Page 1
XYZ Turret Mill
ProtoTRAK SMX CNC
Safety, Programming, Operating, & Care Manual
Covers Models:
•
XYZ Turret Mill with 2-Axis CNC
SMX SLV SMX2
SMX 1500 SMX2
SMX 2000 SMX2
SMX 3000 SMX2
•
XYZ Turret Mill with 3-Axis CNC
SMX SLV SMX3
SMX 1500 SMX3
SMX 2000 SMX3
SMX 3000 SMX3
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
e-mail: sales@southwesternindustries.com | service@southwesternindustries.com |
web: southwesternindustries.com
Document: 25049
Version: 042913
Page 2
Service Department
Tel:
01823 674214
Fax:
01823 674201
Copyright © 2013 XYZ Machine Tools, Ltd. 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 XYZ Machine Tools, Ltd.
While every effort has been made to include all the information required for the purposes of this guide,
XYZ Machine Tools 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.
XYZ Machine Tools
Woodlands Business Park
Burlescombe, Nr Tiverton
Devon, EX16 7LL
Page 3
i
XYZ Machine Tools, Ltd.
XYZ Turret Mill, ProtoTRAK SMX CNC Safety, Programming, Operating and Care Manual
Table of Contents
1.0 Introduction 1
1.1 Conditions of This Manual
1.2 Manual Organization
2.0 Safety Specifications & 2
Lubrication
2.1 Health and Safety Directives
2.2 Danger, Warning Labels & Notes
2.3 Safety Precautions
3.0 Description 12
3.1 Control Specifications
3.2 Display Pendant
3.3 Machine Specifications
3.4 Auto Lube System
3.5 Servo Motors
3.6 Ballscrews
3.7 Electrical Cabinet
3.8 Z Scale
3.9 Auxillary Functions
3.10 Work Light
3.11 Coolant Pump
3.12 Chip Pan/Splash Shield
3.13 Table Guard
3.14 Z Ballscrew and Motor Assy
3.15 Limit Switch
3.16 Optional Equipment
4.0 Basic Operation 27
4.1 Basic Control Operation
4.2 Basic Machine Operation
5.0 Definition, Terms & Concepts 37
5.1 ProtoTRAK Axis Conventions
5.2 Part Geometry & Tool Path Prog
5.3 Planes and Vertical Planes
5.4 Absolute and Incremental Refs
5.5 Referenced & Non Ref Data
5.6 Incremental Ref Position and Prog
5.7 Tool Diameter Compensation
5.8 “ “ When Contouring in Z
5.9 Connective Events
5.10 Conrad
5.11 Memory and Storage
6.0 DRO Mode 43
6.1 Enter DRO Mode
6.2 DRO Functions
6.3 Jog
6.4 Power Feed
6.5 Do One
6.6 Go To
6.7 Teach
6.8 Return Abs Zero
6.9 Tool #
7.0 Program Mode 47
7.1 Programming Overview
7.2 Enter Program Mode
7.3 Program Header Screen
7.4 Auxillary Funtions
7.5 Multiple Fixtures
7.6 Assumed Inputs
7.7 Z Rapid Positioning
7.8 Softkeys within Events
7.9 Programming Events
7.10 Editing Data while Programming
7.11 Look
7.12 Finish Cuts
7.13 2 vs. 3 axis Programming
8.0 Program Mode 57
Part Two: Programming Events
8.1 Position Drill
8.2 Bolt Hole Events
8.3 Mill Events
8.4 Arc Events
8.5 Pocket Events
8.6 Islands Events
8.7 Profile Events
8.8 Engrave Events
8.9 Subroutine Event
8.10 Copy Event
8.11 Finish Teach Event
9.0 Three Axis Program Events 70
9.1 Position Events
8.2 Drill Events
8.3 Bolt Hole Events
8.4 Mill Events
8.5 Arc Events
8.6 Pocket Events
8.7 Islands Events
8.8 Profile Events
8.9 Helix Events
8.10 Subroutine Event
8.11 Copy Event
8.12 Thread Mill Event
8.13 Pause Event
8.14 Engrave Event
8.15 Finish Teach Event
10.0 AGE Programming 91
10.1 Starting the AGE
10.2 AGE Mill Prompts
10.3 AGE Arc Prompts
10.4 Skipping Over Prompts
10.5 The OK/Not OK Flag
10.6 Ending AGE
10.7 Guessing Data
10.8 Look and Guess
10.9 Calculated Data
10.10 Arcs and Conrads
10.11 Tangency
11.0 Edit Mode 97
Page 4
ii
XYZ Machine Tools, Ltd.
XYZ Turret Mill, ProtoTRAK SMX CNC Safety, Programming, Operating and Care Manual
11.1 Delete Events
11.2 Spreadsheet Editing
11.3 Erase Program
11.4 Clipboard
11.5 G Code Editing
12.0 Set-Up Mode 104
12.1 The Tool Table
12.2 Tool Path
12.3 Reference Position
12.4 Fixture Offsets
12.5 Verify Part
12.6 Service Codes
13.0 Run Mode 116
13.1 Run Mode Screen
13.2 2 vs. 3 axis Programming
13.3 Starting a Run
13.4 Program Run
13.5 TRAKing
13.6 Program Run Messages
13.7 Stop
13.8 Feedrate and Speed Override
13.9 Trial Run
13.10 Data Errors
13.11 Fault Messages
14.0 Program In/Out Mode 120
14.1 Softkey Selections
14.2 Basic Navigation of Screens
14.3 Opening a File
14.4 Saving Programs
14.5 Copying Programs
14.6 Deleting Programs
14.7 Renaming Programs
14.8 Backing Up Programs
14.9 Converters
14.10 Compatibility with other Models
14.11 Running G Code Files
14.12 Networking
14.13 Cad/Cam Post Processor
15.0 Sample Program 147
15.1 Sample Program #1
15.2 Sample Program #2
Page 5
1
XYZ Machine Tools Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
1.0 Introduction
Congratulations! Your new XYZ Turret Mill with the ProtoTRAK SMX CNC is an excellent allaround addition to your shop. The ProtoTRAK SMX has an easy-to-use interface and dozens of
features that maximize your productivity for any small-lot production job.
Manual Machining is always available and made easier with features like power feed, 2500
mm per minute rapids, tool offsets and all the best features of sophisticated DRO’s.
Two-Axis Machining is available at the touch of a button for the prototyping and
moderately complex, low volume work that is typically done on knee mills.
Three-Axis CNC Machining is also available for models with the ProtoTRAK SMX3.
Programs may be entered at the control or imported from other applications such as
CAD/CAM.
The operation of the ProtoTRAK SMX CNC has been painstakingly refined to bring you the
best in technology while retaining the ease of use that has made ProtoTRAK the top brand in
controls for low volume production.
The ProtoTRAK SMX CNC allows you to chose the CNC configuration that is right for you. The
base system is a powerful CNC for toolroom work. You may add options for additional
features and capabilities.
This manual will describe the operation of all basic and optional features in the appropriate
context. Where optional features are discussed, a note will explain in which option the
particular feature is found.
1.1 Conditions Of This Manual
All details contained in this manual are accurate at the time of going to press E & OA,
but please be aware that XYZ Machine Tools has a policy of continuous development,
and because of this some details are subject to change without prior notice. Please
be sure to confirm any important specifications and details prior to ordering.
1.2 Manual Organization Notes
This manual covers the operation of all XYZ Turret Mill products that use the ProtoTRAK SMX
CNC.
Some Sections do not apply to all users. For example, if you own a ProtoTRAK SMX 2-axis
machine, you should skip Section 9, Three-axis program events.
Sections that may not apply to all users contain a note to inform you of this fact.
Section 2 of this manual provides important safety information. It is highly recommended
that all operators of this product review this safety information carefully.
.
Page 6
2
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
2.0 Safety
The safe operation of your turret mill depends on its proper use and the precautions taken by
each operator.
Read and study this manual. Be certain every operator understands the operation
and safety requirements of this machine
Always wear safety glasses and safety shoes.
Always stop the spindle and check to ensure the CNC control is in the stop mode
before changing or adjusting the tool or workpiece.
Never wear gloves, rings, watches, long sleeves, neckties, jewellery, 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.
2.1 Health and Safety Directives and Standards
XYZ Milling Machines are certified to comply with the following Directives and
Standards.
EC Machinery Directive 98/37EC
EMC Directive 89/336/EEC
Low Voltage Directive 73/23/EEC
BS EN 13128 Safety of machine tools- Milling machines (including boring machines).
BS EN 1837 Safety of machinery-Integral lighting of machines.
BS EN 60204 Safety of machinery-Electrical equipment of machines.
BS EN 954-1 Safety of machinery Safety related parts of control systems
BS EN 292-2 Safety of machines Basic concepts, general principles for design.
BS EN 1050 Safety of machinery, Principles for risk assessment.
BS EN 953 Safety of machinery. Guards, general requirements for the design and
construction of fixed and movable guards.
BS EN 60529 Degrees of protection provided by enclosures.
2.2 Danger, Warning, Caution, and Note Labels and Notices As Used
In This Manual
before
its use.
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
and/or damage to the equipment. Warning labels on the machine are orange in
color.
CAUTION - Hazards or unsafe practices that
equipment/product damage. Caution labels on the machine are yellow in color.
NOTE - Call attention to specific issues requiring special attention or understanding.
could
result in severe personal injury
could
result in minor personal injury or
Page 7
3
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Safety & Information Labels Used On The
XYZ Turret Mills
It is forbidden by law to deface, destroy or remove any of these labels
Page 8
4
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Safety & Information Labels Used On The
XYZ Turret Mills
It is forbidden by law to deface, destroy or remove any of these labels
Page 9
5
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Safety & Information Labels Used On The
XYZ Turret Mills
It is forbidden by law to deface, destroy or remove any of these labels
Page 10
6
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Safety & Information Labels Used On The
XYZ Turret Mills
It is forbidden by law to deface, destroy or remove any of these labels
Page 11
7
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Safety & Information Labels Used On The
XYZ Turret Mills
It is forbidden by law to deface, destroy or remove any of these labels
Page 12
8
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Safety & Information Labels Used On The
XYZ Turret Mills
It is forbidden by law to deface, destroy or remove any of these labels
Page 13
9
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
415 VOLTS
Safety & Information Labels Used On The
ProtoTRAK SMX CNC
It is forbidden by law to deface, destroy or remove any of these labels
Page 14
10
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
2.3 Safety Precautions
1. Do not operate this machine before the ProtoTRAK SMX CNC Safety,
Installation, Maintenance, Service and Parts List Manual, and the
Safety, Programming, 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
jewellery 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 (wrenches, check keys, etc.) 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
Before you make an adjustment to the part, fixture, coolant nozzle or
take measurements
Before you open safeguards (protective shields, etc.). Never reach
for the part, tool, or fixture around a safeguard.
11. Protect your eyes and the machine as well. Don't use a compressed air hose
to remove the chips or clean the machine (oil, coolant, etc.).
12. Stop and disconnect the machine before you change belts, pulley, gears.
13. Keep work area 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.
Page 15
11
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
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 the 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.
19. Use proper cutting tools for the job. Pay attention to the rotation of the
spindle: Left hand tool for counterclockwise rotation of spindle, and right
hand tool for clockwise rotation of spindle.
20. 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 or
power feed.
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. Large overhang on cutting tools when not required result in accidents and
damaged parts.
24. 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.
25. Prevent fires. Keep flammable materials and fluids away from the machine
and hot, flying chips.
26. When working in manual mode (not CNC) make sure the computer control is
switched to DRO or OFF.
Page 16
12
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
3.0 Description
3.1 ProtoTRAK SMX CNC Specifications
In its base form, the ProtoTRAK SMX CNC is powerful and easy to use. For turret mill
applications, the two-axis CNC is usually preferred because of its simplicity and ease of use.
When three-axis CNC is required, a ballscrew and motor is mounted to the head to drive the
quill.
The list below summarizes the features and specifications. Each feature is described in more
detail in the appropriate section of the manual.
3.1.1 Basic System Specifications
Control Hardware
2 or 3-axis CNC, 3-axis DRO
Real handwheels for manual operation
10.4” color active-matrix screen
Industrial-grade Intel processor
256 Mb Ram
P/S 2 Keyboard connector
2 USB connectors
Override of program feedrate
LED status lights built into display
TEAC floppy drive
Software Features – General Operation
Clear, uncluttered screen display
Prompted data inputs
English language – no codes
Soft keys - change within context
Windows® operating system
Selectable two or three-axis CNC (three-axis CNC models)
Color graphics with adjustable views
Inch/mm selectable
Convenient modes of operation
DRO Mode Features for Manual Machining
Incremental and absolute dimensions
Jog at rapid with override
Powerfeed X, Y (or Z for three-axis CNC models)
Do One CNC canned cycle
Teach-in of manual moves
Servo return to 0 absolute
Tool offsets from library
Z Go To (three-axis CNC models only)
Program Mode Features
Geometry-based 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
Canned cycles
o Position
o Drill
o Bolt Hole
o Mill
o Arc
o Circle pocket
Page 17
13
XYZ Machine Tools Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
o Rectangular pocket
o Circular profile
o Rectangular profile
Program pause
Conrad – automatic corner radius
Math helps with graphical interface
Auto load of math solutions
Tool step over adjustable for pocket routines
Pocket bottom finish pass (three-axis CNC models)
Selectable ramp or plunge cutter entry (three-axis CNC models)
Subroutine repeat of programmed events
Nesting
Rotate about Z axis for skewing data (three-axis CNC models)
Edit Mode Features
Delete events
Erase program
Set Up Mode Features
Program diagnostics
Advanced tool library
Tool names
Tool length offset with modifiers(three-axis CNC models)
Advanced diagnostic routines
Software travel limits
Tool path graphics with adjustable views
Run Mode Features
Trial run at rapid
3D CAM file program run (three-axis CNC models)
3D G code file run with tool comp (three-axis CNC models)
Real time run graphics with tool icon
Z Go To (for two-axis run on three-axis CNC models)
Program In/Out Mode Features
Simple program storage to floppy
CAM program converter
Converter for prior-generation ProtoTRAK programs
3.1.2 Advanced Features Option
The Advanced Features Option may be purchased with the original order or
purchased later. Note, the Advanced Features Option is included in the ProtoTRAK
Offline Software, but must be purchased separately for each ProtoTRAK SMX CNC.
It is easy to tell if you have the Advanced Features Option. If you have the Advanced
Features Option, the features listed below will be active. If you do not, the features
listed below will not be active and any Softkey for that feature will be grayed out. For
example, in the Program Mode, under Pocket, check the Softkey labeled IRREG PCKT.
If the words “IRREG PCKT” are black, the Advanced Feature Option is active. If they
are gray, the Advanced Feature Option is not active.
The other way to tell if the Advanced Features Option is active is to go to Service
Code 318. The Advanced Features Option is active if the letters are in black, inactive
if they are in gray.
With the Advanced Features Option, you get the following:
Auto Geometry Engine ™ (see Section 9.0)
3-axis conversational programming (three-axis CNC models)
Additional Canned Cycles:
- Irregular Pocket (8.6.3)
- Face Mill (8.6.8)
- Circle Island (8.7.1)
Page 18
14
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
- Rectangular Island (8.7.2)
- Irregular Island (8.7.3)
- Irregular Profile (8.8.3)
- Helix (three-axis CNC models) (8.9)
- Thread milling (three-axis CNC models) (8.12)
- Engrave (8.14)
- Tapping (8.15)
G-Code editor
Countdown clock to next pause or tool change
Total program time estimator
Spreadsheet editing
Global data change
Scaling of print data
Multiple fixture offsets
Event comments
Tool path conversational programming
Mirror of programmed events
Copy with or without offsets
Copy Rotate
Copy Mirror
Copy Drill to Tap
Clipboard to copy events between programs
If the Advanced Features Option is not active you may purchase it easily. The
Advanced Features Option is a software option so it is simply a matter of entering the
Activation Password into the ProtoTRAK.
To obtain the Password, see the instructions in section 3.1.8 below.
3.1.3 Networking Option
The Networking Option gives you powerful choices in program storage and handling.
This option may be ordered with your machine or at any time after it is installed in
your shop. A RJ45 port is found on each pendant to hook up your networking cable.
See figure 3.2.2 below for the location of this port.
3.1.4 Installing and using the USB Thumb Drive Flash Memory
The first time you install the USB Thumb Drive, we recommend that you install it after
the ProtoTRAK SMX has booted up. Once it is installed, the memory will be
accessible on Drive D. If you want to buy additional thumb drives, these are readily
available in computer stores. We recommend SanDisk® brand, 128MB or higher.
Other brands may require the installation of separate drivers.
3.1.5 The DXF File Converter Option
The DXF File Converter Option gives you powerful capability for quickly and easily
translating DXF and DWG files into ProtoTRAK SMX programs. If you work with CAD
drawings, we highly recommend that you get a demo of the DXF file converter.
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
To tell if the DXF File Converter is active on your ProtoTRAK SMX 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.
Page 19
15
XYZ Machine Tools Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
The DXF Option Consists of additional software and an Activation Password. The
software can be shipped to you. See Section 3.1.8 below for instructions on ordering
and obtaining your Activation Password.
The DXF Option has its own manual which is shipped with the software.
3.1.6 Converter Options
Optional converters are available for running programs created on other CNCs on the
ProtoTRAK and vice versa.
See section 13.9 for instructions on using converters.
If the converter you want is not active you may purchase it easily. Converters are
software options so it is simply a matter of entering the correct Activation Password
into the ProtoTRAK.
To obtain the Password, see the instructions in section 3.1.8 below.
3.1.7 TRAKing/Electronic Handwheels Option
The TRAKing/Electronic Handwheels Option extends the power of the ProtoTRAK SMX
CNC beyond the ordinary by combining the electronic handwheels with software
routines in the DRO and RUN Modes. If you did not buy this option with the original
machine, you may add it later.
The option includes:
Electronic Handwheels on X and Y (replaces the mechanical handwheels, see Section
3.4.1).
TRAKing of programs during program run (see Section 12.5)
Go To Dimensions (see Section 6.6)
Selectable Fine/Coarse handwheel resolution (see Section 3.4.1)
If you order this option, do not activate the software for the TRAKing/Electronic
Handwheels Option until the electronic handwheels are installed on the machine.
Contact XYZ Machine Tools on 01823 674200 or contact your Area Sales Manager to
make arrangements for an authorized technician to install the electronic handwheels.
For three-axis CNC models, the Go To dimensions for the Z axis are a part of the base
product even if this option is not ordered. You do not need this option for Z-axis Go
To dimensions.
3.1.8 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 SMX CNC.
Software Options are not free. You may call XYZ Machine Tools on 01823 674200 or
contact your Area Sales Manager for a price quotation.
1. We recommend that you install the latest version of the ProtoTRAK SMX
master software before installing the newest option.
2. Go to the ProtoTRAK SMX 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 (for example, “A: Advanced Features”)
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 XYZ Machine Tools on 01823 674200 or contact your Area Sales Manager
with your purchase order number and the numbers you wrote down in step 4
above.
Page 20
16
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
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
3.2.1 Front
Figure 3.2.1 The ProtoTRAK SMX CNC front panel
Keyboard Hard Keys
Feed Keys:
GO: initiates motion in Run. The green LED on the GO key will be lit when the
servomotors are moving the machine either in jog or when the program run has
been initiated by the GO key.
STOP: halts motion during Run. The red LED on the STOP key will be lit when
the servos motors are not moving the machine.
Override Keys:
F/S: selects the function for the override operation. F is for feedrate. When the
LED above the F is lit, arrow presses will increase or decrease axis feedrate. S is
for spindle RPM. When the LED above the S is lit, arrow presses will increase or
decrease the spindle RPM. Note: the spindle override is active only when the
Programmable Electronic Head Option is installed.
Page 21
17
XYZ Machine Tools Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
: Feedrate Override to increase feedrate or spindle rpm up to 150%.
: Feedrate Override to decrease feedrate or spindle rpm down to 10%.
Each button push Modifies the feedrate in 10% increments and the spindle speed
in 5% increments.
ACCESSORY: When the switch is in the On position, the flood coolant pump (or
spray coolant) will come on and stay on during machining operations. In the
Auto mode, the coolant pump or spray coolant will be controlled as programmed
by the Auxiliary functions. To get to the Auto operation, press and hold the
Accessory key. If neither light is on, the coolant pump or spray coolant will not
operate.
F/C: Selects between fine and course resolution for the X and Y handwheels
when the TRAKing/Electronic Handwheels Option is installed. The LED above the
letter indicates which feed is active. Fine feed moves the axis 5mm (.200 inches)
per revolution. Course feed moves 20mm (.800 inches) per revolution.
INC SET: loads incremental dimensions and general data
ABS SET: loads absolute dimensions and general data
INC/ABS: switches all or one axis from incremental to absolute or absolute to incremental
IN/MM: causes Inch to Metric or Metric to Inch conversion of displayed data
LOOK: part graphics in Program mode
X, Y, Z: selects axis for subsequent commands
RESTORE: clears an entry, aborts a keying procedure
0-9, +/-, . : inputs numeric data with floating point format. Data is automatically +
unless +/- key is pressed. All input data is automatically rounded to the system's
resolution.
MODE: to change from one mode of operation to another
SYS: To shut down the ProtoTRAK SMX CNC, change from 2-axis to 3-axis, or
3-axis to 2-axis operation, and other functions.
: reinstates a window
: eliminates a window
HELP: displays 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.
Soft Keys:
Beneath the display are 8 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 there is no program in the current memory, the EDIT Mode softkey
will be grayed out because there is no program to edit.
Page 22
18
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Emergency Stop Switch
FIGURE 3.2.2 The ProtoTRAK SMX CNC left side with connectors labeled
The emergency stop (E-stop) switch kills all power to the spindle and ProtoTRAK's
servomotors. The computer and pendant remain powered. If the Emergency Stop switch is
pushed, it will be necessary to press the Reset Button on the right side of the pendant (see
Section 3.2.3 below) to reenergize the relay.
The Liquid Crystal Display (LCD)
The display of the ProtoTRAK SMX CNC is a 10.4" active-matrix color LCD. The very top is
the Status Line that shows the overall status of the ProtoTRAK SMX CNC. This includes the
current Mode, the current program part number, the current tool number, 2 or 3-axis mode
and 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.
3.2.2 Pendant Left Side (See Figure 3.2.2)
Page 23
19
XYZ Machine Tools Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
3.2.3 Pendant Right Side (See Figure 3.2.3)
FIGURE 3.2.3 The ProtoTRAK SMX CNC right side
Page 24
20
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Pendant Right Side with USB Ports
Keyboard P/S2 port. This port is for the keyboard only. If this port is used, the connection
must be made before the ProtoTRAK is turned on. If the ProtoTRAK is already on, it will not
recognize the keyboard until it is rebooted with the keyboard plugged in. You may also plug
the keyboard into one of the USB ports.
USB Ports. The USB ports are the only ports available for plugging in a mouse. They may
also be used for a keyboard or for plugging in the USB Thumb Drive flash memory. Items
used by USB ports will be recognized even if they are plugged in after the ProtoTRAK is
turned on.
If you need more than two USB ports, we recommend that you install a USB hub.
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.
Drivers for most major brands of mouse and keyboard are already in the ProtoTRAK SMX. If
a mouse or keyboard is not recognized by the ProtoTRAK, it means that the driver is not
Page 25
21
XYZ Machine Tools Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
available. Loading a new driver is not difficult for a qualified computer administrator who can
access the start menu on the ProtoTRAK with a keyboard plugged in (see the Catch 22?).
However, most users would be happier to simply go get a keyboard and mouse that are
already supported. We recommend Microsoft, Logitech and Belkin brand products.
AC on/off. The ProtoTRAK should be shut down properly before turning off (Sections 4.1
and 4.2).
Reset. The reset button re-energizes the relay that is tripped when the E-Stop button is
pressed. To reset the system after an E-Stop press, first reset the E-Stop button by rotating
it until it returns to its out position. After the E-Stop is reset, press and release the Reset
button on the right side of the pendant.
3.3 Mill Specifications
(See Figures 3.3.1 and 3.3.2)
Note: Machine shown above is in the two-axis CNC configuration.
Page 26
22
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
SMX 1500 SMX2
2-Axis CNC,
3-Axis DRO
SMX 2000 SMX2
2-Axis CNC,
3-Axis DRO
SMX 3000 SMX2
2-Axis CNC,
3-Axis DRO
SMX SLV SMX2
2-Axis CNC,
3-Axis DRO
SMX1500 SMX3
3-Axis CNC,
3-Axis DRO
SMX2000 SMX3
3-Axis CNC,
3-Axis DRO
SMX3000 SMX3
3-Axis CNC,
3-Axis DRO
SMX SLV SMX3
3-Axis CNC,
3-Axis DRO
Table Size
1066 x 228
1270 x 254
1371 x 305
1473 x 305
T-Slots 3 3 3 3
Table Travel
660
762
813
1016
Saddle Travel
330
406
431
431
Knee Travel
406
406
406
406
Ram Travel
330
450
450
450
FIGURE 3.3.2 The XYZ Turret Mill back view
Two- and three-axis CNC Turret Mill Specifications
Page 27
23
XYZ Machine Tools Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Maximum Quill Travel,
2-axis CNC
127
127
127
127
Maximum Quill Travel,
3-axis CNC
115
115
115
115
Quill Diameter
86
86
105
105
Spindle Taper
R8
R8
40 ISO
40 ISO
Spindle Speed
75 - 4200
75 - 4200
70 – 3600
70 - 3600
Head Tilt fore & aft
45 - 45
45 - 45
45 – 45
45 - 45
Head Tilt left - right
90 - 90
90 - 90
90 - 90
90 - 90
Spindle Motor Power
3 HP
3 HP
5 HP
5 HP
Power requirements,
machine
16 Amp
16 Amp
20 Amp
20 Amp
Maximum Weight on
Table
350 Kg
350 Kg
550 Kg
580 Kg
Machine Weight
1100 Kg
1250 Kg
1650 Kg
1850 Kg
Machine dims l, w, h
3220 x 2520 x
2200
3220 x 2580 x
2180
3670 x 2690 x
2340
4000 x 2690 x
2340
Max rapid feed X,Y
2500
2500
2500
3800
Max rapid feed, Z CNC
2500
2500
2500
2500
Way surface type
Hard chrome V
way
Hard chrome V
way
Hardened Box
way
Hardened Box
Way
CAUTION!
Failure to properly lubricate the mill will result in the premature failure of bearings and sliding surfaces.
CAUTION!
Failure to manually activate the pump at the beginning of each day, or allowing the Auto Lube to run
dry may cause severe damage to the mill’s way surfaces and ballscrews.
Precision 7207 CP4 spindle bearings
Chrome hardened and ground quill
Meehanite castings
Slide ways are Turcite coated
Wide way surfaces are hardened and ground
3.4 Auto Lubrication System
The way and ballscrew lubrication are supplied by a pump located on the side of the
machine body. The interval and discharge time of the pump are set by XYZ Machine
Tools and should not be changed or altered otherwise your warranty will become
invalid.
After periods of non-operation of the machine we recommended that before you
operate the machine you first press the pump button located on the pump itself. This
will ensure that adequate lubrication is supplied to key parts of the machine before
you start .
Factory Default Values
Interval Time – 50 min
Discharge Time – 5 sec
Discharge Pressure – Approximately 100 – 150psi
Page 28
24
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Head Lubrication
Once Each Week:
1. Fill the oil cup on the front of the head with ISO 32 oil. This oil lubricates the
Hi/Lo range shifter.
2. Fill the ball oiler located in the front lower right corner of the speed hanger
housing. This oil lubricates the speed changer shaft.
3. Extend the quill fully and apply a coating of ISO 32 oil to the outside diameter of
the quill.
Every Four Months:
Apply a good grade of general-purpose grease through the grease fittings on the
back of the head and on the left side of the head. The grease lubricates the low
range gear set and the feed change gears respectively.
3.5 Servo Motors
The servo motors on the table and saddle are 2 newton-meters of torque.
Integrated into each motor is an encoder with 0.000924mm underlying resolution for
models 1500, 2000 and 3000 and .00075mm for model SLV.
3.6 Ballscrews
Precision ground ballscrews are installed in the table and saddle to ensure smooth
traverse and positive control for manual and CNC machining.
3.7 Electrical Cabinet
XYZ Turret Mills require a 415V power supply into the electrical cabinet.
3.8 Z Axis Feedback Scale
For two-axis CNC models, a Z-axis feedback scale is mounted either to the quill or the
knee in order to provide digital readout of the Z axis position.
3.9 Auxiliary Functions (Three-Axis CNC Models Only)
Auxiliary functions are controlled through the ProtoTRAK SMX CNC either in the
program or with the accessory key on the front panel. The Auxiliary functions
consist of the following:
Spindle off command.
An air solenoid to control spray coolant or other pneumatically activated
peripheral equipment. Shop air should not exceed 125 psi.
Switched and fused 120 VAC 8 Amp outlet for coolant pumps, automatic oilers,
etc.
INPUT/OUTPUT to interface with programmable indexers, dividing heads, etc.
o Output from ProtoTRAK SMX CNC is .3-second actuation of a solid-state
relay between pin 3 (plus), and pin 4 (minus).
o Input to the ProtoTRAK SMX CNC is .3-second actuation of a solid-state
relay between pin 1 (plus), and pin 2 (minus).
o Note: Pin 1 is on top, 2 on right, 3 on left, 4 on bottom.
Page 29
25
XYZ Machine Tools Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
3.10 Work Light
An halogen work light is supplied with the machine. It mounts to the left side
(facing) of the column and plugs into a 110v outlet in the electrical cabinet.
3.11 Coolant Pump
The coolant pump is mounted in the back of the machine column. It is plugged into
the electrical cabinet and is configured to operate as commanded by the accessory
key.
3.12 Chip Pan
The Chip Pan fits around the base of the mill to collect coolant and chips.
3.13 Table Guard
The Table guard provides an enclosed workspace mounted on the table. The doors
are switched to prevent the machine spindle starting in any mode if they are open. It
also prevents the operation of the CNC in Run mode with the door open. While it
will aid in the control of chips and coolant, it is not a full, waterproof enclosure.
Removal of these guards is prohibited by law. They are fitted for the benefit of the
machine operator and to comply with the current legislation, removal means you are
breaking the law.
3.14 Z-Axis Ballscrew and Motor Assembly
For three-axis CNC models, a Z-axis ballscrew and motor assembly is mounted on the
head using two tramming bolts and the fine feed boss.
In manual and CNC operations, the quill is moved by a servo motor connected by a
belt to a ballscrew. The ball nut of the ballscrew is attached to fork that engages the
quill in the threaded hole previously used by the quill stop knob.
In CNC operations, the motor is controlled by the CNC program.
In manual operations, the motor is controlled by jog commands from the user and by
the operation of the electronic handwheel.
A limit switch in the assembly prevents damage from over travel. Z-axis traverse is
limited to 115mm.
3.15 Limit Switches
Limit switches are mounted for the saddle and table travel.
3.16 Optional Equipment
3.16.1 Electronic Handwheels
When ordered as part of the TRAKing/Electronic Handwheels Option (see Section
3.1.7) the electronic handwheels replace the standard mechanical handwheels for
table and saddle traverse. The electronic handwheels will operate when the
ProtoTRAK SMX CNC is in a Mode where the machinist controls the motion of the
table and saddle. This includes the DRO Mode, the Set-Up Mode and the TRAKing
operation in the Run Mode. The electronic handwheels will not operate during other
functions, such as when the “Select a Mode” message appears on the screen.
Handwheel resolution is determined by the F/C key on the display. Fine feed moves
5mm (0.200 inches) per revolution, Course feed moves 20mm (0.800 inches) per
revolution.
Page 30
26
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
3.16.2 Linear Scales
The ProtoTRAK SMX CNC may be configured to run either with or without Linear
Scales for X and Y travel. Linear scales have a feedback resolution of 5 Microns.
3.16.3 Power Draw Bar
A manual draw bar comes standard with the machine. A power draw bar option may
be ordered. For the SMX 3000, and SMX SLV machines, the draw bar included in the
option may be M16 or 5/8 UNC.
The standard type of power draw bar is of the appropriate length to fit tool holders
that have a threaded tang on the top ( ISO 40). BT40 and CAT 40 tool holders have
a different arrangement at the small tapered end so a longer drawbar is required to
thread into the tool holder when the retention knob is removed. These longer
drawbars can be provided on request please talk to your Area Sales Manager or XYZ
Machine Tools parts department.
3.16.4 Remote Stop Go Switch
For the convenience of operation while running the program, a Remote Stop/Go
switch may be purchased. This switch is on a ten-foot cable and operates like the
FEED Stop and Go keys on the display.
Page 31
27
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
4.0 Basic Operation
FIGURE 4.1.1 The main “select a mode” screen. Shown here, the Edit and Run Modes are grayed out
because there is no program in current memory
The ProtoTRAK SMX CNC combines the simplicity and flexibility of using a knee mill with the
easy, natural user interface that makes the ProtoTRAK the top brand in CNCs for small lot
machining.
4.1 ProtoTRAK SMX Basic Operation.
Most of the operations of the ProtoTRAK SMX CNC are organized in Modes. Modes are logical
groups of activities that naturally belong together. This eliminates the need to memorize
operations – just select a mode and choose among the soft keys.
Most operations will be discussed within the section that treats the particular mode later in
this manual. The operations described in this section either don’t fit in a particular mode, or
they are relevant to more than one mode.
4.1.1 Switching on the ProtoTRAK SMX CNC
To turn the ProtoTRAK SMX CNC on, move the toggle switch on the display side panel to the Up position.
The Windows operating system and the ProtoTRAK SMX 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 SMX CNC Select Mode screen will appear.
Select the Mode of operation by pressing the soft key beneath the labeled box. Notice that
the EDIT and RUN soft keys are grayed out when the system is first turned on. They will not
function because there is no program in the ProtoTRAK SMX CNC. Once a program is
entered, the EDIT key will function. Once a program is entered and the necessary SET-UP
operations are complete, the RUN key will function.
Page 32
28
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
FIGURE 4.1.4 You will see this screen when the SYS hard key is pressed. The choice
“GO TO 2 AXIS” shows that the CNC is currently in 3-Axis operation.
If the machine has been shut off since the last time the ProtoTRAK SMX was on, you will have
to press the green E-Stop Reset button on the right side of the ProtoTRAK display pendant
before using operations that involve the servo motors.
The ProtoTRAK SMX CNC has a screen saver already programmed in. If the system is not
used (either by a key stroke or by counting) for 20 continuous minutes, the display will turn
itself off. The LED’s on the keypad will flash every few seconds to indicate that the system is
still on. Press any key or move any axis to bring the screen back to its previous display. The
key you press will be ignored except to turn the screen on.
4.1.2 Shutting Down the ProtoTRAK SMX CNC
Important: the system must be turned off properly. First press the SYS hard key
and then press the SHUT DOWN soft key (see Figure 4.6). After a few seconds, you
will see the message "it is now safe to turn off your computer". Turn the ProtoTRAK
SMX CNC off by moving the toggle switch on the display side panel to the down
position.
Note: When you turn the PROTOTRAK SMX CNC off, always wait a few seconds before turning it back
on.
4.1.3 Emergency Stop
Press the button to shut off power to the spindle motor and axis motors. Rotate the
switch to release. Once the switch is released, you must reset the relay by pressing
the green button on the right side of the ProtoTRAK SMX pendant (figure 3.2.3).
4.1.4 Switching Between Two and Three-Axis Operation
For three-axis XYZ Turret Mill models, The ProtoTRAK SMX CNC may be operated as a
two or three-axis CNC. Press the SYS hard key. Softkey F2 will read GO TO 2 AXIS
when the ProtoTRAK SMX CNC is currently operating in three axis and it will say GO
TO 3 AXIS when the ProtoTRAK SMX CNC is currently operating in two axis. See
Figure 4.1.4.
4.1.5 Coolant Pump
Your mill is supplied with a coolant pump. If you do not have the Auxiliary Functions
active (they are active for the three-axis models only) the coolant pump is operated
by the Accessory key on the ProtoTRAK SMX front panel. If you do have the Auxiliary
Page 33
29
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
FIGURE 4.1.6.1 The first Math Helps screen. Choose among the alternatives based on the
information you need to calculate
Functions, the operation of the coolant system may be programmed within the
program events. With the Auxiliary Functions set-up, manual control of the coolant
system is through the Accessory key on the front panel of the SMX CNC.
Use of the ACCESSORY hard key:
ON - will turn on the coolant pump until you turn it off.
AUTO - will turn on the coolant pump as programmed into events for three-axis
models; will turn on the coolant pump when the machine is feeding for two-axis
models.
Off (no light) - the coolant pump stays off.
4.1.6 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.
Math Helps
When the blue question mark does not appear, pressing HELP will initiate the Math
Helps.
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.
Page 34
30
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
FIGURE 4.1.6.2 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 Z beginning.
Load End: will load the displayed solution into the event as the X and Z end.
Load Center: will load the displayed solution into the event as the X and Z 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.
4.1.7 Windows Up or Down
Some of the selections in the ProtoTRAK SMX CNC will cause a window to appear
with a message. To eliminate the window in order to see what is behind it, press the
hard key. To restore the window, press the hard key.
4.1.8 Turning Options On and Off
If the Advanced Features Option and Networking/Memory Options have been
installed, you may run the ProtoTRAK SMX with them turned off. This has the benefit
of making the system easier to use.
To turn the options on or off, press the SYS hard key. You will get the screen shown
in Figure 4.1.4 above. Press the Options On/Off softkey. This will take you directly to
the screen that will allow you to turn options on and off. You can also get to this
screen using Service Code 334.
Page 35
31
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
The Programmable E-Head Option and TRAKing/Electronic Handwheel Option may
not be turned on or off. If they are installed, they must remain active.
4.2 Machine Operation
This section covers the operation of the XYZ Turret Mills. If you purchased your
ProtoTRAK SMX CNC as a retrofit, please refer to the user manual that came with
your machine.
4.2.1 Spindle On/Off, Forward/Reverse
The spindle switch is located to the left of the SMX display.
Turn the Spindle switch to left to 1 for forward (clockwise) spindle rotation if the
Hi-Lo-Neutral lever is in the low position.
Turn the Spindle switch right to 2 for forward (clockwise) spindle rotation if the
Hi-Lo-Neutral lever is in the high position.
Turn the Spindle switch straight ahead for off.
Page 36
32
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
Figure 4.2.0 XYZ SMX 1500 Mill head front view. Shown without the standard quill glass
scale.
Page 37
33
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
CAUTION!
Do not run ProtoTRAK SM program unless the table and saddle clamps are free .
4.2.2 Table, Saddle, Knee/Clamps
The table clamps are located on the front of the saddle. Rotate them clockwise until
snug--overtightening is not necessary.
The saddle clamp is located on the left side of the saddle. Pull forward to clamp the
table until snug--overtightening is not necessary.
The knee clamps are located on the left side of the knee for the K2 and K3
mills, and on the right side for the K4.
4.2.3 Raising/Lowering the Knee
For models 1500 and 2000, the knee is raised and lowered using the hand crank
located on the left front of the knee. Clockwise rotation moves the knee up, while
counterclockwise rotation moves the knee down.
For models 3000 and SLV, the knee is raised by the power rise/fall. Turn the button
located on the switch box to the left of the SMX display. A clockwise turn raises the
table a counterclockwise turn lowers it.
Be sure the knee is unclamped before raising or lowering.
4.2.4 Spindle Brake
A pneumatic air cylinder activates an automatic spindle brake when the spindle motor
is turned off. The brake disengages when the spindle is started.
4.2.5 Draw Bar
The draw bar holds the R8 or #40 ISO tool holders into the spindle taper. The bar
has a 5/8-unc right hand thread and should be tightened with a 23mm wrench from
the top of the head. When tightening, it is necessary to activate the spindle brake
(See 4.2.4 above). If the tool holder does not release from the spindle, lightly tap on
the top of the bar to dislodge the tool.
4.2.6 High-Low-Neutral Level
For both the standard head and the Programmable Electronic Head Option, the range
selection is made through the High-Low-Neutral Lever.
Figure 4.2.6
Page 38
34
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
CAUTION!
Never attempt to change the range selection through the High-Low-Neutral lever when the
spindle is rotating. Be certain the spindle ON/OFF switch is in the Off position
.
CAUTION!
Do not rotate the variable speed crank when the spindle is stationary.
i00166
Rotate the spindle by hand to help engage the lever into the high or low position.
Note: Shifting from the high to low range, or low to high range changes the direction of
rotation for the On/Off switch (See Section 4.2.1).
4.2.7 Speed Changes
For the standard vari-speed head, spindle speed may be varied by rotating the
variable speed crank. When the Programmable Electronic Head Option is installed,
the spindle speed is controlled by the ProtoTRAK SMX CNC. See the instructions in
the Program Mode, DRO Mode and Run Mode.
4.2.8 Operating the Quill
For two-axis CNC models, the quill may be moved up and down through its range
with the quill feed handle. The quill may be locked into position by rotating the quill
lock clockwise. Pull the handle out slightly to rotate it freely to a new position.
For three-axis CNC models, the quill is operated by the electronic handwheel mounted
on the side of the Z Ballscrew and Motor Encoder.
Note: sections 4.2.9 through 4.2.15 refer to two-axis CNC models.
4.2.9 Adjusting the Quill Stop (Two-Axis CNC Models)
The quill stop may be adjusted by rotating the micrometer dial nut. It is locked in
place with the knurled nut.
4.2.10 Power Feed Engagement Lever (Two-Axis CNC Models)
Figure 4.2.10
The power feed is engaged or disengaged with this selector. Pull out the knob and rotate it
clockwise to disengage power feed. Rotate it counterclockwise to engage power feed.
Page 39
35
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
CAUTION!
It is recommended that the selector be disengaged when the spindle is not running. Never
have the feed engaged when the spindle RPM is over 3000. Always leave the selector in the
disengaged position unless the feed function is being used.
Figure 4.2.10.2
i00166
4.2.11 Fine Feed Direction Shaft (Two-Axis CNC Models)
The direction of the fine feed is set by the position of the fine feed direction shaft. IN
sets the direction down, OUT sets the direction up, and NEUTRAL in the middle.
Page 40
36
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
Figure 4.2.10.3 Quill Feed Selector one model
Figure 4.2.10.4 Quill Feed Selector one model
4.2.12 Quill Feed Selector (Two-Axis CNC Models)
This selector is used to set the quill feed speed.
To change speeds, pull the knob out and rotate the selector to the proper position. It is
generally easier to change speeds with the spindle running or rotated by hand. Do not
force the lever.
4.2.13 Feed Trip Lever (Two-Axis CNC Models)
The Feed Trip Lever stops the quill feed motion when the quill stop knob reaches the
quill micrometer dial.
Move the lever to the left to engage, or to the right to disengage.
4.2.15 Fine Automatic Quill Feed (Two-Axis CNC Models)
1. Be certain the quill lock is off.
2. Set the quill micrometer dial to the proper depth.
3. Engage the Power Feed Engagement lever when the motor is stopped.
4. Select proper quill feed (see above).
4.2.16 Setting Stops for Three-Axis CNC Models
When the Z-axis ballscrew and motor assembly is installed for three-axis CNC
operation, the quill stop mechanism is not available. Instead, there are convenient
inputs in the DRO Mode and the Run Mode for setting quill stops.
Page 41
37
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
5.0 Definitions, Terms & Concepts
FIGURE 5.1 ProtoTRAK SMX CNC conventions
5.1 ProtoTRAK SMX CNC Axis Conventions
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.
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 & Tool Path Programming
The ProtoTRAK SMX CNC gives you ultimate flexibility in programming. Programs
that are entered through the ProtoTRAK SMX CNC system can be entered as either
Part Geometry or Tool Path (optional).
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 SMX 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:
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 SMX 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.
_________________________________________________________________
Page 42
38
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Note: Tool Path programming is part of the Advanced Features Option.
FIGURE 5.4 Each point has both an absolute and an incremental reference in the X axis. The
ProtoTRAK SMX CNC allows you to program using either.
FIGURE 5.3 Vertical Planes
Programs generated by CAD/CAM systems are always generated as Tool Path programs and
are run as such even if the Advanced Features Option has is not active on the ProtoTRAK SMX
CNC.
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). Programming vertical planes requires the Advanced Features Option (Section
3.1.2).
Unlike most CNC controls,
the ProtoTRAK SMX CNC can
machine arcs in any vertical
plane rather than just XZ or YZ.
5.4 Absolute & Incremental Reference
The ProtoTRAK SMX 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:
5.5 Referenced & Non-Referenced Data
Data is always loaded into the ProtoTRAK SMX 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
Page 43
39
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
or ABS SET key. This manual uses the term SET when either INC SET or ABS SET
FIGURE 5.7.1 Examples of tool right
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
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. Helix programming
requires the Advanced Features Option.
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
specificevents above for the last event that is programmed. A.G.E. Profile
Programming requires the Advanced Features Option.
For example, if an ARC event followed a MILL event, a 50mm incremental X BEG
would mean that in the X direction the beginning of the ARC event is 50mm 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 SMX 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.
Page 44
40
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
FIGURE 5.8.1 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
FIGURE 5.7.2 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.
5.8 Tool Diameter Compensation when Contouring in Z
with Part Geometry
Note: Z contouring requires the Advanced Features Option (Section 3.1.2)
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 the Part Geometry option is selected. There is no Z-axis up tool
offset applied when the Tool Path option is selected.
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.
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.
Page 45
41
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
FIGURE 5.8.2 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
FIGURE 5.10.1 A Conrad is added between the two intersecting lines
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).
5.10 Conrad
Conrad is a unique feature of the PROTOTRAK SMX 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.
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 SMX CNC will ignore
the Conrad.
Page 46
42
XYZ Machine Tools, Ltd.
XYZ Turret Mill & ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
For the figure below, you program an Arc event from X1, Z1 to X2, Z2, and a Mill to X3, Z3.
FIGURE 5.10.2 A Conrad is added between an arc and a line
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.
5.11 Memory & 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 SMX 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.
Storage of programs can be done on a USB device or on a disk in the floppy drive.
We strongly recommend you habitually back up programs.
When the Network Option is purchased, program storage can also be saved to an
offline computer that is networked to your SMX CNC.
Page 47
43
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
FIGURE 6.1 The DRO screen
6.0 DRO Mode
The ProtoTRAK SMX CNC operates in DRO Mode as a sophisticated 3-axis digital readout with
jog and power feed capability.
6.1 Enter DRO Mode
Press MODE, select DRO soft key. The screen will show:
Note the RETURN soft key is lit when in Jog or Power Feed operation.
6.2 DRO Functions
Clear Entry: Press RESTORE, then re-enter all keys.
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.
Note: This will also reset the incremental dimension 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.
Page 48
44
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
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.
6.3 Jog
The servomotors can be used to jog the table, saddle and ram.
a. Press the JOG soft key.
b. A flashing message will appear saying "CAUTION: JOG KEYS ARE ACTIVE".
c. To jog, press the X, Y or Z hard keys.
d. To stop jogging, release the key.
e. The speed of jog is displayed in the box next to the words "Feed Rate” on the
lower left side of the LCD screen.
f. Press the +/- hard key to reverse direction. When the number in the Feed rate
box is negative, this indicates the minus direction.
g. Press the RATE keys to reduce and to increase the jog speed in 10
percent increments. The changes in speed may be seen in the Feed rate box
and on the green feed rate indicator. The amount of override is displayed in
the Override box.
h. To jog at a certain rate, simply enter that number as inches or mm per minute and
then press the X, Y or Z key. You may also use the override key to adjust this
number. Press RSTR to return to 150 ipm or 3800mm/min.
i. Press RETURN soft key to return to manual DRO operation.
6.4 Power Feed
The servomotors can be used as a power feed for the table, saddle or quill, 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 50mm of the table in the negative direction, you
would enter: X, 50, +/-, INC SET.
d. Initiate the power feed move by pressing GO.
e. The feedrate is automatically set to 254 mm per min (or 10 ipm). Press FEED
or FEED to adjust the feedrate from 254 to 2540 mmpm. (or 1 ipm to 100
ipm)
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.
6.5 Do One
The Do One routines in the DRO mode allow you to do one CNC operation while
machining manually without having to write a program.
The programming and tool path of the events in Do One are nearly identical to those
in the Program Mode. See Section 8 for instructions for programming.
Page 49
45
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
6.6 Go To (TRAKing/Electronic Handwheels Option)
The Go To function in the DRO mode allows you to set a dimension in X, Y or Z at
which you want the machine to stop moving when you are cranking manually. For
example, if you wanted to machine manually exactly 5omm of table motion, you
would input: Go To, X, 50, Inc Set. While the Go To window is displayed, the
ProtoTRAK SMX will not let you pass that 50mm dimension you set.
a. Press the Go To key.
b. Enter the axis, X, Y, Z or any combination. Input the dimension(s).
c. Press Inc Set or Abs Set.
d. Crank the handwheel. Motion will stop at the entered dimension even if you
continue to crank the handwheel.
6.6.1 Go To for Three-Axis CNC Models
Whether or not the TRAKing/Electronic Handwheels Option is active, XYZ Turret Mills
with the Z-axis ballscrew and motor assembly installed for three-axis CNC will have
this feature enabled for manual quill operation. Simply follow the instructions above.
If the TRAKing/Electronic Handwheels Option is not active, only the Z will be available
for setting a Go To dimension.
6.7 Teach
Teach gives you the ability to enter X and Y dimensions into a program. It can be a
useful way of entering a few manual moves for operations like clearing out excess
material or remembering a few hole locations.
The process of using Teach is in two parts. The first part takes place in the DRO
Mode. This is where you start the Teach program, establish the program events and
enter the X and Y dimensions. The second part is in the Program Mode. This is
where you complete the Teach events that you began in the DRO Mode by entering
the rest of the data. Once the data is entered, the Teach events become just like the
other events that make up a program.
6.7.1 Entering Teach Data
From the DRO screen, press Teach.
On the top of the screen, you will see the message "Teach" and an event counter.
When you enter Teach, you are actually programming events. If there is already a
program in current memory, Teaching will add events to the end of the program. If
there is not already a program in current memory, Teaching will start a new program.
For example, if you already had a program in current memory that had 10 events,
when you press Teach, the event counter will say EVENT 11. If there was no
program, the event counter will say EVENT 1.
The event counter shows the event for which data is being entered. You may teach
in position, drill and mill events only.
On the first Teach screen, the softkeys are:
POSN: a position move. For two-axis programming, the POSN and DRILL events are
combined.
DRILL: a drill or bore.
MILL BEGIN: the beginning of a straight line or MILL event.
END TEACH: ends the teaching process and returns you to the main DRO screen.
Page 50
46
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Safety, Programming, Operating & Care Manual
If you press the POSN or DRILL key, the event counter will go up by one and the
screen remains the same. If you press the MILL BEGIN key, the event counter stays
on the same number. That is because you have given the beginning point of the line
but not yet the end. The softkey selections will change to:
MILL END: the last point of the Mill event. Press this to end the Mill event and select
a POSN, DRILL or new MILL event.
MILL CONT: the last point of the current Mill event, but the beginning of the next
Mill event. You may enter successive Mill events by pressing the MILL CONT key.
Pressing either of the above softkeys will cause the event counter to increase by one.
At any time you may exit the Teach and return to the DRO screen. The events you have
defined with their X and Y dimensions are finished in the Program Mode. See Section 8.14.
6.8 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 servos will turn on, move the
quill to Z retract (for three-axis CNC models) then move the table at rapid speed to
your X and Y absolute zero position, and then turn off. You will be at zero and in
manual DRO operation.
6.9 Tool #
The ProtoTRAK SMX CNC allows you to use the data for tools in your Tool Table (see
Section 11.1) in the DRO Mode. To change tools, press the TOOL # soft key and enter
the tool number when prompted by the Data Input Line.
Even when you set up a tool in the Set-Up Mode, if you do not wish to use the tools in
the Tool Table, simply ignore the Tool # feature.
Page 51
47
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
FIGURE 7.2 The Program Mode header screen. Most selections above
relate to the Advanced Features Option. If your screen shows only
Program Name and Dwell, The Advanced Features Option is not active.
7.0 Program Mode
Getting Started & Some General Information
7.1 Programming Overview
The ProtoTRAK SMX 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 SMX CNC will allow only one program in current memory. To write a
new program, you must first erase the one in current memory (you may want to first
store the program for use in the future). If there is already a program in current
memory, entering the Program mode will allow you to edit or add to that program.
Page 52
48
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
FIGURE 7.3 Pressing the Help hard key when the Program Name is highlighted calls up alpha keys
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 summarized in the program as "Event 0".
7.3.1 Program Name
Programs written on the ProtoTRAK SMX CNC are usually named for the part that is
to be machined. When programs (or files) are named using the ProtoTRAK SMX CNC,
the name can be up to 20 characters long. Programs imported into the ProtoTRAK
SMX CNC may be longer. While 20 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. 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 SMX
CNC.
Use a keyboard plugged into the ProtoTRAK SMX CNC to name the program.
To use the alpha keys and special characters on the ProtoTRAK SMX 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.
Page 53
49
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
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 SMX CNC that you are finished with the alpha
table. Numbers may still be added to the program name.
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 DATA FWD softkey to select general programming options. See Section 3.1.2
for more information about the Advanced Features Option.
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. This function is part of the Advanced Features Option.
Dwell Request: For three-axis CNC machining only. 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.
Auxiliary Function Request: Asks if you wish to activate any of the optional
auxiliary functions (see Section 7.4) at any time during the program. Select the
appropriate YES or NO soft key. If you select YES you will be prompted to input the
type and sequencing of the auxiliary functions during event programming. Auxiliary
Functions are optional for three-axis CNC models only.
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. Turn and A.G.E. Arc event. This function is part of the Advanced
Features Option.
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.
Multiple Fixtures: Asks you if you wish to turn on the multiple fixtures offset.
Answering Yes will cause a prompt to appear at each event asking which fixture the
event was referenced from. If you select Yes, the Data Input Line will ask you to
enter a fixture default number from one to six. The fixture default number is the
fixture that will be applied to all the events in current memory when Multiple Fixtures
is turned on or when a new event is programmed without another event being
specified. Enter the default fixture, or leave the number unchanged, and press SET.
Multiple Fixtures are explained more fully in Section 7.5. This function is part of the
Advanced Features Option.
Dimension Definition: The ProtoTRAK SMX 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.
Page 54
50
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
Input:
Function
Comments
0
None
No Auxiliary functions will begin when this event begins to run.
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 SMX 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. Tool Path programming is part of
the Advanced Features Option.
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.
DATA FWD: moves the highlight forward through the programming options without
setting an input into the program.
DATA BACK: moves the highlight backward through the programming options
without setting an input into the program.
GO TO BEGIN: puts the Program Header on the left side of the screen and the first
event 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, Auxiliary Function
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.
PART GEO: sets up the programming as Part Geometry.
TOOL PATH: sets up the programming as Tool Path. This function is part of the
Advanced Features Option.
7.4 Auxiliary (AUX) Functions (Three-Axis CNC Models Only)
When the Auxiliary Function Option is installed and active, the ProtoTRAK SMX CNC
can control four different auxiliary functions. You can select whether to activate or
deactivate these functions at the beginning or end of each event.
If Auxiliary Functions are selected on the program header, the system will prompt for
AUX BEG and AUX END in each event.
When running programs with Auxiliary functions, the ACCESSORY hard key on the front
panel must be in the correct position. If you want the program to automatically turn the
Auxiliary functions on and off, press the ACCESSORY key until the light is on in the AUTO
position.
AUX BEG options:
Page 55
51
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
1
Coolant/Air
The coolant pump or air solenoid will be turned on when this event begins to
run.
3
Pulse Indexer
Activates a 0.3 second electronic pulse at the beginning of the event. See
note below.
0
None
No Auxiliary functions will turn off at the end of this event.
1
Coolant/Air
Off
Turns the coolant or air solenoid off at the end of this event.
3
Pulse Indexer
Activates a 0.3 second electronic pulse at the end of this event. See note
below.
4
Spindle
Turns off the spindle at the end of this event. Note, the spindle automatically
turns off for each tool change – it is not necessary to program a spindle off.
AUX END options:
Coolant/Air on and off is automatically programmed for tool changes. If you want the
air or coolant pump on while cutting the entire part, you need only program the Aux
begin in the first event and Aux end in the last event. The coolant pump or air
solenoid will turn on at the beginning of the programmed event and will turn off
during tool changes.
The Pulse Indexer function is designed to operate with a standard indexer. Programming
an Aux 3 at the end of an event will cause the ProtoTRAK SMX CNC to stop machining at
the end of the event and wait for a signal from the indexer or rotary table that it has
finished its programmed move, then it will resume machining at the next event. If you
want the ProtoTRAK SMX CNC to return the head to the Z retract position before moving
to the next event, put the Aux 3 command in a Pause event. The ProtoTRAK SMX CNC will
interpret the signal from the indexer or rotary table as a GO command and continue
machining without you having to press the GO key.
7.5 Multiple Fixtures
This function is part of the Advanced Features Option.
You may run your program using up to six fixtures plus a base. A fixture is a location on
your machine with a defined offset from your absolute 0. When you program an event to
have a fixture, it will treat the offset as if it were absolute zero shift. The programmed X,
Y and Z absolute dimensions are relative to the absolute reference for the specified fixture.
For example, say you had two vises on the table. On the first vise, you established the
lower left jaw as the absolute 0. At the same time, you measured the distance between
the absolute zero you just established and the lower left jaw of the other vise. You
entered that measurement as an offset from your base vise (the first one) and the other
vise, which is Fixture #2. Any events that you programmed using Fixture #2 would treat
the lower left corner of that second vise like the absolute 0 for the X, Y and Z dimensions
in the events.
Fixture offsets are handy for combining different programs together to run at the
same time or to make multiple parts by repeating the events with different fixtures.
The fixture offsets are entered in the Set-up mode. There is a base fixture, called
fixture number one. We recommend that Event #1 in your program uses fixture
number one. It doesn’t have to; we just believe it is clearer that way.
7.5.1 The Default Fixture
In the program header screen, you entered a default fixture number (if you didn’t, it
assumed fixture #1 as the default fixture). If there are program events already in current
memory when you change the multiple fixture from NO to YES, they will all receive the
default fixture number automatically. When you change the default fixture number in the
program header screen from one fixture to another, all the events that had the previous
default fixture number will be changed to the new default fixture number.
If there are no program events in current memory when you change the multiple
fixture feature from NO to YES, the prompt will be added to the end of every event
Page 56
52
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
you then program. The default fixture number will be assumed if you press SET
without specifying a different number. If you do specify a different fixture number
that fixture number will become the assumed input for subsequent events when SET
is pressed.
7.5.2 Fixtures and Running the Program
To run the program, first go to the DRO mode and set absolute 0 at the base fixture,
Fixture #1.
In the Run mode, the SHOW ABS displays the absolute position relative to the fixture
in the event being run, that is, the absolute dimension that was programmed.
7.5.3 Editing Fixtures
With the Multiple Fixtures feature turned to YES, you may edit the fixture number in
the Program Mode event by event. You may also use the Search Edit feature in the
Edit Mode to change fixture numbers.
See Section 11.4 for setting up fixture offsets.
7.6 Assumed Inputs
The ProtoTRAK SMX CNC will automatically program the following when you simply
press SET (either INC SET or ABS SET):
Tool Offset: If the first event with an offset, CENTER. If not the first event with an
offset, 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.
7.7 Z Rapid Positioning (Three-Axis CNC Models)
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 57
53
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
FIGURE 7.8 Soft keys used while programming an event
FIGURE 7.9.1 The header screen has been completed and is on the left side. Select an event type
from the soft keys. Three-axis CNC events are shown.
7.8 Softkeys within Events
Once a geometry (Event) such as Mill or Bolt Hole is selected, the softkeys will
change. See Figure 7.8
PAGE FWD: moves forward through the programmed events.
PAGE BACK: moves backwards through the programmed events.
DATA FWD: moves forward through the event inputs. Note, use the DATA FWD key
and not a SET key when you do not want to input a value.
DATA BACK: moves backwards through the event inputs.
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.
7.9 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 SMX CNC, an Event is a geometry, or a feature of a
part.
Page 58
54
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
FIGURE 7.9.2 When the More soft key is selected, these additional event types are available for
three-axis CNC models. If the Advanced Features or E-Head Option are not active, relevant
functions will be grayed out.
FIGURE 7.9.3 Here, a Bolt Hole event was selected for three-axis CNC. For two-axis,
Z programming prompts do not appear. The ProtoTRAK SMX CNC is prompting you to
enter the number of holes.
When the MORE soft key is selected, the soft keys change to:
After an event type is selected from the soft keys, 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.
7.10 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 as long as you are still
programming that same event. Press the DATA BACK or DATA FWD (Forward) soft
key until the incorrect prompt and data are highlighted and shown in the conversation
line. Enter the correct number and SET. The ProtoTRAK SMX 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 (the PAGE BACK softkey will work as well).
Page 59
55
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
7.11 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 SMX 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.
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.
: shifts drawing down.
: shifts drawing up.
: shifts drawing to the left.
: shifts drawing to the right.
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.
Note: The LOOK routine does not check for programming errors. Use Tool Path in the SET
UP Mode to check movement of the tool.
7.12 Finish Cuts
The Pocket and Profile events are designed with built-in finish cut routines because
they are complete, and stand-alone pieces of geometry. Shapes machined with a
series of Mill or Arc events (either with or without A.G.E. Profile) don't have an
automatic routine for making finish cuts. There is, however, a very simple technique
that can be used.
a. Program the shape using the print dimensions, and ignore the need to leave
material for a finish cut.
b. Using a subroutine event, Repeat all the events in "a." but call out a different
tool number.
Page 60
56
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
EVENT 1
BOLT HOLE
EVENT 1
BOLT HOLE
DRILL OR BORE
# HOLES
# HOLES
X CENTER
X CENTER
Y CENTER
Y CENTER
RADIUS
Z RAPID
ANGLE
Z END
TOOL #
RADIUS
ANGLE
# PECKS FOR DRILL
Z REEDRATE
TOOL #
FIGURE 7.13 Programming a Bolt Hole. On the left, the prompts required in programming in three-axis CNC.
On the right, the prompts required for two-axis.
c. In Set-Up Mode "lie" about the tool diameter for the tool called out in events in
"a.". Input a tool diameter equal to the actual tool diameter plus 2 times the
finish cut you wish to leave. The ProtoTRAK SMX CNC will think the tool is
bigger than it really is and, therefore, shift a little further away from the
machined shape.
d. In Set-Up Mode input the actual diameter for the tool called in the Repeat
event "b". This will produce the final dimensioned cut.
7.13 Two Versus Three-Axis Programming for Three-Axis CNC
Models.
For mills with the Z-axis ballscrew and motor assembly installed, the ProtoTRAK SMX
CNC may be operated as either a two or three-axis CNC. Many jobs in tool rooms are
simply easier to do with a two-axis CNC. Other jobs are more complex or require a
lot of metal removal, so the extra programming and set-up of the three-axis is worth
the effort.
The ProtoTRAK SMX CNC lets you choose how much CNC you want to use on the job
at hand. See Section 4.6 for switching between two and three-axis operation.
Programming is very similar between the two.
In Figure 7.13 the prompts for programming a Bolt Hole in two-axis and in three-axis
are shown side by side. Note that the difference is that the three-axis requires a few
additional prompts.
For the convenience of users who have two-axis CNC models, the programming will
be explained in two different sections. If you have a three-axis CNC model, we
suggest you skip the two-axis programming section since the programming is very
similar.
Page 61
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
57
8.0 Two-Axis Program Events
This section describes the events and prompts you encounter when programming your ProtoTRAK
SMX as a two-axis CNC. If you have a three-axis XYZ Turret Mill you may want to skip this section.
Events are fully defined pieces of geometry. By programming events, you tell the ProtoTRAK
SMX 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 Set-Up Mode.
8.1 POSN DRILL:
This event type positions the table and quill 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. You would use this event type to program a hole for drilling. In program
run, the CNC will move to the dimension you program and will wait for you to press GO
before moving to the next event. You may also use this event type to position the table for
some other purpose, such as to avoid a clamp or to move off the workpiece for a tool
change.
To program a Position event press the POSN DRILL 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
Tool # is the tool number you assign. SET will use the tool number of the previous event.
8.2 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:
# 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
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.
Tool #: is the tool number you assign
8.3 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.
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
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 (that must lie in
the same plane for part geometry programming).
Page 62
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
58
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.
Feedrate: is the milling feedrate from Begin to End in in/min from .1 to 100, or
mm/min from 5 to 2540 (up to 3800 for model SLV)
Tool #: is the tool number you assign
Continue: input 1 for Yes if you want to mill continuously from this line to the next
event, input 2 for No if you want the ProtoTRAK SMX to stop at the end of the event.
8.4 ARC Events
This event allows you to mill with circular contouring any arc (fraction of a circle).
In ARC events when X Center and Y Center are programmed incrementally, they are
referenced from X End and Y End respectively. An ARC event may be programmed
with a CONRAD if it is connective with the next event.
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
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
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction of the
arc
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
XY Feedrate: is the milling feedrate from Begin to End in in/min from .1 to 100, or
mm/min from 5 to 2540 (up to 3800 for model SLV)
Tool #: is the tool number you assign
Continue: input 1 for Yes if you want to mill continuously from this line to the next
event, input 2 for No if you want the ProtoTRAK SMX to stop at the end of the event.
8.5 POCKET Event
This event selection gives you a choice between circle pocket, rectangular pocket and irregular
pocket.
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 stepover 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 stepover percentage.
The value you enter here will remain the same until you change it again.
Page 63
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
59
8.5.1 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
Radius: is the finish radius of the circle
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for
milling
Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut.
Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540 (up to
3800 for model SLV)
Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign
8.5.2 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).
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
Conrad: is the value of the tangential radius in each corner
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for
milling
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut
XY Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540
(up to 3800 for model SLV)
Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign
8.5.3 Irregular Pocket (Advanced Features Option)
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
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut
Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540 (up
to 3800 for model SLV)
Page 64
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
60
Fin Feedrate: is the finish cut milling feedrate in in/min from .1 to 100, or mm/min
from 5 to 2540 (up to 3800 for model SLV)
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 10.0.
No islands may exist in an irregular pocket.
8.5.4 Tool Path in Pocket Events
In Program Run, the ProtoTRAK SMX will first direct the cutter along a path to rough
out all the material inside of the perimeter, and then will do a rough cut along the
inside of the perimeter which leaves the amount of material programmed in the FIN
CUT prompt. This will be followed by a finish pass (if FIN CUT was not zero) along
the inside of the perimeter at the Finish Feedrate.
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 SMX
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 pocket will be machined in two or more
steps. When a step is completed, the ProtoTRAK SMX will prompt "CHECK Z" at
which time you should raise your quill out of the pocket. Press GO and the tool will
move at rapid to the beginning of the next step and then there will be a prompt for
you to "SET Z" for you to position the tool for the depth you want.
In the Set Up Mode, you may check your tool path for hidden areas. The yellow X's
show points where you will receive a prompt to move the quill. The red dashed lines
show the rapid moves.
8.5.5 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.
8.5.6 Face Mill (Advanced Features Option)
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
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.
Feedrate: is the milling feedrate in in/min from .1 to 800, or mm/min from 5 to
20320
Tool #: is the tool number you assign
Page 65
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
61
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%.
8.6 Islands (Advanced Features Option)
Islands programming is available as part of the Advanced Features Option. See
Section 3.1.2.
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 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.
8.6.1 Circular Island (Advanced Features Option)
When the Advanced Features Option is active, press the Circle Island soft key if you
wish to mill a circular island.
Prompts for the Circular Islands:
X CENTER: is the X dimension of the center of the Island.
Y CENTER: is the Y dimension of the center of the Island.
RADIUS: is the finish radius of the Island.
DIRECTION: is the milling direction, clockwise or counterclockwise.
FIN CUT ISL: Finish cut for the Island. If 0 is input, there will be no 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.
FEEDRATE: the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540
(up to 3800 for model SLV).
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts
TOOL #: is the tool number you assign.
8.6.2 Rectangular Island (Advanced Features Option)
Page 66
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
62
When the Advanced Features Option is active, 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.
CONRAD ISL: the value of the tangential radius in the corners of the island.
DIRECTION: is the milling direction, clockwise or counterclockwise
FIN CUT ISL: Finish cut for the Island. If 0 is input, there will be no 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.
FEEDRATE: the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540
(up to 3800 for model SLV).
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts
TOOL #: is the tool number you assign.
8.6.3 Irregular Island (Advanced Features Option)
When the Advanced Features Option is active, 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 pocket 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.
FIN CUT ISL: Finish cut for the Island. If 0 is input, there will be no 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.
Page 67
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
63
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.
FEEDRATE: the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540
(up to 3800 for model SLV).
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 10.0.
8.7 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.
When the irregular profile event is started the ProtoTRAK SMX CNC will automatically initiate
the powerful Auto Geometry Engine. See Section 10.0 for programming with A.G.E.
8.7.1 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.
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.
Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut.
Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540 (up to
3800 for model SLV).
Finish Feedrate: is the milling feedrate for the finish cut.
Tool #: is the tool number you assign.
8.7.2 Rectangular Profile
Press the RECTANGLE soft key if you wish to mill a rectangular frame (all corners
are 90o 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.
Conrad: is the value of the tangential radius in each corner.
Page 68
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
64
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.
Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut.
Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540 (up to
3800 for model SLV).
Fin Feedrate: is the milling feedrate for the finish cut (if programmed).
Tool #: is the tool number you assign.
8.7.3 Irregular Profile (Advanced Features Option)
When the Advanced Features Option is active, 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.
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.
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.
Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540 (up
to 3800 for model SLV).
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut.
Fin Feedrate: is the finish cut milling feedrate in in/min from .1 to 100, or mm/min
from 5 to 2540 (up to 3800 for model SLV).
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 10.0. Irregular Profile and Auto Geometry
Engine programming is part of the Advanced Features Option.
8.8 Engrave Event (Advanced Features Option)
The Engrave Event allows you to machine numbers, letters and special characters as
part of a part program. See figure 8.8 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
Page 69
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
65
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.
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 (F8) 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.
FEEDRATE: The feedrate of XYZ along the path of the text.
Tool #: is the tool number you assign.
Page 70
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
66
FIGURE 8.9.1 Holes 1-4 are mirrored across the Y
axis to 5-8, respectively, about a line X OFFSET from
X=absolute 0
FIGURE 8.8 The above figure shows the text and special characters available for the
Engrave event. 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.
8.9 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 SMX 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. 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 (Advanced Features Option) 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:
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
Page 71
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
67
not rotate another rotate event, however you can rotate a mirror event. Consider the
FIGURE 8.9.2 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
figure below:
Press the SUBROUTINE (SUB) soft key to call up the Repeat, Mirror, and Rotate options.
8.9.1 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.
# Repeats: is the number of times events are to be repeated up to 99.
% Feed: the percentage of the feeds programmed in the repeated events. 100% is
assumed.
Tool #: is the tool number you assign.
8.9.2 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.
Page 72
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
68
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.
8.9.3 Rotate
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.
8.10 COPY Events (Advanced Features Option)
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, or Rotate.
Copy is very useful. With copy you can:
Edit the events that are being repeated, mirrored or rotated without changing
the original events.
Connect so that the quill will not move up to the Z Rapid position, and back
down unnecessarily. However, to be connective, you must be certain that the X,
Y, Z begin of the first event, once offset or rotated, coincides with the X, Y, Z
end of the last event.
Program an event parallel to X or Y (where the geometry is the easiest to
describe), rotate it to the desired position, and 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 11.4.
Page 73
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
69
Figure 8.10 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 Finishing Teach Events
Teach events are either POSN/DRILL or MILL events that are originated in the DRO
Mode (see Section 6.6).
The Teach events that are started in the DRO Mode must be finished in the Program
Mode before running. Teach events are of these different types:
TEACH POSN/DRILL - See Section 8.1 for a description of Position/Drill event
prompts.
TEACH MILL - a straight line that specifies the beginning and the end. When
TEACH MILL events are defined using the CONT MILL softkey, the prompts for
information that cannot change will be suppressed. See Section 8.3 for a description
of Mill event prompts.
When a Teach event is unfinished, the words NOT OK will appear next to the event
type. Once the prompts are completed, the words NOT OK and Teach will disappear.
The event will become a normal POSN/DRILL or MILL event.
Page 74
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
70
9.0 Three-Axis Program Events
This section describes the program events and prompts that are available in three-axis
programming. If your ProtoTRAK SMX CNC is configured for two-axis programming only, you
should skip this section.
Events are fully defined pieces of geometry. By programming events, you tell the ProtoTRAK
SMX 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 Set-Up Mode.
9.1 POSN: Position Events
This event type positions the table and quill 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 at 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. RPM programming is available only if the Programmable Electronic Head
Option is active.
Tool # is the tool number you assign. SET will use the tool number of the previous event.
9.2 DRILL Events
This event positions the table to the specified X and Y position, moves the HEAD at
rapid to the Z RAPID location, feeds the quill 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: is the number of tool withdrawal cycles. Each cycle drills and then
retracts to the Z rapid position. The factory setting is for each peck to be
successively smaller, taking the largest cuts at the beginning and the smallest at the
end (Variable). You may change this to equal pecks. To do this, press the HELP key
when the highlight is on this prompt. This will take you to a screen where you may
choose to have the same amount of material taken per peck (Fixed). You can also
choose Chip Break, where the tool will perform fixed pecks, but only rapid out about
0.5mm after each peck, instead of going back to the Z rapid position after every
peck. This new setting will remain until you change it again.
Page 75
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
71
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event. RPM programming is available only if the Programmable Electronic Head
Option is active.
Z Feedrate: is the drilling feedrate.
Tool #: is the tool number you assign.
9.3 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: selects whether the hole is to be drilled or bored.
If the Programmable Electronic Head Option is active, you will also have the choice:
Tap = 3.
# 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 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. Tap is available only if
the Programmable Electronic Head Option is active.
# PECKS: is the number of tool withdrawal cycles. Each cycle drills and then
retracts to the Z rapid position. The factory setting is for each peck to be
successively smaller, taking the largest cuts at the beginning and the smallest at the
end (Variable). You may change this to equal pecks. To do this, press the HELP key
when the highlight is on this prompt. This will take you to a screen where you may
choose to have the same amount of material taken per peck (Fixed). You can also
choose Chip Break, where the tool will perform fixed pecks, but only rapid out about
0.5mm after each peck, instead of going back to the Z rapid position after every
peck. This new setting will remain until you change it again.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event. RPM programming is available only if the Programmable Electronic Head
Option is active.
Z Feedrate: is the drilling feedrate.
Tool #: is the tool number you assign.
9.4 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.
Page 76
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
72
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 Depth: is the depth of the cut in Z. If the Advanced Features Option is active, Z
Begin and Z End prompts will appear in the place of Z Depth.
Z Begin: is the Z dimension to the beginning of the mill cut (Advanced Features
Option).
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.
Z End: is the Z dimension to the end of the mill cut; incremental is Z Begin
(Advanced Features Option).
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. RPM programming is available only if the Programmable Electronic Head
Option is active.
Z Feedrate: is the Z feedrate from Z Rapid to Z begin.
XYZ Feedrate: is the milling feedrate from Begin to End in in/min from .1 to 100, or
mm/min from 5 to 2540.
Tool #: is the tool number you assign.
Continue: Yes or no. This prompt appears when the Advanced Features Option is
not active in order to program a continuous tool path without stops and eliminate
repetitive prompts in the next event. If the Advanced Features Option is active, use
the Profile event to accomplish the same thing.
9.5 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).
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 a 180o arc, 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 SMX CNC will automatically assume that all 180o arcs that
have the same beginning, ending and center dimensions for Z, lie in the XY plane. If you want
a 180o arc in a vertical plane, you must program two 90o 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.
Page 77
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
73
Z Depth: is the depth of the cut in Z. If the Advanced Features Option is active, Z
Begin and Z End prompts will appear in the place of Z Depth.
Z Begin: is the Z dimension to the beginning of the arc cut (Advanced Features
Option).
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.
The Z End dimension is programmed only if the Advanced Features Option is active.
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.
The Z Center dimension is programmed only if the Advanced Features Option is
active.
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. RPM programming is available only if the Programmable Electronic Head
Option is active.
Z Feedrate: is the Z feedrate from Z Rapid to Z Begin.
XYZ Feedrate: is the milling feedrate from Begin to End in in/min from .1 to 100, or
mm/min from 5 to 2540.
Tool #: is the tool number you assign
Continue: Yes or no. This prompt appears when the Advanced Features Option is
not active in order to program a continuous tool path without stops and eliminate
repetitive prompts in the next event. If the Advanced Features Option is active, use
the Profile event to accomplish the same thing.
9.6 POCKET Event
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 stepover 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 stepover
percentage. The value you enter here will remain the same until you change it
again.
Page 78
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
74
9.6.1 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 9.6.5 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 9.6.7 for a bottom finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event. RPM programming is available only if the Programmable Electronic Head
Option is active.
FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available
only if the Programmable Electronic Head Option is active.
Z Feedrate: is the Z feedrate from Z rapid to Z end.
XYZ Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540.
Fin Feedrate: is the milling feedrate for the finish cut.
Tool #: is the tool number you assign.
9.6.2 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).
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.
Page 79
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
75
# 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 9.6.5 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 9.6.7 for a bottom finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event. RPM programming is available only if the Programmable Electronic Head
Option is active.
FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available
only if the Programmable Electronic Head Option is active.
Z Feedrate: is the Z feedrate from Z rapid to Z end.
XYZ Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540.
Fin Feedrate: is the milling feedrate for the finish cut.
Tool #: is the tool number you assign.
9.6.3 Irregular Pocket (Advanced Features Option)
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 9.6.5 for more information about the zigzag ramp.
Z Feedrate: is the Z feedrate from Z rapid to Z end.
XYZ Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to
2540.
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut. See
Section 9.6.7 for a bottom finish cut.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event. RPM programming is available only if the Programmable Electronic Head
Option is active.
FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available
only if the Programmable Electronic Head Option is active.
Fin Feedrate: is the finish cut milling feedrate in in/min from .1 to 100, or mm/min
from 5 to 2540.
Tool #: is the tool number you assign.
Page 80
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
76
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.
9.6.4 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 SMX
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.
9.6.5 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.
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 SMX 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.
9.6.6 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.
9.6.7 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.
Page 81
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
77
9.6.8 Face Mill (Advanced Features Option)
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
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%.
9.7 Islands (Advanced Features Option)
Islands programming is available as part of the Advanced Features Option. See
Section 3.1.2.
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
Page 82
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
78
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.
9.7.1 Circular Island (Advanced Features Option)
Press the Circle Island soft key if you wish to mill a circular island.
Prompts for the Circular Island:
X CENTER: is the X dimension of the center of the Island.
Y CENTER: is the Y 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.
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. RPM programming is available only if the Programmable Electronic Head
Option is active.
FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available
only if the Programmable Electronic Head Option is active.
Z FEEDRATE: is the Z feedrate from Z rapid to Z end.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540.
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts.
Page 83
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
79
TOOL #: is the tool number you assign.
9.7.2 Rectangular Island (Advanced Features Option)
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 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.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event. RPM programming is available only if the Programmable Electronic Head
Option is active.
FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available
only if the Programmable Electronic Head Option is active
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.
Z FEEDRATE: is the Z feedrate from Z rapid to Z end.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts
TOOL #: is the tool number you assign.
Page 84
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
80
9.7.3 Irregular Island (Advanced Features Option)
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 pocket 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 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. RPM programming is available only if the Programmable Electronic Head
Option is active.
FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available
only if the Programmable Electronic Head Option is active
Z FEEDRATE: is the Z feedrate from Z rapid to Z end.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540.
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.
Page 85
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
81
9.8 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 SMX CNC will automatically initiate
the powerful Auto Geometry Engine. See Section 10.0 for programming with A.G.E.
9.8.1 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.
RPM: is the spindle RPM for the event. INC SET will use the RPM of the previous
event. RPM programming is available only if the Programmable Electronic Head
Option is active.
FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available
only if the Programmable Electronic Head Option is active.
Z Feedrate: is the Z feedrate from Z rapid to Z end.
XYZ Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540.
Finish Feedrate: is the milling feedrate for the finish cut.
Tool #: is the tool number you assign
9.8.2 Rectangular Profile
Press the RECTANGLE soft key if you wish to mill a rectangular frame (all corners
are 90o 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.
Page 86
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
82
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. RPM programming is available only if the Programmable Electronic Head
Option is active.
FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available
only if the Programmable Electronic Head Option is active.
Z Feedrate: is the Z feedrate from Z rapid to Z end.
XYZ Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to 2540.
Fin Feedrate: is the milling feedrate for the finish cut (if programmed).
Tool #: is the tool number you assign.
9.8.3 Irregular Profile (Advanced Features Option)
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.
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).
Z Feedrate: is the Z feedrate from Z rapid to Z end.
XYZ Feedrate: is the milling feedrate in in/min from .1 to 100, or mm/min from 5 to
2540.
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. RPM programming is available only if the Programmable Electronic Head
Option is active.
Page 87
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
83
FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available
only if the Programmable Electronic Head Option is active.
Fin Feedrate: is the finish cut milling feedrate in in/min from .1 to 100, or mm/min
from 5 to 2540.
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 10.
9.9 Helix Events (Advanced Features Option)
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.
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. RPM programming is available only if the Programmable Electronic Head
Option is active.
XYZ Feedrate: is the feedrate from beginning to end in in/min from .1 to 100, or
mm/min from 5 to 2540.
Tool #: is the tool you assign.
9.10 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 SMX 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
Page 88
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
84
holes, duplicating some machined shapes, or even repeating an entire program with
FIGURE 9.10.1 Holes 1-4 are mirrored across the Y axis to 5-8, respectively, about a line X OFFSET from
X=absolute 0
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 (Advanced Features Option) 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:
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:
Page 89
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
85
FIGURE 9.10.2 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
Press the SUBROUTINE (SUB) soft key to call up the Repeat, Mirror, and Rotate options.
9.10.1 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%. RPM programming is available only if the Programmable
Electronic Head Option is active.
% Feed: the percentage of the feeds programmed in the repeated events. 100% is
assumed.
Tool #: is the tool number you assign.
9.10.2 Mirror (Advanced Features Option)
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.
Page 90
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
86
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.
9.10.3 Rotate
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.
9.11 COPY Events (Advanced Features Option)
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.
Connect so that the quill will not move up to the Z Rapid position, and back
down unnecessarily. However, to be connective, you must be certain that the X,
Y, Z begin of the first event, once offset or rotated, coincides with the X, Y, Z
end of the last event.
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.
Page 91
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
87
Figure 9.11 In the above example, the offset that puts the group of holes in the
desired location is X=-1.50 and Y=-1.00.
9.11.1 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
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
9.12 Thread Mill Event (Advanced Features Option)
To program a Thread Mill event press the Thread mill soft key. This event includes
an automatic move in and out by 1.25mm 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.
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 mm or inch. For example, the pitch for a M5 x
1mm screw is 1 mm. For Imperial units, 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 divided by 20 =
0.05”.
Page 92
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
88
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.
DIRECTION: clockwise or counterclockwise.
# PASSES: - the number of passes to cut the thread to its final depth
Z FEEDRATE: The feedrate from Z Rapid to Z Begin.
XYZ FEEDRATE: The feedrate of XYZ along the path of the helix.
FIN CUT: width of the finish cut. If 0 is input, there is no finish cut.
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. RPM programming is available only if the Programmable Electronic Head
Option is active.
FIN RPM: is the spindle RPM for the finish cut. FIN RPM programming is available
only if the Programmable Electronic Head Option is active.
TOOL#: is the tool number you assign.
9.13 PAUSE Events
The purpose of the Pause Event is to allow you to program a stop condition within
the program. The effect of this event is to turn off the spindle, move the head to
the Z retract location with the X and Y position corresponding to the end of the
previous event and stopping the program run.
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 soft key. 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.
9.14 Engrave Event (Advanced Features Option)
The Engrave Event allows you to machine numbers, letters and special characters as
part of a part program. See Figure 9.14 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.
Page 93
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
89
Prompts for the Engrave Event:
Figure 9.14 The above figure shows the text and special characters available for the Engrave event.
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
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 (F8) 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. RPM programming is available only if the Programmable Electronic Head
Option is active.
Z FEEDRATE: Is the feedrate from Z rapid to Z end.
XYZ FEEDRATE: The feedrate of XYZ along the path of the text.
Tool #: is the tool number you assign.
.
9.15 Finishing Teach Events
Teach events are either POSN, DRILL or MILL events that are originated in the DRO
Mode (see Section 6.7).
The Teach events that are started in the DRO Mode must be finished in the Program
Mode before running. Teach events are of these different types:
TEACH POSN - for two-axis operation, the Position and Drill event types are
combined. See Section 9.1 for a description of Position event prompts.
Page 94
XYZ Machine Tools, Ltd.
XYZ Machine Tools Ltd. and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
90
TEACH DRILL- this may also be made into a bore event. See Section 9.2 for a
description of Drill event prompts.
TEACH MILL - a straight line that specifies the beginning and the end. When
TEACH MILL events are defined using the CONT MILL softkey, the prompts for
information that cannot change will be suppressed. See Section 9.4 for a description
of Mill event prompts.
When a Teach event is unfinished, the words NOT OK will appear next to the event
type. Once the prompts are completed, the words NOT OK and Teach will disappear.
The event will become a normal MILL, DRILL, or POSN event.
Page 95
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
91
10.0 Auto Geometry Engine (A.G.E.) Programming
FIGURE 10.1 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. Two-axis CNC programming will not require Z data. *
This entire section deals with the Auto Geometry Engine (A.G.E.), which is part of the
Advanced Features Option. If the Advanced Features Option is not active, the Auto
Geometry Engine is not available on your control. If you sometimes need to program
prints with data missing, the Auto Geometry Engine alone is worth the price of the
Advanced Features Option. See Section 3.1.2 for more information about the
Advanced Features Option.
When you program an Irregular Pocket or an Irregular Profile the A.G.E. is
automatically started.
The A.G.E. is powerful software that works behind the easy-to-use geometry
programming of the ProtoTRAK SMX 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.
10.1 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:
Where:
A.G.E. Mill: A straight line from one X Y point to another.
A.G.E. Arc: Any part of a circle.
Page 96
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
92
End A.G.E.: Ends the A.G.E. programming for the Irregular Pocket or Irregular
FIGURE 10.2 A.G.E. Mill prompts. Enter what you know, skip or guess the ones you don’t
Profile.
Abort A.G.E.: Aborts all A.G.E. events. The data for all the events is lost.
10.2 A.G.E. Mill Prompts
Press the A.G.E. Mill key.
Prompts in A.G.E. Mill programming:
Tangent: this refers to the tangency of the mill to the previous event. See Section
10.11 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.
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 10.7 for using Guess and Section 10.8 for using the Graphics to
enter a Guess.
Page 97
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
93
10.3 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
10.11 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 10.7.
10.4 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 DATA FWD softkey. After
you press the DATA FWD 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 DATA FWD or DATA BACK
key. Using INC SET or ABS SET will change the data.
If you want the event back on the right side, use the BACK hard key.
10.5 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 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 DATA FWD softkey.
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.
10.6 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 SMX CNC cannot program the tool path to clear the
pocket.
Page 98
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
94
The Irregular Profile has no such restriction since profiles may be open or closed.
FIGURE 10.7 The X End dimension has been entered as a guess—note the letter G
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 BACK hard key
or the PAGE FWD or PAGE BACK softkeys to position on of the A.G.E. events on the
right side of the screen. You may edit or insert other events.
10.7 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 SMX 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.
Guesses should always be entered as absolute dimensions. Once entered, the
guessed data is green and there is 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.
10.8 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 the highlight is on the prompt for which you wish to enter a guess, press the
Guess key. The Data Input Line will say "Enter Guess for X END" (for example). At
this point, press the LOOK key.
Page 99
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
95
Figure 10.8.1 When the Data Input Line says "Enter Guess" pressing LOOK gives you the
ability to use graphics to make your guesses.
On the screen shown in the figure above, the Data Input Line says "Enter Guess for X
BEG". Pressing LOOK at this point will take you to a special version of the LOOK
graphics. Using a mouse or the cursor keys, you may move a point around the
screen. When you come to the place where your point is, use the Enter key.
The softkeys for this special version of the LOOK graphics:
: move the cursor around the screen.
ZOOM IN: makes the drawing larger.
ZOOM OUT: makes the drawing smaller.
ENTER END: when the cursor is at the point you want to use as a guess, use this to
enter the end point of a line or an arc.
ENTER CENTER: use this to register a guess for the center of an arc.
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.
Your guess entries are loaded into the program when you exit the LOOK screen by
pressing BACK or by pressing LOOK again. The ProtoTRAK will use the last ENTER
key press and load that into the program.
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.
Page 100
XYZ Machine Tools, Ltd.
XYZ Turret Mill and ProtoTRAK SMX CNC Retrofit Safety, Programming, Operating & Care Manual
96
FIGURE 10.8.2 When the events are calculated based on Guessed data, they are represented by a dotted line
10.9 Calculated Data
Prompts that are skipped or for which guesses are entered may be replaced by data
calculated by the ProtoTRAK SMX 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.
10.10 Arcs and Conrads
If the print is missing a lot of data, it may be desirable to program arcs as separate
events where possible. This gives the system more information to work with.
10.11 Tangency
Tangency can occur between a mill and arc or an arc and arc. Specifically it means
necessary but not sufficient that the two geometries share one and only one. 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
Loading...