Data While Programming
While programming an event, all data is entered by pressing the appropriate numeric keys
and pressing INC SET or ABS SET. If you enter an incorrect number before you press
INC SET or ABS SET you may clear the number by pressing RSTR (Restore). Then,
input the correct number and press SET.
If incorrect data has been entered and SET, you may correct it you may correct it easily
by pressing an arrow key until the incorrect prompt and data are highlighted and shown
in the conversation line. Enter the correct number and SET. The ProtoTRAK PMX CNC
will not allow you to skip past prompts (by pressing DATA FWD) which need to be
entered to complete an event except when using the A.G.E. in the Irregular Pocket or
Irregular Profile event.
Previous events may be edited by pressing the BACK hard key to the left of the soft keys.
The previous event will be shifted from the left side of the screen to the right and may be
edited. The BACK key may be pressed all the way to the Program Header Screen.
7.9 LOOK
As you program each event, it is helpful to see your part drawn. For quick graphics while
in the Program Mode, press the LOOK hard key.
This function is active at the end of each event, or whenever the conversation line is
prompting Select Event. Press the LOOK key and the ProtoTRAK PMX CNC will draw
the part. Press LOOK again, or BACK to bring back the Select Event screen. You may
also select a new view or adjust the view.
Softkeys in LOOK:
ADJUST VIEW: gives additional options for adjusting the view of the drawing. See
below.
FIT DRAW: automatically resizes the drawing to fit the entire part program on the
screen.
Page 58
53
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
LIST STEP: displays the list of events on the left side of the screen and with a purple
highlight on the first event. As LIST STEP is pushed, the highlight shifts to the next
event. As this happens, that event is also highlighted in the graphics by having its color
change to purple.
START EVENT NUMBER: will prompt you to enter an event number for highlighting.
This is useful for moving quickly to a particular event in a large program.
XY: displays a view in the XY plane.
YZ: displays a view in the YZ plane.
XZ: displays a view in the XZ plane.
3D: displays an isometric view
Softkeys in Adjust view:
FIT DRAW: automatically resizes the drawing to fit the entire part program on the
screen.
ZOOM IN: makes the drawing larger.
ZOOM OUT: makes the drawing smaller.
RETURN: returns you to the first LOOK screen. The adjustments you made will stay on
the screen until you press another selection that overrides those adjustments. The LIST
STEP function may be used with the adjustment unaltered.
Use the arrow keys to shift the position of the drawing on the screen.
Note: The LOOK routine does not check for programming errors. Use Tool Path in the
Set Up Mode to check movement of the tool.
Page 59
54
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
8.0 Program Mode Part 2: Program Events
Events are fully defined pieces of geometry. By programming events, you tell the
ProtoTRAK PMX CNC what geometry you want to end up with; it figures the tool path
for you from your answers to the prompts and the tool information you give it in the SetUp Mode.
8.1 POSN: Position Events
This event type positions the table and spindle at a specified position. The positioning is
always at rapid speed (modified by feedrate override) and in the most direct path possible
from the previous location. The most common use of the position event is to move the
tool around an obstacle such as a clamp. For this reason, Z and X - Y motion will not
occur simultaneously. First, the Z (head) will move to the higher of the Z rapid position
of the current and next event, then the X (table) and Y (saddle) will move to the
programmed position.
To program a Position event press the POSN soft key.
Prompts for the Position event:
X END is the X dimension to the position
Y END is the Y dimension to the position
Z Rapid is the Z dimension to the position
RPM is the spindle RPM for the event. INC SET will use the RPM of the previous event.
Tool # is the tool number you assign. SET will use the tool number of the previous
event.
Note: the blue ? is active during the Tool # prompt. Pressing the HELP hard key will
take you to a screen where you may view, edit or enter tool diameter and tool type.
NOTE - On all RPM line prompts for all events except tap, a blue “?” will be visible,
which when pressed will allow the user to run the spindle in reverse. A “REV” prompt
will show up in the event to the right of the RPM programmed.
8.2 DRILL Events
This event positions the table to the specified X and Y position, moves the spindle at
rapid to the Z RAPID location, feeds the tool to the Z END location, and rapids back to Z
RAPID for drill, and feeds back for bore.
Press the DRILL soft key.
Prompts for the drill event:
Drill=1, Bore=2: selects whether the hole is to be drilled or bored.
X: is the X dimension to the hole
Y: is the Y dimension to the hole
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the bottom of the hole
# Pecks for Drill: the factory setting is for each peck to be successively smaller, taking
the largest cuts at the beginning and the smallest at the end. When the highlight is on this
prompt, you may change this setting by pressing the HELP key. This will take you to a
Page 60
55
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
screen where you may choose to have a fixed amount of material taken per peck or have
Warning!
The boring tool you are using must be placed in the spindle
consistently when using this feature. If you place the boring tool
in the spindle 180º from how you set the tool up the first time, the
cutting tool will crash into your workpiece.
the cutter move up just enough to break the chip before continuing to feed down.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
Z Feedrate: is the drilling feedrate
Tool #: is the tool number you assign
If a bore is selected and entered, you can change the tool path of the bore from the default
tool path of feeding in and feeding out at the programmed rpm. After selecting Bore, use
the cursor key to move over the prompt again. The blue ? will appear. Press HELP to be
able to change the tool path to feed down, position away from the cut and then rapid out
of the hole. The following prompts will appear:
Angle: is the angle from 3 o’clock CCW to the location of the cutting insert
Retract Dist: is the distance the cutting tool will retract towards the center of the bored
hole.
8.3 BOLT HOLE Events
This event allows you to program a bolt hole pattern without needing to compute and
program the position of each hole.
Prompts for the Bolt Hole event:
Drill=1, Bore=2, Tap = 3: selects whether the hole is to be drilled or bored
Once the bore is selected and entered, you can change the tool path of the bore from the
default tool path of feeding in and feeding out at the programmed rpm. After selecting
Bore, use the cursor key to move over the prompt again. The blue ? will appear. Press
HELP to be able to change the tool path to feed down, position away from the cut and
then rapid out of the hole.
# Holes: is the number of holes in the bolt hole pattern
X Center: is the X dimension to the center of the hole pattern
Y Center: is the Y dimension to the center of the hole pattern
Z Rapid: is the Z dimension to transition from rapid to feed
Z Begin: appears for tapping only, this is the top of the work piece
Z End: is the bottom of the hole
Radius: is the radius of the hole pattern from the center to the center of the holes
Angle: is the angle from the positive X axes (that is, 3 o'clock) to any hole; positive
angle is measured counterclockwise from 0.000 to 359.999 degrees, negative angles
measured clockwise.
Pitch: is the pitch of the tap that is used if the Tap option is chosen.
Page 61
56
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
# of Variable Pecks: the factory setting is for each peck to be successively smaller,
taking the largest cuts at the beginning and the smallest at the end. When the highlight is
on this prompt, you may change this setting by pressing the HELP key. This will take
you to a screen where you may choose to have a fixed amount of material taken per peck
or have the cutter move up just enough to break the chip before continuing to feed down.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
Z Feedrate: is the drilling feedrate
Tool #: is the tool number you assign
8.4 MILL Events
This event allows you to mill in a straight line from any one XYZ point to another,
including at a diagonal in space. It may be programmed with a CONRAD if it is
connective with the next event (this next event must lie in the same plane as the Mill
event).
Prompts for the Mill Event:
X Begin: is the X dimension to the beginning of the mill cut
Y Begin: is the Y dimension to the beginning of the mill cut
Z Rapid: is the Z dimension to transition from rapid to feed
Z Begin: is the Z dimension to the beginning of the mill cut
X End: is the X dimension to the end of the mill cut; incremental is from X Begin
Y End: is the Y dimension to the end of the mill cut; incremental is from Y Begin
Z End: is the Z dimension to the end of the mill cut; incremental is from Z Begin.
Conrad: is the dimension of a tangential radius to the next event (that must lie in the
same plane for part geometry programming)
Tool Offset: is the selection of the tool offset to right (input 1), offset to left (input 2), or
tool center--no offset (input 0) relative to the programmed edge and direction of tool
cutter movement and as projected in the XY plane.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
Z Feedrate: is the Z feedrate from Z Rapid to Z end in in/min from .1 to 700, or mm/min
from 5 to 17780
XYZ Feedrate: is the milling feedrate from Begin to End in in/min from .1 to 800, or
mm/min from 5 to 20320
Tool #: is the tool number you assign
Note: to program a series of connected lines and arcs on the same plane, use the Pocket or
Profile events.
8.5 ARC Events
This event allows you to mill with circular contouring any arc (fraction of a circle) that
lies in the XY plane or a vertical plane (see Section 5.3). Vertical plane arcs are also
limited to those that are entirely concave or convex (in other words, if you think of the
arc lying on the surface of the earth, then it can't cross the equator, again limited to
quadrants surface of the earth , going from the equator to the South Pole).
Page 62
57
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
In ARC events when X Center, Y Center, and Z Center are programmed incrementally,
they are referenced from X End, Y End, and Z End respectively. An ARC event may be
programmed with a CONRAD if it is connective with the next event (this next event must
lie in the same plane as the Arc event).
Note: When an arc is 180 degrees, there are several paths that all have the same
beginning, ending, and center locations. To illustrate, Imagine that if you were on the
earth's equator and you wanted to get to the other side of the earth you could go
clockwise or counterclockwise around the equator, or you could go up over the north
pole, or down under the south pole. The ProtoTRAK PMX CNC will automatically
assume that all 180 degree arcs that have the same beginning, ending and center
dimensions for Z, lie in the XY plane. If you want a 180 degree arc in a vertical plane,
you must program two 90 degree arcs or some equivalent.
Prompts for the Arc Event:
X Begin: is the X dimension to the beginning of the arc cut
Y Begin: is the Y dimension to the beginning of the arc cut
Z Rapid: is the Z dimension to transition from rapid to feed
Z Begin: is the Z dimension to the beginning of the arc cut.
X End: is the X dimension to the end of the arc cut; incremental is from X Begin
Y End: is the Y dimension to the end of the arc cut; incremental is from Y Begin
Z End: is the Z dimension to the end of the arc cut; incremental is from Z Begin.
X Center: is the X dimension to the center of the arc; incremental is from X End
Y Center: is the Y dimension to the center of the arc; incremental is from Y End
Z Center: is the Z dimension to the center of the arc; incremental is from Z End.
Conrad: is the dimension of a tangential radius to the next event (which must lie in the
same plane)
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction of the arc as
viewed looking down for an arc in the XY plane, looking from the front for a vertical
plane, or looking from the right for a vertical YZ plane
Tool Offset: is the selection of the tool offset to right (input 1), offset to left (input 2), or
tool center--no offset (input 0) relative to the programmed edge and direction of tool
cutter movement and as projected in the XY plane
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
Z Feedrate: is the Z feedrate from Z Rapid to Z end in in/min from .1 to 700, or mm/min
from 5 to 17780
XYZ Feedrate: is the milling feedrate from Begin to End in in/min from .1 to 800, or
mm/min from 5 to 20320
Tool #: is the tool number you assign
Note: to program a series of connected lines and arcs on the same plane, use the Pocket or
Profile events.
Page 63
58
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
8.6 POCKET Events
This event selection gives you a choice between, circle pocket, rectangular pocket and
irregular pocket within the XY plane.
Pockets include machining the circumference, as well as all the material inside the
circumference of the programmed shape. If a finished cut is programmed, it will be made
at the completion of the final pass. The cutter will arc in and arc out of the finish cut and
position itself the finish cut dimension away from the part before moving the tool out of
the part.
The factory setting for tool step over while machining a pocket is 70%. This may be
changed. When you first enter the pocket event, the blue ? will appear next to the help
key. Pressing Help will give you the choice of entering a new tool step over percentage.
The value you enter here will remain the same until you change it again.
8.6.1 Circular Pocket
Press the CIRCLE PCKT soft key if you wish to mill a circular pocket.
Prompts for the Circle Pocket:
X Center: is the X dimension to the center of the circle
Y Center: is the Y dimension to the center of the circle
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension at the bottom of the pocket; incremental is from the previous
event
Radius: is the finish radius of the circle
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling
# Passes: number of cycles to machine to the final depth spaced equally from Z Rapid to
Z End (hint: keep Z Rapid small)
Entry mode: choose between a zigzag ramp and a plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See Section 8.6.5 for more information about the zigzag ramp.
Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut. See
Section 8.6.7 for a bottom finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
FIN RPM: is the spindle RPM for the finish cut.
Z Feedrate: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or mm/min
from 5 to 17780
XYZ Feedrate: is the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320
Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign
8.6.2 Rectangular Pocket
Press RECTANGLE soft key if you wish to mill a rectangular pocket (all corners are 90o
right angles and the sides are parallel to the X and Y axes).
Page 64
59
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
The prompts for the rectangular pocket:
X1: is the X dimension to any corner
Y1: is the Y dimension to the same corner as X1
X3: is the X dimension to the corner opposite X1; incremental is from X1
Y3: is the Y dimension to the same corner as X3; incremental is from Y1
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension at the bottom of the pocket; incremental is from the previous
event
Conrad: is the value of the tangential radius in each corner
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling
# Passes: is the number of cycles to machine to the final depth spaced equally from Z
Rapid to Z End.
Entry mode: choose between a zigzag ramp and a plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See Section 8.6.5 for more information about the zigzag ramp.
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut. See
Section 8.6.7 for a bottom finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
FIN RPM: is the spindle RPM for the finish cut.
Z Feedrate: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or mm/min
from 5 to 17780
XYZ Feedrate: is the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320
Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign
8.6.3 Irregular Pocket
Press the IRREG PCKT soft key if you wish to mill a pocket other than a rectangle or
circle. The Irregular Pocket event gives you the powerful Auto Geometry Engine to
define a shape made up of straight lines (Mills) and arcs.
The first screen in an Irregular Pocket event will define the beginning point and some of
its general parameters. The last event of the irregular pocket must end at the same point
as defined in the first event.
X Begin: is the X dimension of the beginning of the pocket
Y Begin: is the Y dimension of the beginning of the pocket
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension of the depth of the pocket.
# Passes: is the number of cycles to machine to the final depth spaced equally from Z
rapid to Z end (hint: keep Z Rapid small)
Entry Mode: choose between a zigzag ramp and a plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See Section 8.6.5 for more information about the zigzag ramp.
Page 65
60
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut. See
Section 8.6.7 for a bottom finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
FIN RPM: is the spindle RPM for the finish cut. Z Feedrate: is the Z feedrate from Z
rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320
Fin Feedrate: is the finish cut milling feedrate in in/min from .1 to 800, or mm/min from
5 to 20320
Tool #: is the tool number you assign
When the initial screen is complete, you will define the perimeter of the pocket with a
series of A.G.E. Mills and A.G.E. Arcs. Programming with the Auto Geometry Engine is
explained in Section 9.0.
No islands may exist in an irregular pocket.
8.6.4 Tool Path in Pocket Events
In Program Run, the pocket path will be either the plunge or zigzag cuts to Z depth along
either the X or Y, followed by the required number of cuts to clear out the interior
material, and then the rough cut along the inside of the perimeter. This will be repeated
for each pass and then followed by a finish pass (if FIN CUT was not zero) along the
inside of the perimeter at the Finish Feedrate and final depth. If a bottom finish cut was
programmed, it will be machined before the perimeter finish cut.
Whether the cuts to clear the interior material of the irregular pocket are along the X or
Y-axis depends on if there are hidden areas of the pocket. The ProtoTRAK PMX CNC
always looks to cut along the X-axis first. If there are areas that are hidden to the X-axis,
it will machine along the Y-axis. If there are hidden areas that cannot be machined
continuously in the X or Y-axis, the tool will return to Z retract and then reposition to
machine the hidden area.
8.6.5 Zigzag Z Depth Cuts
In programming pocket events, you have a choice to program the cuts to Z depth either as
a plunge or a zigzag ramp. For rectangular and circular pockets, the tool will start in the
center of the pocket. For irregular pockets, since there is no center defined, the tool will
start in the lower left corner of the pocket. The direction of the ramp will be the same as
the initial direction in either X or Y, depending on how the pocket is to be cut.
The tool will zigzag back and forth along the X or Y over a length of one tool radius
while at the same time moving in the Z direction. When it travels one tool radius along
this direction, it will have traveled a distance of ten percent of the tool diameter along the
Z. This works out to roughly ramping into the part at an angle of 11 degrees.
Page 66
61
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
In order to use a zigzag ramp, the X or Y move must be larger than the diameter of the
tool plus the radius of the tool, minus the finish cut of the pocket. The formula is:
the pocket x or y move > tool diameter + tool radius - fin cut
If the tool is too large for the zigzag ramp, the ProtoTRAK PMX CNC will give an error
message during program run and will then default to plunge. This will occur for each
pass of the pocket depth.
8.6.6 Conrad in Pocket Events
A Conrad may be added to the last event of an Irregular Pocket. The Conrad will be
inserted between the end of the last event and the beginning of the next event.
8.6.7 Bottom Finish Cut
The standard finish cut is along the walls of the part, but you may have the ProtoTRAK
machine a finish cut along the bottom as well. When the highlight is on the Fin Cut
prompt, the blue ? appears next to the Help key. Pressing help gives you the ability to
choose a Finish cut in Z. You can remove the bottom finish cut by placing the highlight
on the Fin Cut prompt and pressing Help again. When you select Yes to the bottom
finish cut, the following prompt will appear:
Z FIN CUT: the finish cut at the bottom.
8.6.8 Face Mill Event
Press Face Mill soft key if you wish to face or clean up the top of a workpiece.
The cutter will automatically start off of the part that you define. The cutter will move
along the X axis to remove the material starting from where you defined X1, Y1 and
finishing at the corner programmed as X3, Y3.
The prompts for the face mill:
X1: is the X dimension to any corner
Y1: is the Y dimension to the same corner as X1
X3: is the X dimension to the corner opposite X1; incremental is from X1
Y3: is the Y dimension to the same corner as X3; incremental is from Y1
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension at the bottom of the pocket; incremental is from the previous
event
# Passes: is the number of cycles to machine to the final depth spaced equally from Z
Rapid to Z End.
Z Fin Cut: is the depth of the finish cut. If 0 is input there will be no finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
FIN RPM: is the spindle RPM for the finish cut.
Z Feedrate: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or mm/min
from 5 to 17780
Page 67
62
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
XYZ Feedrate: is the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320
Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign
Note – if you press the HELP key when you are on the X1 prompt, you can adjust the
step over distance of the face mill. The default is 95% of the cutter width. You can
adjust it from 1 to 99%.
8.7 ISLAND Events
Within the Pocket event choices, you may also select a circular, rectangular or irregular
island. An Island is a shape that is left standing when the surrounding material is
removed. The ProtoTRAK gives you the ability to machine almost any shape as an
island within a rectangular pocket. Both the shape of the island and the dimension of the
surrounding pocket are defined within the Island Event.
The tool path for machining the Island Event is that the tool will first plunge or ramp into
the material next to the island, offset by the programmed finish cut, to the depth of the
first pass. The tool will machine the perimeter of the island, offset by the island finish
cut. Then the tool will machine the material in the pocket in a spiral path, moving away
from the island in the programmed clockwise or counterclockwise direction. It will
continue this outward spiral motion until it encounters the programmed rectangular
perimeter (or pocket). It will then follow the perimeter, offset by the pocket finish cut.
It will proceed in this manner through the number of programmed passes. On the final
pass, it will machine the island finish cut, then the pocket finish cut. If a Z finish cut is
programmed, it will do this in the same spiral pattern as the roughing passes between
machining the island and pocket finish cuts. The tool will ramp away from the finish cut
by the amount of the finish cut before it raises out of the part.
8.7.1 Circular Island
Press the CIRCLE ISLAND soft key if you wish to mill a circular island.
Prompts for the Circle Pocket:
X CENTER: is the dimension of the center of the Island
Y CENTER: is the dimension of the center of the Island
Z RAPID: is the Z dimension of the transition from rapid to feed
Z END: is the Z dimension at the bottom of the pocket; incremental is from the previous
event
RADIUS: is the finish radius of the Island
DIRECTION: is the milling direction, clockwise or counterclockwise
#PASSES: the number of roughing passes to the depth
ENTRY MODE: choose between zigzag ramp and plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See the previous section for more information about the zigzag ramp.
Page 68
63
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
FIN CUT ISL: Finish cut for the Island. If 0 is input, there will be no finish cut. See the
previous section for a bottom finish cut.
X1 POCKET: X dimension for one corner of the rectangular pocket that surrounds the
island.
Y1 POCKET: Y dimension for one corner of the rectangular pocket that surrounds the
island.
X3 POCKET: X dimension for the opposite corner of the rectangular pocket that
surrounds the island.
Y3 POCKET: Y dimension for the opposite corner of the rectangular pocket that
surrounds the island.
CONRAD PCKT: the value of the tangential radius in the corners of the rectangular
pocket that surrounds the island.
FIN CUT PCKT: finish cut along the perimeter of the pocket. If 0 is input, there will be
no finish cut. See the previous section for a bottom finish cut.
RPM is the spindle RPM for the event. INC SET will use the RPM of the previous event.
FIN RPM: is the spindle RPM for the finish cut.
Z FEEDRATE: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or
mm/min from 5 to 17780.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts
TOOL #: is the tool number you assign.
8.7.2 Rectangular Island
Press the RECT ISLAND softkey if you wish to machine a rectangular island.
Prompts for the RECT ISLAND:
X1 Island: X dimension for one corner of the rectangular island.
Y1 Island: Y dimension for one corner of the rectangular island.
X3 Island: X dimension for the opposite corner of the island.
Y3 Island: Y dimension for the opposite corner of the island.
Z RAPID: is the Z dimension of the transition from rapid to feed
Z END: is the Z dimension at the bottom of the pocket; incremental is from the previous
event
CONRAD ISL: the value of the tangential radius in the corners of the island.
DIRECTION: is the milling direction, clockwise or counterclockwise
#PASSES: the number of roughing passes to the depth
ENTRY MODE: choose between zigzag ramp and plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See the previous section for more information about the zigzag ramp.
FIN CUT: Finish cut for the Island. If 0 is input, there will be no finish cut. See the
previous section for a bottom finish cut.
X1 POCKET: X dimension for one corner of the rectangular pocket that surrounds the
island.
Y1 POCKET: Y dimension for one corner of the rectangular pocket that surrounds the
island.
Page 69
64
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
X3 POCKET: X dimension for the opposite corner of the rectangular pocket that
surrounds the island.
Y3 POCKET: Y dimension for the opposite corner of the rectangular pocket that
surrounds the island.
CONRAD PCKT: the value of the tangential radius in the corners of the rectangular
pocket that surrounds the island.
FIN CUT PCKT: finish cut along the perimeter of the pocket. If 0 is input, there will be
no finish cut. See the previous section for a bottom finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
FIN RPM: is the spindle RPM for the finish cut.
Z FEEDRATE: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or
mm/min from 5 to 17780.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts
TOOL #: is the tool number you assign.
8.7.3 Irregular Island
Press the IRREG ISLAND key if you wish to mill an island other than a rectangle or
circle. The Irregular Island gives you the powerful Auto Geometry Engine to define a
shape made up of straight lines and arcs.
The first screen in an Irregular Island event will define the beginning point and some of
its general parameters. The last event of the irregular island must end at the same point
as defined in the first event.
Prompts for the Irregular Island event:
X BEGIN: X dimension to the beginning of the island.
Y BEGIN: Y dimension to the beginning of the island.
Z RAPID: is the Z dimension of the transition from rapid to feed
Z END: is the Z dimension at the bottom of the pocket; incremental is from the previous
event
#PASSES: the number of roughing passes to the depth
ENTRY MODE: choose between zigzag ramp and plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See the previous section for more information about the zigzag ramp.
FIN CUT: Finish cut for the Island. If 0 is input, there will be no finish cut. See the
previous section for a bottom finish cut.
X1 POCKET: X dimension for one corner of the rectangular pocket that surrounds the
island.
Y1 POCKET: Y dimension for one corner of the rectangular pocket that surrounds the
island.
X3 POCKET: X dimension for the opposite corner of the rectangular pocket that
surrounds the island.
Page 70
65
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Y3 POCKET: Y dimension for the opposite corner of the rectangular pocket that
surrounds the island.
CONRAD PCKT: the value of the tangential radius in the corners of the rectangular
pocket that surrounds the island.
FIN CUT PCKT: finish cut along the perimeter of the pocket. If 0 is input, there will be
no finish cut. See the previous section for a bottom finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
FIN RPM: is the spindle RPM for the finish cut.
Z FEEDRATE: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or
mm/min from 5 to 17780.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320.
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts.
TOOL #: is the tool number you assign.
When the initial screen is complete, you will define the perimeter of the island with a
series of A.G.E. Mills and A.G.E. Arcs. Programming with the Auto Geometry Engine is
explained in Section 9.0.
8.8 PROFILE Events
This event allows you to mill around the outside or inside of a circular or rectangular
frame or an irregular profile. The irregular profile may be closed or open. All profiles
are limited to the XY plane.
When the irregular profile event is started the ProtoTRAK PMX CNC will automatically
initiate the powerful Auto Geometry Engine. See Section 9.0 for programming with
A.G.E.
8.8.1 Circle Profile
Press the CIRCLE soft key if you wish to mill a circular frame.
Prompts in the Circle Profile event:
X Center: is the X dimension to the center of the circle
Y Center: is the Y dimension to the center of the circle
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension to the bottom of the frame; incremental is from the previous
event
Radius: is the finish radius of the circle
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling
Tool Offset: is the selection of the tool offset to the right (input 1), offset to the left
(input 2), or tool center--no offset (input 0) relative to the programmed edge and direction
of the cutter movement
# Passes: is the number of cycles to machine to the final depth spaced equally from Z
Rapid to Z End (hint: keep Z Rapid small)
Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut
Page 71
66
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
FIN RPM: is the spindle RPM for the finish cut.
Z Feedrate: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or mm/min
from 5 to 17780
XYZ Feedrate: is the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320
Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign
8.8.2 Rectangular Profile
Press the RECTANGLE soft key if you wish to mill a rectangular frame (all corners are
90 degree right angles).
Prompts for the rectangular profile:
X1: is the X dimension to any corner
Y1: is the Y dimension to the same corner as X1
X3: is the X dimension to the corner opposite X1; incremental is from X1
Y3: is the Y dimension to the same corner as X3; incremental is from Y1
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension at the bottom of the frame; incremental is from the previous
event
Conrad: is the value of the tangential radius in each corner
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling
Tool Offset: is the selection of the tool offset to the right (input 1), offset to the left
(input 2), or tool center--no offset (input 0) relative to the programmed edge and direction
of the cutter movement
# Passes: is the number of cycles to machine to the final depth spaced equally from Z
Rapid to Z End (hint: keep Z Rapid small)
Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
FIN RPM: is the spindle RPM for the finish cut.
Z Feedrate: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or mm/min
from 5 to 17780
XYZ Feedrate: is the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320
Fin Feedrate: is the milling feedrate for the finish cut (if programmed).
Tool #: is the tool number you assign
8.8.3 Irregular Profile
Press the IRREG PROFILE soft key if you wish to mill a profile other than a rectangle or
circle. The Irregular Profile event gives you the powerful Auto Geometry Engine to
define a shape made up of straight lines (Mills) and arcs.
Page 72
67
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
The Irregular Profile is a series of events that are programmed to machine continuously.
The first event of the series will be called an IRR PROFILE and it will define the
beginning point of the profile and other information that applies to the entire profile.
X Begin: is the X dimension of the beginning of the profile
Y Begin: is the Y dimension of the beginning of the profile
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension of the depth of the profile
Tool Offset: is the selection of the tool offset to right (input 1), offset to left (input 2), or
tool center--no offset (input 0) relative to the programmed edge and direction of tool
cutter movement
# Passes: is the number of cycles to machine to the final depth spaced equally from Z
rapid to Z end (hint: keep Z Rapid small)
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
FIN RPM: is the spindle RPM for the finish cut.
Z Feedrate: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or mm/min
from 5 to 17780
XYZ Feedrate: is the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320
Fin Feedrate: is the finish cut milling feedrate in in/min from .1 to 800, or mm/min from
5 to 20320
Tool #: is the tool number you assign
When the initial Irregular Profile screen is complete, the rest of the profile is programmed
using A.G.E. Mill and A.G.E. Arc events. Programming with the Auto Geometry Engine
is explained in Section 9.0.
8.9 HELIX Events
The HELIX Event is found after you press the MORE softkey from the Select Event
screen. It allows you to machine in a circular path in the XY plane while you
simultaneously move the Z-axis linearly.
Press the HELIX soft key.
X Center: is the X dimension to the center of rotation of the helix
Y Center: is the Y dimension to the center of rotation of the helix
Z Rapid: is the Z dimension to transition from rapid to feed
Z Begin: is the Z dimension to the beginning of the helix
Z End: is the Z dimension at the end of the helix
Radius: is the radius from the center of rotation to the helix
Angle: is the angle from the positive X axis (that is, 3 o'clock) to the starting position of
the helix
# Rev: is the number of revolutions in the helix, for example, 0.75 would be
270 degrees, or 3.25 would be three times around plus 90 degrees
Direction: is the clockwise (input 1) or counterclockwise (input 2) direction of the helix
Page 73
68
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Tool Offset: is the selection of the tool offset to right (input 1), offset to left (input 2), or
tool center--no offset (input 0) relative to the programmed edge and direction of the cutter
movement
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
Z Feedrate: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or mm/min
from 5 to 17780
XYZ Feedrate: is the feedrate from beginning to end in in/min from .1 to 800, or
mm/min from 5 to 20320
Tool #: is the tool you assign
8.10 Subroutine Events
The Subroutine Events are used for manipulating previously programmed geometry
within the XY plane.
The Subroutine Event is divided into three options: Repeat, Mirror, and Rotate.
Repeat and Rotate may be connective. As long as the rules of connectivity are satisfied
(see Section 5.9), the ProtoTRAK PMX CNC will continue milling between preceding
and subsequent events.
REPEAT allows you to repeat an event or a group of events up to 99 times with an offset
in X and/or Y and/or Z. This can be useful for drilling a series of evenly spaced holes,
duplicating some machined shapes, or even repeating an entire program with an offset for
a second fixture.
Repeat events may be "nested." That is, you can repeat a repeat event, of a repeat event,
of some programmed event(s). One new tool number may be assigned for each Repeat
Event.
MIRROR is used for parts that have symmetrical patterns or mirror image patterns. In
addition to specifying the events to be repeated, you must also indicate the axis or axes
(X or Y or XY are allowed) that the reflection is mirrored across. In addition, you must
specify the offset from absolute zero to the line of reflection. You may not mirror
another mirror event, or mirror a rotate event. Consider the figure below:
Page 74
69
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Above, holes 1-4 are mirrored across the Y axis to 5-8, respectively, about a line X
OFFSET from X=absolute 0
ROTATE is used for polar rotation of parts that have a rotational symmetry around some
point in the XY plane. In addition to specifying the events to be repeated, you must also
indicate the absolute X and Y position of the center of rotation, the angle of rotation
(measured counterclockwise as positive; and clockwise as negative), and the number of
times the specified events are to be rotated and repeated. You may not rotate another
rotate event, however you can rotate a mirror event. Consider the figure below:
Shape A programmed with 4 MILL events and Conrads. Using ROTATE, these 4 events
are rotated through a 45 degree angle about a point offset from absolute zero by X Center
and Y Center dimensions. A is rotated 3 times to produce shape B, C, and D
Page 75
70
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Press the SUBROUTINE (SUB) soft key to call up the Repeat, Mirror, and Rotate
options.
8.10.1 REPEAT
Press the REPEAT soft key.
Where:
First Event #: is the event number of the first event to be repeated
Last Event #: is the event number of the last event to be repeated; if only one event is to
be repeated, the Last Event # is the same as the First Event #
X Offset: is the incremental X offset from event to be repeated
Y Offset: is the incremental Y offset from event to be repeated
Z Offset: is the incremental Z offset from event to be repeated
Z Rapid Offset: is the incremental Z rapid offset from event to be repeated
# Repeats: is the number of times events are to be repeated up to 99
% RPM: is the percentage of RPM in the programmed events. SET will load in the
assumed % of 100%.
% Feed: the percentage of the feeds programmed in the repeated events. 100% is
assumed
Tool #: is the tool number you assign
8.10.2 MIRROR
Press the MIRROR soft key.
First Event #: is the event number of the first event to be mirrored
Last Event #: is the event number of the last event to be mirrored; if only one event is to
be mirrored, the last event is the same as the first.
Cutting Order: input 1 to cut from the lowest mirrored event to the highest (forward) and
2 to machine from the highest mirrored event to the lowest (backward).
This way you can keep all the machine motion in a consistent direction as it moves from
the original shape to the mirrored shape and keep all cutting either climb or conventional.
Mirror Axis: is the selection of the axis or axes to be mirrored (input X or Y or XY,
SET)
X Offset: is the distance from Y absolute 0 to the Y-axis line of reflection
Y Offset: is the distance from X absolute 0 to the X-axis line of reflection
8.10.3 ROTATE Z Axis
Press the ROTATE soft key.
First Event #: is the event number of the first event to be rotated
Last Event #: is the event number of the last event to be rotated; if only one event is to be
rotated, the last event is the same as the first
X Center: is the X absolute position of the center of rotation
Y Center: is the Y absolute position of the center of rotation
Angle: is the angle of rotation of the repeated events (positive is counterclockwise;
negative is clockwise)
# Repeats: is the number of times events are to be rotated up to 99
Page 76
71
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
8.11 COPY Events
Copy Events are programmed exactly like Subroutine Events. The only difference is that
in Copy the events are rewritten into subsequent events. If, for example, in event 11 you
copy repeated events 6, 7, 8, 9, 10 with 2 repeats, events 6-10 would be copied with the
input offsets into events 11-15, and recopied into 16-20.
Copy Events may be REPEAT, MIRROR, ROTATE or DRILL to TAP.
Copy is very useful. With Copy you can:
- Edit the events that are being repeated, mirrored or rotated without changing the
original events.
- Program an event parallel to X or Y (where the geometry is the easiest to describe),
rotate it to the desired position, then delete the original.
- Use the clipboard to paste previously stored events from another program into the
current program. After you press the CLIPBOARD key, you will enter the offset from
the previous program's absolute zero to the current program's absolute zero (see figure
below). For information about putting events into the clipboard, see Section 10.4.
In the above example, the offset that puts the group of holes in the desired location is X=-
1.50 and Y=-1.00.
8.11.1 Copy Drill to Tap
The copy drill to tap feature allows you to convert a series of drill events over to a tap
event. Prompts in this event.
First Event #: is the event number of the first drill event to be copied
Last Event #: is the event number of the last drill event to be repeated; if only one event
is to be repeated, the Last Event # is the same as the First Event #
Z Rapid: is the Z dimension to transition from rapid to feed. Make sure that Z rapid is
set high enough to compensate for the amount of float in the floating tapping head.
Z End: the depth of the thread
Page 77
72
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
PITCH - the distance from one thread to the next in inches or mm. It is equal to one
divided by the number of threads per inch. For example, the pitch for a 1/4-20 screw is 1
20 = .05 inches
RPM: spindle RPM
Tool #: is the tool number you assign
8.12 THREAD MILL Event
To program a Thread Mill Event press the THREAD MILL soft key. This event includes
an automatic move in and out by 0.050” of the thread. Prompts in the Thread Mill Event:
X CENTER: the X dimension of the center of the thread
Y CENTER: the Y dimension of the center of the thread
Z RAPID: the Z dimension where the Z rapid feed slows to Z program feed
Z BEGIN: the Z dimension where the threading pass begins
Z END: the Z bottom of the thread
DIRECTION: clockwise or counterclockwise
PITCH: the distance from one thread to the next in inches or mm. It is equal to one
divided by the number of threads per inch. For example, the pitch for a 1/4-20 screw is
1/20 = .05 inches
MAJOR DIA: the largest diameter of the thread (the root for an ID thread, the crest for an
OD thread)
MINOR DIA: the smallest diameter of the thread (the root for an OD thread, the crest for
an ID thread)
SIDE: input 1 for inside, 2 for outside
ANGLE: the angle the tool feeds into the beginning depth
# PASSES: - the number of passes to cut the thread to its final depth
FIN CUT: width of the finish cut. If 0 is input, there is no finish cut.
Z FEEDRATE: is the Z feedrate from Z rapid to Z end in in/min from .1 to 700, or
mm/min from 5 to 17780
XYZ FEEDRATE: The feedrate of XYZ along the path of the helix.
If something other than 0 is input for finish cut, the following prompt appears:
FIN FEEDRATE: the milling feedrate for the finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
FIN RPM: is the spindle RPM for the finish cut.
TOOL#: is the tool number you assign.
8.13 PAUSE Events
The purpose of the Pause Event is to allow you to program a stop condition within the
program. The Pause event will stop the program where it ended at the previous event. If
you open the door during a Pause Event the spindle and coolant will turn off
Page 78
73
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Pause Events are useful if you want to stop the program to make a measurement, change
a fixture, etc.
NOTE: In general, you should avoid programming a Pause Event between two
connective events. The Pause Event will cause the events to NOT be connective.
To program a Pause Event press the PAUSE softkey. Because there is no input required,
simply press SET to load and the event counter will advance by one and the Select Event
screen will reappear.
In run, press the GO key after a pause to continue.
8.14 TAP Events
Tap Events allow rigid tapping. The feedrate of the thread will be calculated from the
pitch and RPM entered. The RPM range that the ProtoTRAK PMX is from 150 to 2000
rpm. An error message will occur if you try to tap outside of these ranges.
To program a tap event press the TAP softkey.
Prompts in the Tap event:
X: the X dimension to the center of the hole (Help key active and allows the selection of
a left-hand thread).
Y: the Y dimension to the center of the hole
Z Rapid: is the Z dimension to transition from rapid to feed.
Z Begin: the top of the work piece
Z End: the depth of the thread
PITCH - the distance from one thread to the next in inches or mm. It is equal to one
divided by the number of threads per inch. For example, the pitch for a 1/4-20 screw is
1/20 = .05 inches
RPM: spindle RPM
Tool #: is the tool number you assign
8.14.1 Tapping Notes and Recommendations
- Harder materials will require slower speeds and tap size may also be limited.
- Make sure your tap is not dull. Dull taps will require more torque to cut and may not
cut threads to specification.
- Cutting oil will play a large role in determining the size of tap you can use in a given
material.
- Make sure your tap is running true in the holder.
- The tap has to attain sufficient speed as it is entering the work piece. The ProtoTRAK
PMX CNC will automatically calculate the distance required to gain momentum and that
distance may be different than the programmed Z Rapid. (That is why we require the Z
Begin dimension).
- Selecting Help (blue question mark) at the first prompt of the Tap event will give you
the ability to switch to a left-hand thread. This choice is not available in the Tap option
of the Bolt Hole event.
Page 79
74
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
8.15 ENGRAVE Event
The Engrave Event allows you to machine numbers, letters and special characters as part
of a part program. See below for the letters and special characters that are available in
the Engrave Event.
When programming with the Engrave Event, the ProtoTRAK will construct a box to
contain the text you define. This box is oriented along the X axis like the text in this
sentence, and you may program up to 40 characters per event (although you will only be
able to see 20 characters on the prompts screen). To machine text in a direction other
than the X axis, simply use multiple Engrave Events and place the lower left corner of the
box wherever you would like. The numbers and letters you program will always have a
standard orientation (like the letters on this page) – you cannot program tilted or inverted
letters with the Engrave Event. The letters are of the font shown in the figure and all
capitals.
Prompts for the Engrave Event:
First, define the lower left corner of the box that will contain your text:
X BEGIN: The X coordinate of where you want your text to begin
Y BEGIN: The Y coordinate of where you want your text to begin
Z RAPID: The Z dimension where the Z rapid feed slows to Z program feed
Z END: The Z dimension to the bottom of your text.
HEIGHT: The height of your text. Each character varies in width; the set height of the
character will change the width in order to keep the overall size of the character
proportional.
TEXT: The text to be milled. When you get to this prompt, the Alpha keys will
automatically pop up to allow you to enter the text. Once you have finished entering text,
you must press End and then any of the SET keys to successfully enter your text into the
event. The alpha keys will appear automatically if the text field is blank. If you have
already entered text but wish to make a change, you will see a blue question mark appear
on the lower left corner of the screen when you scroll to this field, press the Help button
and the alpha keys will appear.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event.
Z FEEDRATE: is the Z feedrate from Z rapid to Z end in in/min from .1 to 800, or
mm/min from 5 to 20320.
XYZ FEEDRATE: The feedrate of XYZ along the path of the text
Tool #: is the tool number you assign
Page 80
75
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
The above figure shows the text and special characters available for the Engrave event.
Input
Function
Comments
1
Coolant
The coolant pump will be turned on when this event begins to run.
2
Air on
The air solenoid will be turned on when this event begins to run.
3
Coolant Off
Turns the coolant off at the end of this event.
4
Air Off
Turns the air solenoid off at the end of this event.
5
Pulse
Indexer
Activates a 0.3 second electronic pulse at the beginning of the event.
See note below.
6
Part Change
Brings the table and saddle forward for convenient access to the fixture
Notice the field that is labeled “Text Length”. This field will display the total length of
your programmed text and will update as you enter each character.
8.16 Auxiliary (AUX) Functions Event
Auxiliary operations are programmed as events in the ProtoTRAK PMX CNC to make it
easier to turn functions on and off for the entire program.
When running programs with Auxiliary functions, the Coolant and Air hard keys on the
Run panel must be in the correct position. If you want the program to automatically turn
the Auxiliary functions on and off, press the hard key until the light is on in the AUTO
position.
Auxiliary Event options:
Page 81
76
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Position
or work piece. The position along the X axis may be changed using a
Service Code.
7
4th Axis
Auto Clamp
OFF
Turns off the auto clamp feature on 4th axis units that require air to run.
8
4th Axis
Auto Clamp
ON
Turns on the auto clamp feature on 4th axis units that require air to run.
The default if no AUX event is program is to auto clamp.
9
Cornering –
Blend or
Exact Stop
Allows the program to blend a corner or exact stop in the corner.
When you blend moves, some accuracy will be lost. This cornering
AUX really only applies or has an impact when S curves are turned on
in service code 508. See S curve section below.
Coolant/Air on and off is automatically programmed for tool changes.
The Pulse Indexer function is designed to operate with a standard indexer. Programming
a Pulse Indexer will cause the ProtoTRAK PMX CNC send a signal to the connected
indexer or rotary table and then wait for the return signal that the devise has finished its
programmed move. The ProtoTRAK PMX CNC then it will resume machining at the
next event.
S Curve Information – turned on and off with service code 508
1. S curves are utilized when your feedrate is greater than 40 ipm. For feedrates below
40 ipm, there is no value to S curves. The surface finish seen under a end mill is
generally improved when S curves are used.
2. In our AUX event, we have added a new prompt under 9 that gives the user the
choice to have the control perform corner blending (G64) or exact stop (G61). The
default is exact stop when S curve is turned on and this applies to feedrates that are
greater than 40 ipm. Please see the figure below for how the AUX event looks.
a. Exact stop means the control will get into exact position and there will be
minimal error. This may add some additional time to run a program versus if
blending is used or if S curves were turned off.
b. Corner blending will make the machine blend or round a corner. The machine
will not get into exact position and hence you will see some error when
machining. The error is dependent on the feedrate you are machining at. The
higher the feedrate, the more error you will see. With corner blending on, the
machine will not slow down as much in the corners and your cycle time will
be faster. Please note that cornering error will only show up at feedrates
above 40 ipm.
c. Please note that G61 exact stop and G64 corner blending are common G codes
found on many CNC controls and not unique to Southwestern Industries.
G64 is often labeled as G61 cancel versus the corner blending term we use but
it is in essence the same thing.
Page 82
77
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
3. Please note that if you do use corner blending in your program, we will automatically
get into exact position on the following moves or events.
a. Bore and drill event – the final depth that you program in your event will get
into exact position.
b. All position or rapid moves will get into exact position. For example, if you
are rapiding out of a hole in Z and then positioning in X and Y to a new hole
location, the control will get into exact position. You don’t have to worry
about the control rounding the corner if you have corner blending on.
c. All individual Z moves that lead into XY moves will get into exact position.
For example, when you feed down to the bottom of any pocket or profile, we
will get into exact position before moving the X or Y axis.
d. Helix and thread mill events will get into exact position at the beginning and
end of the event.
e. Please note that when you are using tool compensation (tool right or tool left)
and making a sharp outside corner, we generate a walk around arc to create
the corner. This means the error will be minimal with corner blending turned
on.
4. The following are the some notes about how exact stop (G61) works.
a. Exact stop will only be used when the machine makes a change of direction
where the angle between the line you are on to the next line is less than 170
degrees or larger than 190 degrees. See the illustration below for what this
specifically means.
Page 83
78
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
b. Surfacing type programs that are comprised of small moves that have small
angles between the moves should not require a G64 or corner blending to be
turned on to avoid hesitation.
c. All moves that are tangent to each other also will not have exact stop (G61)
apply. Please note that when making a 90° outside corner with tool
compensation applied, we generate an arc to machine the sharp corner so
these moves are tangent.
d. For all moves where exact stop will apply, the user may notice a slight
hesitation on these moves. This is due to the control getting into exact
position before performing the next move.
Page 84
79
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
9.0 Program Mode
Part 3: The Auto Geometry Engine (A.G.E.)
Programming
This entire section deals with the Auto Geometry Engine which is automatically started
when you program an Irregular Pocket (Section 8.6.3) or an Irregular Profile (Section
8.8.3).
The A.G.E. is powerful software that works behind the easy-to-use geometry
programming of the ProtoTRAK PMX CNC. It is treated in its own section because it
works differently than the other event types. Unlike other events, the A.G.E. allows you
to:
- Enter the data you know, and skip the prompts you don’t.
- Use different types of data (like angles) that may be available from the print.
- Enter guesses for the X and Y ends and centers not available on the print.
With the A.G.E., you can easily overcome limitations in the data the print provides
without having to spend time in laborious calculations.
9.1 Starting the A.G.E.
The A.G.E. is started automatically when you enter the Irregular Pocket or Irregular
Profile event. The first set of prompts you encounter will be the header information.
Once that information is entered, you will see the following screen:
Page 85
80
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Once the profile header screen is finished, you choose between an A.G.E. Mill and an
A.G.E. Arc to define the shape.
Where:
A.G.E. MILL: A straight line from one X Y point to another.
A.G.E. ARC: Any part of a circle.
END A.G.E.: Ends the A.G.E. programming for the Irregular Pocket or Irregular Profile.
ABORT A.G.E.: Aborts all A.G.E. events. The data for all the events is lost.
9.2 A.G.E. Mill Prompts
Press the A.G.E. Mill key.
A.G.E. Mill prompts. Enter what you know, skip or guess the ones you don’t.
Prompts in A.G.E. Mill programming:
TANGENT: this refers to the tangency of the mill to the previous event. See Section
9.11 for a discussion of tangency.
X END: is the X dimension to the end of the mill cut; incremental is X Begin
Y END: is the Y dimension to the end of the mill cut; incremental is Y Begin
CONRAD: is the dimension of a tangential radius to the next event
ANGLE END: is the angle measured counterclockwise from this mill event to the next.
Do not input if the next event is an arc
LENGTH: is the length of the mill from beginning to end
Page 86
81
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
LINE ANGLE: is the angle of this mill line (moving from begin to end) measured
counterclockwise from the positive X axis (that is 3 o’clock)
GUESS: This softkey will appear when the prompt is on X or Y dimensioned data. Press
the Guess key before you press INC SET or ABS SET to enter the data as a guess. See
Section 9.7 for using Guess and Section 9.8 for using the Graphics to enter a Guess.
9.3 A.G.E. Arc Prompts
Press the A.G.E. ARC key.
Prompts in A.G.E. Arc programming:
TANGENT: this refers to the tangency of the mill to the previous event. See Section
9.11 for a discussion of tangency.
DIRECTION: is the clockwise (input 1), or counterclockwise (input 2) direction of the
arc
X END: is the X dimension to the end of the arc cut; incremental is from X Begin
Y END: is the Y dimension to the end of the arc cut; incremental is from Y Begin
X CENTER: is the X dimension to the center of the arc; incremental is from X End
Y CENTER: is the Y dimension to the center of the arc; incremental is from Y End
CONRAD: is the dimension of a tangential radius to the next event
RADIUS: is the radius of the arc
CHORD LENGTH: is the straight line distance from the begin point to the end point
CHORD ANGLE: is the angle spanned by the arc
In addition to the normal Softkeys, this additional one will appear in A.G.E. Arc
programming:
GUESS: this softkey will appear when the prompt is on X or Y dimensioned data. Press
the Guess key before you press INC SET or ABS SET to enter the data as a guess. See
Section 9.7
9.4 Skipping Over Prompts
In the A.G.E., events don't have to be fully defined before you can go to the next one.
You can skip the data you don’t know by using the cursor hard keys on the Program
Panel. After you press the arrow down key at the last prompt, the event will move to the
left side of the screen and the Select Event screen will appear.
When skipping over prompts or editing, always use the cursor keys. Using INC SET or
ABS SET will change the data.
If you want the event back on the right side, use the left hard key.
9.5 The OK/NOT OK Flag
Each A.G.E. event has a flag that tells you if it has been fully defined. Sometimes data
from later events is needed to define previous events. To the immediate right of the event
Page 87
82
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
type, the words OK or NOT OK appear, depending on whether that particular event is
defined.
Once the OK flag appears for the event, you do not need to enter more information. Skip
past the rest of the prompts with the down cursor hard key.
If you leave the Program Mode and then return, pressing the GO TO END softkey will
take you automatically to the first NOT OK event.
9.6 Ending A.G.E.
Any time all the events are of an Irregular Profile are OK, the A.G.E. may be ended. If
you are programming an Irregular Pocket, there is an additional requirement that must be
satisfied before the A.G.E. may be ended: the X and Y end point of the last event must be
the same as the X and Y beginning point, so that the pocket is closed.
Otherwise, the ProtoTRAK PMX CNC cannot program the tool path to clear the pocket.
The Irregular Profile has no such restriction since profiles may be open or closed.
Once the A.G.E. is ended, the Irregular Pocket or Irregular Profile event is complete and
you may then choose from all the programming canned cycles from the Select an Event
screen. To reopen the A.G.E. Profile or Pocket, simply use the left cursor hard key to
position on of the A.G.E. events on the right side of the screen. You may edit or insert
other events.
9.7 Guessing Data
Whenever you are missing X or Y Ends or Centers, you should generally enter a guess.
Guessed data is treated differently by the ProtoTRAK PMX CNC than regular data.
Often, the information you put into the system will allow it to calculate a mathematically
correct line or arc that would satisfy the conditions of the hard data you entered. This
line or arc may yield more than one solution to particular point you are looking for. That
is where the Guess comes in: the A.G.E. uses the guess to choose from the
mathematically possible solutions. In most cases, your guesses do not have to be very
precise. The smaller the lines or arcs, the more precise the guess should be.
Page 88
83
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
The X End dimension has been entered as a guess - note the letter G
Guesses should always be entered as absolute dimensions. Once entered, the guessed
data will have a 'G' next to it. Guessed data will be labeled this way in all the events that
are flagged NOT OK. Once an event is OK, the guessed data will be replaced by
calculated data. If you wish to edit your guesses, placing it on the right side of the screen
will cause your original guessed data to reappear.
You can enter a combination of guessed and non-guessed data. For example, if you were
to enter the dimension for X End without guessing, you would still be able to enter the
dimension of Y End using guess.
9.8 LOOK and Guess
Guessed data may be entered by pressing the number keys and then SET. However, you
may find it more convenient to use the LOOK graphics to enter guesses. When prompted
to enter a guess you can press LOOK to go to a special version of the LOOK graphics.
Using the cursor keys, you may move a point around the screen. When you come to the
place where your point is, use the Enter sofg key.
Your guess entries are loaded into the program when you exit the LOOK screen by
pressing LOOK again. The ProtoTRAK will use the last ENTER key press and load that
into the program.
Page 89
84
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
When you use the graphics to guess dimensions on arcs, you may load in guesses for both
the X/Y End and the X/Y Center before leaving the LOOK screen.
When you have not first pressed the Guess key, pressing LOOK gives you the same
screen as in regular programming. Whether you enter the guesses as key presses or by
using the graphics, the drawing of the LOOK screen distinguishes between events that are
fully defined and those that rely on guessed data. OK events are represented by solid
lines. NOT OK events are represented by dashed lines.
9.9 Calculated Data
Prompts that are skipped or for which guesses are entered may be replaced by data
calculated by the ProtoTRAK PMX CNC. Calculated data is shown in red in order to
distinguish it from the data that you entered. You cannot edit calculated data, but you
may edit your original input. By putting the event with the calculated data on the right
side of the screen, you may position the cursor to the prompt and re-input the data.
9.10 Arcs and Conrads
If the print is missing a lot of data, it may be desirable to program arcs as separate events
where possible. If you know the center and radius of an arc, program it as an arc rather
than using the Conrad. This gives the system more information to work with in figuring
out other missing points.
Page 90
85
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
9.11 Tangency
Tangency can occur between a mill and arc or an arc and arc. Specifically it means that
the two events share one and only one point. You would answer yes to the TANGENCY
prompt if the event you are programming is tangent to the previous event. The
information that events are tangent helps the Auto Geometry Engine calculate other
dimensions.
You can often tell by looking at the print if events are tangent: tangent intersections tend
to blend smoothly, without a sharp corner.
Smooth, probably tangent sharp, not tangent
For the A.G.E., the tangent mill or arc is assumed to continue in the same direction, and
not double back on the previous event:
Like this not this
Page 91
86
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
10.0 Edit Mode
Within Program Mode, you can recall and re-input specific data prompt by prompt.
The changes you make in the Edit Mode affect only the program in current memory. In
order to preserve the changes for future use, the program must be stored again under the
same name in the Program In/Out Mode.
10.1 Delete Events
To delete a group of events in the program, press DELETE EVENTS.
The Data Input Line will prompt for the first event to be deleted. Input the event number
of the first event and press SET. Next the Data Input Line will prompt for the last event
number to be deleted. Put in the last number and press SET.
The remaining events will be renumbered.
10.2 Spreadsheet Editing
Spreadsheet Editing allows you to view program inputs in a table and make global
changes to the program. This is particularly useful if you are working with a large
program and you need to make a change to many events.
When you press the SEARCH EDIT softkey, the screen will load a table that contains
data for every event.
The Search Edit softkey launches Spreadsheet Editing. View the entire program by the
variables you select.
Page 92
87
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
The first time the screen appears, the data is sorted by event number. Each row
represents the data for the event number shown in the first column on the left. The event
number is always displayed in the first column, but the other data displayed on the table
can be changed.
Soft Keys in Search Edit:
PAGE FWD: pages forward through the table.
PAGE BACK: pages backwards through the table.
SORT: enables you to change the sort to any of the data displayed. See Section 10.2.2
CHANGE ALL: enables you to make global changes of data. See 10.2.3
Arrow Buttons on Program Panel:
The 4 arrow buttons on the program panel allow you to cursor throughout the spreadsheet
and highlight the data you want to edit. Only data that is highlighted and appears in the
Data Input Line may be edited. Note: the EVT# (event number) and (event) TYPE may
not be edited in Search Edit so the highlighter will not go there.
10.2.1 Selecting Data to be Displayed on the Search Edit Table
In order to change the data selected in the table, press the HELP hard key. There will be
a listing of all the data types that may be edited in Search Edit. Press the RETURN soft
key and the table will be reloaded with the data that you selected.
Pressing Help while viewing the spreadsheet lets you change the program parameters.
Page 93
88
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
After you press the HELP hard key, the screen will display all the different parameters
that can be displayed on the spreadsheet. To either select or deselect any parameter,
simply highlight that parameter and press SET. When you are finished, press the Return
softkey and return to the spreadsheet.
10.2.2 Sorting Data
Data may be sorted by any of the data types displayed in the column head. Red letters
show which column is used for sorting the data.
To change the sort, press the SORT softkey, then select the type of data you want to use
for sorting from the softkeys.
The table will be changed to sort the data in ascending order (the smallest value first, the
largest last).
10.2.3 Making Global Changes to Data
Sometimes it is useful to be able to change data in a program without having to go
through each event one at a time. For example, if you were to want to change the tool
number for every milling event, it may be a chore to go through each event in a long
program to make the changes on that event type.
In order to make global changes:
1. Sort the data in a way that groups together the things you want to change.
2. Highlight the data value that is highest on the table (nearest to the top) that you want
changed.
3. Press the CHANGE ALL softkey. All the inputs that are the same as the one you
highlighted and are listed together below the data you highlighted will then be
highlighted.
4. Enter the new value, then press set. All the highlighted data will be changed to the
value you just input.
Example:
From the screen shown in 10.2, we will change the Z Feed for each of the mill events in
the program.
1. Sort by event type to get all the Mill events together.
2. Highlight the Z Feed in the first Mill event (Event # 8).
Page 94
89
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
After sorting by Event Type, the highlighter is placed on the Z feed of the first Mill Event
3. Press the CHANGE ALL softkey. All the Z Feeds in the Mill events are highlighted.
Page 95
90
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Pressing the Change All softkey highlights the Z feed for all the Mill events.
4. Type in the new Z Feed value and press INC SET or ABS SET.
Page 96
91
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Type the new Z Feed and then SET to change all the highlighted values from 50 to 40.
In this example, the Z feed is changed from 50 to 40 for all the Mill Events.
10.3 Erase Program
Use the ERASE PROG soft key to erase the program from the current memory. Erasing
the program from current memory will not affect any programs that are stored.
If you have made changes to the program and wish to save this modified program, you
will need to store it. See Section 14.4
10.4 Clipboard
The Clipboard feature is a way to copy events in one program in order to put them into a
different program. It is a two-part process that takes place in two different Modes. First,
in the Edit Mode, the desired events are copied, or placed on the Clipboard, from the
source program. Then the events are inserted into the destination program in the Program
Mode.
When you press the Clipboard key from the Edit Mode, you start the process that copies
the events that you want to put into a different program than the one in current memory.
Before you do that, you should write a program or open the program file that has the
events you want to copy. This is called the source program.
Page 97
92
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Inspect the events you want to copy. Make sure that the dimensioned data uses Absolute
references in the first event to be copied and in all events where it will be important.
Incremental references may be used, but keep in mind where the Incremental reference
will be made from. See the section on Incremental Reference Position in this manual.
In addition, you may want to modify this program in order to get all the events you want
together. For example, if you want to copy events 2-5 and 7-12, you may want to modify
the program to delete events 1 and 6 first. That way, you can copy the all the events as
they are now numbered from 1 to 10. Remember that you can modify this program just
for this purpose and it will not affect the original program unless you save it with the
modifications in the Program In/Out Mode.
When the source program is ready, press the CLIPBOARD softkey. A message will
appear that says "Copy Events Onto Clipboard" and the Data Input Line will read "From
Event". Enter the number of the first event that you want copied and press SET.
The Data Input Line will read "To Event". Enter the number of the last event you want
copied and press SET.
The group of events that you have specified is now on the clipboard and will remain there
until you replace it with something else by going through the same procedure. When
power is turned off to the CNC the clipboard information will also be lost.
The events on the clipboard are inserted into a program in the Program Mode. See
Section 8.11.
Page 98
93
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
10.5 G-Code Editor
The G-Code Editor allows the edit of G-Code programs that are opened as .GCD or PTG
files. Once edited, the program may be re-saved as .GCD or PTG files. ProtoTRAK
Geometry-style programs may not be saved as .GCD or PTG files.
Use the G-Code Editor to modify G-Code programs.
You must connect a mouse and keyboard in order to use the G-Code Editor.
When you enter the G-Code Editor, the G-Code program is displayed starting at the first
Block Number. Use the scroll bar to move up and down through the program. Use the
mouse and keyboard to edit like you would an MS Notepad™ file.
Search allows you to launch a simple find-and-replace routine to aid in editing large GCode files.
Page 99
94
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
The find and replace routine.
Click in the FIND WHAT box and enter the item you want to find. Click on THE FIND
NEXT box and the G-Code Editor will locate the next occurrence of that item.
Successive clicks on Find Next will continue to search through the program. Use Match
Whole Word to limit the search to the entire word. For example, if you want to find G2,
but not G20 or G22, select Match Whole Word Only.
Instead of typing the item into the Find What box, you may simply highlight an item on
the G-Code Editor screen. That item will be entered into the Find What box for you.
To make changes to Find What items, type what you want to have into the Replace With
box. You can replace items one at a time by clicking first the FIND NEXT box then the
REPLACE WITH box for as many changes as you want to make. You can replace every
item in the program with a single click of the REPLACE ALL box.
Return closes the G-Code Editor and returns the screen to the Edit Mode.
Note: If you use the USB Thumb Drive to store a G-code (.gcd) program file, you must
leave the Thumb Drive plugged into the USB port the entire time the program is in
current memory. If you unplug the thumb drive with the program still in current
memory, the ProtoTRAK will display an error message.
Page 100
95
Southwestern Industries, Inc.
TRAK LPM Programming, Safety, & Operating Manual
Any change made in the editor will be applied the next time you run the program. To
permanently save these changes, go to PROG IN/OUT screen and use the save feature.
10.6 Update GCD
The UPDATE GCD button will show up when a .PTG file is loaded into memory. This
feature allows you to update the G code file that is linked within the .PTG file. This is
useful when you go back to your offline computer and update your G code file and then
want to re-insert it into your .PTG file.
If you load just a .GCD file into memory, then this button will be grayed out until you
save the program as a .PTG file. A .PTG file is created when you save a G code file with
notes and pictures.
When using UPDATE GCD, you must first remove the link to the G code file that is in
your .PTG file. To do so, press the TAB softkey and highlight the file in question and
then press REMOVE ITEM as shown in the figure below.
Loading...