TRAK DPMS3, DPMS5 ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual

TRAK DPMS3, DPMS5 ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
TRAK DPMS3, DPMS5
ProtoTRAK SM CNC


Safety, Programming, Operating & Care Manual
Document: P/N 23210
Version:
092303
Southwestern Industries, Inc.
Plant location: 2615 Homestead Place
P. O. Box 9066
Rancho Dominguez, CA 90220-5610 USA
Compton, CA 90224-9066 USA
T | 310.608.4422 | F | 310. 764.2668
Service Department: 800.367.3165
e-mail: [email protected] | [email protected] | web:
www.southwesternindustries.com
Copyright 2003, Southwestern Industries, Inc. All rights are reserved. No part of this publication
may be reproduced, stored in a retrieval system, or transmitted, in any form or by any means,
mechanical, photocopying, recording or otherwise, without the prior written permission of
Southwestern Industries, Inc.
While every effort has been made to include all the information required for the purposes of this
guide, Southwestern Industries, Inc. assumes no responsibility for inaccuracies or omission and
accepts no liability for damages resulting from the use of the information contained in this guide.
All brand names and products are trademarks or registered trademarks of their respective
holders.
Southwestern Industries, Inc.
2615 Homestead Place
Rancho Dominguez, CA 90220
Phn 310/608-4422 ! Fax 310/764-2668
Service Department
Phn 800/367-3165 ! Fax 310/886-8029
Table of Contents
1.0
Introduction
1.1
Manual Organization
2.0
2.1
2.2
Safety
2.3
Safety Publications
Danger, Warning, Caution and Note
Labels and Notices Used in this Manual
Safety Precautions
3.0
Description
3.1
3.2
3.3
3.4
3.5
3.6
3.7
3.8
3.9
4.0
4.1
4.2
4.3
4.4
4.5
4.6
4.7
4.8
4.9
5.0
5.1
5.2
5.3
5.4
5.5
5.6
Display Pendant Front
3.1.1
Keyboard Hard Keys
3.1.2
Soft Keys
3.1.3
Emergency Stop Switch
3.1.4
The Liquid Crystal Display
Pendant Left Side
Pendant Right Side
Machine Specifications
Lubrication System
3.5.1
Factory Default Values
Electrical Cabinet
Optional Equipment
3.7.1
Position Encoders
3.7.2
Power Draw Bar
3.7.3
Remote Stop Go Switch
3.7.4
Work Light
3.7.5
Coolant Pump
3.7.6
Auxiliary Functions
3.7.7
Limit Switches
Integrated Ram and Quill Encoders
Servo Motors
Basic Operation
Switching the ProtoTRAK SM CNC on
Shutting down the ProtoTRAK VM
Spindle Forward/Off/Reverse
Manual Operation of Ram, Table, Saddle
Emergency Stop
Switching Between Two and Three-Axis
Operation
Mister/Coolant Pump
Help Functions
4.8.1
Math Helps
Windows Up or Down
Definitions, Terms & Concepts
ProtoTRAK SM CNC Axis Conventions
Part Geometry & Tool Path Programming
Planes and Vertical Planes
Absolute & Incremental Reference
Referenced & Non-Referenced Data
Incremental Reference Position in
Programming
3
5.9
5.10
5.11
Tool Diameter Compensation
Tool Diameter Compensation When
Contouring in Z with Part Geometry
Connective Events
Conrad
Memory & Storage
3
6
6.0
DRO Mode
6.1
6.2
6.3
6.4
6.5
6.6
6.7
6.8
Enter DRO Mode
DRO Functions
Jog
Power Feed
Do One
Teach
6.6.1
Entering Teach Data
Return to Absolute Zero
Tool #
7.0
Program Mode
1
9
9
10
10
10
11
12
13
15
15
15
15
15
15
16
16
16
16
16
16
16
17
18
18
18
18
18
19
19
19
20
21
21
22
22
23
23
5.7
5.8
7.1
7.2
7.3
7.4
7.5
7.6
7.7
7.8
7.9
7.10
7.11
7.12
7.13
23
25
26
26
27
29
29
30
30
31
31
31
32
32
Part 1: Getting Started & Some General Info
Programming Overview
33
Enter Program Mode
33
Program Header Screen
34
7.3.1
Program Name
34
7.3.2
General Program Options
35
7.3.3
Program Header Softkeys
36
Auxiliary (AUX) Functions
36
Multiple Fixtures
37
7.5.1
The Default Fixture
38
7.5.2
Fixtures & Running the Program
38
7.5.3
Editing Fixtures
38
Assumed Inputs
38
Z Rapid Positioning
38
Softkeys within Events
39
Programming Events
39
Editing Data While Programming
40
LOOK
41
Finish Cuts
41
Two Versus Three-Axis Positioning
42
8.0
Program Mode
Part 2: Program Events
8.1
8.2
8.3
8.4
8.5
8.6
POSN: Position Events
DRILL Events
BOLT HOLE Events
MILL Events
ARC Events
POCKET Event
8.6.1
Circular Pocket
8.6.2
Rectangular Pocket
8.6.3
Irregular Pocket
8.6.4
Tool Path in Pocket Events
8.6.5
Zigzag Z Depth Cuts
8.6.6
Conrad in Pocket Events
8.6.7
Bottom Finish Cut
i
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
43
43
44
44
45
46
46
46
47
48
48
48
48
8.7
8.8
8.9
8.10
8.11
8.12
8.13
8.14
8.15
9.0
Islands
8.7.1
Circular Island
8.7.2
Rectangular Island
8.7.3
Irregular Island
PROFILE Events
8.8.1
Circle Profile
8.8.2
Rectangular Profile
8.8.3
Irregular Profile
HELIX Events
SUBROUTINE Events
8.10.1 Repeat
8.10.2 Mirror
8.10.3 Rotate
COPY Events
THREAD MILL Event
PAUSE Events
ENGRAVE Event
Finishing Teach Events
49
49
50
51
52
52
52
53
54
54
56
56
56
57
57
58
58
58
Program Mode
Part 3: The Auto Geometry Engine
(A.G.E) Programming
9.1
9.2
9.3
9.4
9.5
9.6
9.7
9.8
9.9
9.10
9.11
Starting the A.G.E.
A.G.E. Mill Prompts
A.G.E. Arc Prompts
Skipping Over Prompts
The OK/NOT OK Flag
Ending A.G.E.
Guessing Data
LOOK and Guess
Calculated Data
Arcs and Conrads
Tangency
10.0
Edit Mode
10.1
10.2
10.3
10.4
Delete Events
69
Spreadsheet EditingTM
69
10.2.1 Selecting Data to be Displayed on the
Search Edit Table
70
10.2.2 Sorting Data
71
10.2.3 Making Global Changes to Data
71
Erase Program
73
Clipboard
73
11.0
Set Up Mode
11.1
The Tool Table
11.1.1 The Tool Table Screen
11.1.2 The Logic of the Tool Table
11.1.3 Initial Tool Set-Up
11.1.4 Starting Over: Erasing Tool Info
11.1.5 Adding a Tool
11.1.6 Replacing a Tool
11.1.7 Z Modifiers
11.1.8 Resetting the Reference Point
11.1.9 Saving Tool Information
11.1.10 Opening a Program
11.1.11 Making Tool Set-Ups Easy
11.1.12 Tool Table & 2-Axis CNC Operation
Tool Path
11.2.1 Soft Keys in Tool Path
11.2
61
62
63
63
63
64
64
65
66
66
66
75
76
76
77
78
78
78
78
79
79
79
79
79
80
80
11.3
11.4
11.5
Reference Positions (REF POSN)
11.3.1 Z Retract
11.3.2 Home Positions
11.3.3 Limit Positions
Fixture Offsets
Service Codes
12.0
Run Mode
13.0
Program In/Out Mode
13.1
Softkey Selections in the Program
In/Out Mode
90
Basic Navigation of Program In/Out Mode
Screens
90
13.2.1 Basic Parts of the Program In/
Out Mode Screens
90
13.2.2 Softkeys in the Program In/Out
Mode Screens
91
Opening a File
91
Saving Programs
91
Copying Programs
92
Deleting Programs
93
Renaming
94
Backing Up
95
ConvertersTM
96
13.9.1 Activating Converters
96
13.9.2 Converting from a Different Format
Into a ProtoTRAK SM CNC
97
13.9.3 Converting from the ProtoTRAK CNC
to a Different Format
98
ProtoTRAK and TRAK CNC Capability
98
13.10.1 File Formats
99
13.10.2 Opening .MX2 & .MX3 Files
99
13.10.3 Running ProtoTRAK SM Files on
ProtoTRAK & TRAK CNC
99
Running G Code Files
100
13.11.1 G Codes Recognized by the
ProtoTRAK SM CNC
101
13.11.2 M Codes Supported by the
ProtoTRAK SM CNC
101
13.11.3 Valid Characters for Word/Address
Sequences
101
Networking
102
13.12.1 What is a Network?
102
13.12.2 Why would you want to use the
networking capability of the
ProtoTRAK SM CNC control?
102
13.12.3 A Word of Advice Before Setting
Up Your Network
103
13.12.4 Peer-to-Peer Networking
103
12.1
12.2
12.3
12.4
12.5
12.6
12.7
12.8
12.9
12.10
13.2
13.3
13.4
13.5
13.6
13.7
13.8
13.9
13.10
13.11
13.12
Run Mode Screen
Two Versus Three-Axis Running
Starting to Run
Program Run
Program Run Messages
Stop
Feedrate Override
Trial Run
Data Errors
Fault Messages
ii
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
81
81
82
82
82
82
85
85
86
86
87
87
87
87
88
88
13.13
13.14
13.12.5 Basic Network Set-Up
13.12.6 Server & Client Network Overflow
13.12.7 Network Description of
the ProtoTRAK
RS232 Interface
13.13.1 Connections
13.13.2 Receiving a File
13.13.3 Sending a File
CAD/CAM & Post Processors
13.14.1 Writing a Post Processor
13.14.2 Convertible G-Codes
13.14.3 Supported Addresses
13.14.5 Format Terms & Definitions
13.14.6 G Codes that Generate Errors
13.14.7 Accepted M Codes
103
108
111
111
112
112
113
114
115
116
116
117
118
119
ProtoTRAK SM Training Checklist
iii
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
1.0 Introduction
Congratulations! Your TRAK DPM milling machine with the ProtoTRAK SM CNC is an excellent
toolroom machine. It features an easy-to-use interface and dozens of features that maximize
machinist’s productivity for any kind of toolroom job.
Manual machining is always available and made easier with features like power feed, 150 inch
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 prototyping and moderately
complex, low volume work.
Three-axis machining is programmed and run with unprecedented flexibility. Programs may
be entered at the control or imported from CAD/CAM files. Advanced color graphics show
program features.
The operation of the ProtoTRAK SM 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.
1.1
Manual Organization
Section 2 of this manual provides important safety information. It is highly
recommended that all operators of this product review this safety information.
Section 3 provides a description of the TRAK DPMS3, DPMS5 and the ProtoTRAK SM
CNC.
Section 4 describes the operation of the milling machine and some basic operations of
the ProtoTRAK SM CNC.
Section 5 defines some terms and concepts useful in learning to program and operate
the ProtoTRAK SM CNC.
The ProtoTRAK SM CNC is organized into six Modes of operation that are described in
the following sections.
Section 6 DRO: Digital Readout, jog, and powerfeed operations.
Section 7 Programming, Part 1: covers some general programming information and
instructions on starting new programs.
Section 8 Programming, Part 2: Program Events - instructions for the canned cycles, or
events used to program the ProtoTRAK SM CNC.
Section 9 Programming, Part 3: the A.G.E., or Auto Geometry Engine, so powerful it
gets its own section.
Section 10 Edit: for routines to make large-scale changes to programs in current
memory, including the powerful Spreadsheet Editing®
Section 11 Set-Up: Tool information, part graphics and special codes.
Section 12 Run: Instructions on running a program to machine your part.
Section 13 Program In/Out: Storing and managing your programs.
1
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
.
2
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
2.0 Safety
The safe operation of the TRAK DPMS5 or DPMS3 depends on its proper use and the precautions
taken by each operator.
2.1
•
Read and study this manual. Be certain every operator understands the operation
and safety requirements of this machine before its use.
•
Always wear safety glasses and safety shoes.
•
Always stop the spindle and check to ensure the CNC control is in the stop mode
before changing or adjusting the tool or workpiece.
•
Never wear gloves, rings, watches, long sleeves, neckties, jewelry, or other loose
items when operating or around the machine.
•
Use adequate point of operation safeguarding. It is the responsibility of the
employer to provide and ensure point of operation safeguarding per OSHA 1910.212 Milling Machine.
Safety Publications
Refer to and study the following publications for assistance in enhancing the safe use of
this machine.
Safety Requirements For The Construction, Care And Use of Drilling, Milling,
and Boring Machines (ANSI B11.8-1983). Available from The American National
Standards Institute, 1430 Broadway, New York, New York 10018.
Concepts And Techniques Of Machine Safeguarding (OSHA Publication Number
3067). Available from The Publication Office - O.S.H.A., U.S. Department of Labor, 200
Constitution Avenue, NW, Washington, DC 20210.
2.2
Danger, Warning, Caution, and Note Labels and Notices As Used
In This Manual
DANGER - Immediate hazards that will result in severe personal injury or death.
Danger labels on the machine are red in color.
WARNING - Hazards or unsafe practices that could result in severe personal injury
and/or damage to the equipment. Warning labels on the machine are orange in color.
CAUTION - Hazards or unsafe practices that could result in minor personal injury or
equipment/product damage. Caution labels on the machine are yellow in color.
NOTE - Call attention to specific issues requiring special attention or understanding.
3
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5 ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Safety & Information Labels Used On The
TRAK DPMS5 or DPMS3
It is forbidden by OSHA regulations and by law to deface, destroy or remove any
of these labels
4
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
230 VOLTS
Safety & Information Labels Used On The
TRAK DPMS5 or DPMS3
It is forbidden by OSHA regulations and by law to deface, destroy or remove any
of these labels
5
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
2.3
Safety Precautions
1.
Do not operate this machine before the TRAK DPMS5 or DPMS3 Safety,
Installation, Maintenance, Service and Parts List Manual, and the TRAK
DPMS5 or DPMS3 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
jewelry including watches and rings, neckties, and any loose-fitting clothing.
5.
Keep your hair away from moving parts. Wear adequate safety headgear.
6.
Protect your feet. Wear safety shoes with oil-resistant, anti-skid soles, and steel
toes.
7.
Take off gloves before you start the machine. Gloves are easily caught in moving
parts.
8.
Remove all tools (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.
6
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
15. Prevent slippage. Keep the work area dry and clean. Remove the chips, oil,
coolant and obstacles of any kind around the machine.
16. Avoid getting pinched in places where the table, saddle or spindle head create
"pinch points" while in motion.
17. Securely clamp and properly locate the workpiece in the vise, on the table, or in
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.
7
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
8
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
3.0 Description
3.1
Display Pendant Front (see Figure 3.1)
FIGURE 3.1 The ProtoTRAK SM CNC front panel
3.1.1
•
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.
FEED !: feedrate override to increase feedrate up to 150%.
FEED ": feedrate override to decrease feedrate down to 10%.
ACCESSORY: When the switch is in the On position, the coolant pump (or mister)
will come on and stay on during machining operations. In the Auto mode, the
coolant pump or mister 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 mister will not operate.
9
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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 SM CNC and change from 2-axis to 3-axis, or
3-axis to 2-axis operation.
!
"
: 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.
3.1.2
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 the Z retract is not set, the RUN mode key will be grayed out because setting
the Z retract is a necessary step for running a program.
3.1.3
Emergency Stop Switch
The emergency stop (E-stop) switch kills all power to the spindle and ProtoTRAK's servomotors.
The computer and pendant remain powered.
3.1.4
The Liquid Crystal Display (LCD)
The display of the ProtoTRAK SM CNC is a 10.4" active-matrix color LCD. The very top is the
Status Line that shows the overall status of the ProtoTRAK SM 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.
10
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
3.2
Pendant Left Side (See Figure 3.2 for a description of the left side panel of the display.)
FIGURE 3.2 The ProtoTRAK SM CNC left side with connectors labeled
11
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
3.3
Pendant Right Side (See Figure 3.3 for a description of the connectors and
features located on the right side of the display panel.)
FIGURE 3.3 The ProtoTRAK SM CNC right side
12
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
3.4
Machine Specifications (See Figures 3.4.1 and 3.4.2)
FIGURE 3.4.1 The TRAK DPM S Series machine overview
13
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
TRAK DPMS3
Table Size - 50" x 10"
T-Slots – 3 x .63” x 2.48”
Travel (X, Y, Z) – 30 x 17 x 23.5”
Maximum quill travel – 5”
Quill diameter – 3 15/16”
Spindle Taper – NST 40
Spindle Speed Range – 70-4200 rpm
Spindle Center to Column Face – 19”
Spindle motor – 3 HP
Power Requirement control - 110V; 1P; 10A
Power Requirement machine – 220/440V; 3P;
8.5/4.25A
Maximum Weight on Table - 1320 lb
Height of table from bottom of bed – 38”
Maximum spindle nose to table – 23.5”
Minimum height – 85”
Maximum height – 95”
Width of machine including table – 73”
Length of electric box door closed – 76”
Overall width including full table traverse – 108”
Overall length with electrical door open – 70”
Footprint of machine – 24” x 44”
Weight net/shipping lbs. – 4100/4400
Maximum work capacities in mild steel – drilling,
1” dia; tapping, ¾”; milling, 3 in3/min
Maximum rapid feed – 150 IPM
FIGURE 3.4.2 The TRAK DPMS3 Series back view
14
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
TRAK DPMS5
Table Size - 50" x 12"
T-Slots – 3 x .63” x 2.48”
Travel (X, Y, Z) – 40 x 20 x 23.5”
Maximum quill travel – 5”
Quill diameter – 3 15/16”
Spindle Taper – NST 40
Spindle Speed Range – 70-3950 rpm
Spindle Center to Column Face – 20”
Spindle motor – 5 HP
Power Requirement control - 110V; 1P; 10A
Power Requirement machine – 220/440V; 3P; 14/7A
Maximum Weight on Table - 1760 lb
3.5
Height of table from bottom of bed – 41”
Maximum spindle nose to table – 23.5”
Minimum height – 87”
Maximum height – 98”
Width of machine including table – 94”
Length of electric box door closed – 81”
Overall width including full table traverse – 136”
Overall length with electrical door open – 77”
Footprint of machine – 24” x 48.4”
Weight net/shipping lbs. – 4400/4600
Maximum work capacities in mild steel – drilling,
1” dia; tapping, 1”; milling, 5 in3/min
Maximum rapid feed – 150 IPM
Lubrication System
3.5.1
Factory Default Values
Interval Time – 60 min.
Discharge Time – 15 sec
Discharge Pressure – Approximately 100 – 150psi
To adjust the amount of Discharge Pressure displayed on the lube pump gauge, loosen
the jam nut and turn the adjustment screw located on the top right side of the lube
pump while the lube pump is activated. To activate the lube pump use Service Code
“300,” see Section 11.4.
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 DPMS3 or DPMS5 mill way surfaces and ballscrews.
The settings for the lube pump can be viewed by doing the following: press Service
Codes, press “A” (software), press Code 313. This screen lists the values programmed
for the cycle time and discharge time.
3.6
Electrical Cabinet
The TRAK DPMS3 and DPMS5 use two electrical inputs. Spindle 220 or 440V power is
wired into the cabinet. A cord is supplied from the cabinet to a 110V power source for
running the ProtoTRAK SM CNC.
3.7
Optional Equipment
3.7.1
Position Encoders
The ProtoTRAK SM CNC may be configured to run either with or without independent
position encoders for X and Y travel. Optional encoders include the TRAK sensors or
glass scales, each with .0002” underlying resolution.
3.7.2
Power Draw Bar
A manual draw bar, of the NMTB or NST type comes standard with the machine. A
power draw bar option may be ordered. The draw bar included in the option may be
CAT or NMTB/NST.
15
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
An NMTB/NST type of draw bar is the appropriate length to fit tool holders that have a
threaded tang on the top. The CAT type is longer to thread into CNC tool holders that
have the tool changer grip, or retention knob removed.
3.7.3
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.
3.7.4
Work Light
An optional halogen work light is available. It mounts to the left side (facing) of the
column and plugs into a 110v outlet in the electrical cabinet.
3.7.5
Coolant Pump
The optional coolant pump is mounted in the back of the machine column. It is plugged
into the electrical cabinet and may be configured to operate as commanded by the
auxiliary functions.
3.7.6 Auxiliary Functions
Auxiliary functions are controlled through the ProtoTRAK SM 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 misters or other pneumatically activated peripheral
equipment. Shop air should not exceed 125 psia.
•
Switched and fused 120 VAC 8 Amp outlet(s) for coolant pumps, automatic oilers,
etc.
•
INPUT/OUTPUT to interface with programmable indexers, dividing heads, etc.
o Output from ProtoTRAK SM CNC 3 is .3-second actuation of a solid-state
relay between pin 3 (plus), and pin 4 (minus).
o Input to the ProtoTRAK SM 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.
3.7.7 Limit Switches
There are limit switches for the ram, saddle and table travel.
3.8
Integrated Ram and Quill Encoders
A glass scale for the Quill operation is standard. Ram motion is measured by an encoder
on the ram servo motor. The feedback from these encoders is integrated and displayed
in the Z-axis digital readout as one dimension.
3.9
Servo Motors
The servo motors on table, saddle and ram are 560 in-oz torque. Integrated into each
motor is an encoder with 0.000018” underlying resolution.
16
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
4.0 Basic Operation
One of the things that makes the TRAK DPM so easy to use is that most of the operations of the
ProtoTRAK SM 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 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
Switching the ProtoTRAK SM CNC On
To turn the ProtoTRAK SM CNC on, move the toggle switch on the display side panel to the Up position.
The Windows operating system and the ProtoTRAK SM CNC software will take a few seconds to
load from the system's flash memory. If you have connected the ProtoTRAK SM CNC to a
network, it may take as long as 90 seconds for the communications to be established. When
complete, the ProtoTRAK SM 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 SM 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.
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 SM 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.
17
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
4.2
Shutting down the ProtoTRAK SM 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 SM CNC off
by moving the toggle switch on the display side panel to the down position.
If the CNC is not shut down properly, the system will make you wait while it runs a scan
disk self-diagnostic routine and scold you for not following the instructions.
Note: When you turn the PROTOTRAK SM CNC off, always wait a few seconds before turning it back on.
4.3
Spindle Forward/Off/Reverse
The spindle is controlled through the drum switch mounted on the side of the machine head.
4.4
Manual Operation of the Ram, Table & Saddle
The TRAK DPMS3 or DPMS5 may be used manually. The head/ram may be jogged to
any location and the quill operated manually. Either motion will count in Z.
4.5
Emergency Stop
Press the button to shut off power to the spindle motor and axis motors. Rotate the
switch to release.
4.6
Switching Between Two and Three-axis Operation
The ProtoTRAK SM 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 SM CNC is currently
operating in three axis and it will say GO TO 3 AXIS when the ProtoTRAK SM CNC is
currently operating in two axis. See Figure 4.6.
FIGURE 4.6 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.
18
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
4.7
Mister/Coolant Pump
An optional coolant pump may be connected to your TRAK DPMS3 or DPMS5. A mister or
pump may be operated either manually or programmed in the events if the optional AUX
Function is also purchased.
To
•
•
•
4.8
operate the mister or coolant pump manually, use the ACCESSORY hard key:
ON - will turn on the mister or coolant pump until you turn it off.
AUTO - will turn on the mister or coolant pump on, as programmed into events.
Off (no light) - the coolant pump or mister stays off.
Help Functions
When a blue question mark appears next to the HELP hard key, that means special
functions or configuration settings are available for the current operation. For example,
at the program header with the highlight on the program name, the blue question mark
appears. Pressing the HELP key at that time will call up a table with alpha and special
characters you can use to name your program.
4.8.1 Math Helps
When the blue question mark does not appear, pressing HELP will initiate the Math
Helps.
FIGURE 4.8.1 The first Math Helps screen. Choose among the alternatives based on the
information you need to calculate
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.
19
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK VM CNC Safety, Programming, Operating & Care Manual
FIGURE 4.8.2 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.
4.9
Windows Up or Down
Some of the selections in the ProtoTRAK SM CNC will cause a window to appear with a
message. To eliminate the window in order to see what is behind it, press the u hard
key. To restore the window, press the t hard key.
20
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
5.0 Definitions, Terms & Concepts
5.1
ProtoTRAK SM 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.
FIGURE 5.1 ProtoTRAK SM CNC conventions
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 SM CNC gives you ultimate flexibility in programming. Programs that are entered
through the ProtoTRAK SM CNC system can be entered as either Part Geometry or Tool Path.
Part Geometry programming is the popular programming style of the ProtoTRAK family of
products. This is done by defining the final geometry of the part, and the ProtoTRAK SM
CNC has the job of figuring out the tool path from the part dimensions and the tool setup 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 vertical planes
Using Geometry Programming, it is impossible for the ProtoTRAK SM 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.
21
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
_________________________________________________________________
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.
5.3
Planes and Vertical Planes
A plane is any flat surface. If that surface lies flat on the table, it is the XY plane. That is, if you
move your finger along that surface or plane, you are moving in the X and/or Y direction, but not
in Z (or at least not until you pick your finger up). If you tilted that surface (think of it as a piece
of paper) straight up so that it faces the front of the machine, it would be in the XZ plane. If you
tilted it up so that it faced left or right, it would be in the YZ plane.
A vertical plane is any plane (or surface) tipped up on its edge on the table (see below).
Unlike most CNC controls,
the ProtoTRAK SM CNC can
machine arcs in any vertical
plan rather than just XZ or YZ.
FIGURE 5.3 Vertical planes
5.4
Absolute & Incremental Reference
The ProtoTRAK SM 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:
FIGURE 5.4 Each point has both an absolute and an incremental reference in the X axis. The
ProtoTRAK SM CNC allows you to program using either.
22
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
5.5
Referenced & Non-Referenced Data
Data is always loaded into the ProtoTRAK SM CNC by using the INC SET or ABS SET key.
X, Y, Z positions are referenced data. In entering any X, Y, or Z position data, you must
note whether it is an incremental or absolute dimension and enter it accordingly. All
other information (non-referenced data), such as tool diameter, feedrate, etc. is not a
position and may, therefore, be loaded with either the INC SET or ABS SET key. This
manual uses the term SET when either INC SET or ABS SET may be used
interchangeably.
5.6
Incremental Reference Position in Programming
When X, Y, Z RAPID and Z data for the beginning position of any event are input as
incremental data, this increment must be measured from some known point in the
previous event. Following are the positions for each event type from which the
incremental moves are made in the subsequent event:
Position: X, Y and Z programmed
Drill: X, Y, Z RAPID, and Z END programmed
Bolt Hole: X CENTER, Y CENTER, Z RAPID and Z END programmed
Mill: X END, Y END, Z RAPID and Z END programmed
Arc: X END, Y END, Z RAPID and Z END programmed
Circle (POCKET or FRAME): X CENTER, Y CENTER, Z RAPID and Z END programmed
Rectangle or Irregular (POCKET or PROFILE): X1 and Y1 corner, Z RAPID and Z
END programmed
Helix: The X END, Y END, Z RAPID, and Z END programmed
Sub: The reference position as defined for the specific events above for the event prior
to the first event that was repeated.
A.G.E. PROFILE: The appropriate reference position as defined for the specific events
above for the last event that is programmed
For example, if an ARC event followed a MILL event, a 2.0 inch incremental X BEG would
mean that in the X direction the beginning of the ARC event is 2.0 inches from the end of
the MILL event.
5.7
Tool Diameter Compensation
Tool diameter compensation allows the machined edges shown directly on the print to be
programmed instead of the center of the tool. The ProtoTRAK SM 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.
23
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
FIGURE 5.7.1 Examples of tool right
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.
24
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
5.8
Tool Diameter Compensation when Contouring in Z with Part Geometry
Left and right tool diameter offsets are always those projected into the XY plane. Tool
offsets in the Z direction are always up and assume the use of a ball end mill. When
contouring in the Z-axis, this up tool offset is always activated regardless of left, right,
center if 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.
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
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.
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
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).
25
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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 SM CNC that allows you to program a tangentially
connecting radius between connective events, or tangentially connecting radii for the corners of
pockets and frames without the necessity of complex calculations.
For the figure below, you program an Arc event from X1, Y1 to X2, Y2 with tool offset left, and
another Arc event from X2, Y2 to X3, Y3 also with tool offset left. During the programming of the
first Arc event, the system will prompt for Conrad at which time you input the numerical value of
the tangentially connecting radius r=K3. The system will calculate the tangent points T1 and T2
and direct the tool cutter to move continuously from X1, Y1 through T1, r=k3, T2 to X3, Y3.
FIGURE 5.10.1 A Conrad is added between the two intersecting lines
Note: Conrad must always be the same as or larger than the tool radius for inside corners. If Conrad is
less than the tool radius, and an inside corner is machined, the ProtoTRAK SM CNC will ignore the
Conrad.
For the figure below, you program an Arc event from X1, Z1 to X2, Z2, and a Mill to X3, Z3.
During the programming of the Arc event, the system will prompt for Conrad at which time you
input the numerical value of the tangentially connecting radius r=k. The system will calculate the
tangent points T1 and T2 and direct the tool cutter to move continuously from X1, Z1 through T1,
r=k, T2 and on to X3, Z3.
FIGURE 5.10.2 A Conrad is added between an arc and a line
26
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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 SM 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 information is on the ProtoTRAK SM
CNC flash memory, a floppy disk or an offline computer connected to the ProtoTRAK SM
CNC via the RS232 or network connection.
27
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
28
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
6.0 DRO MODE
The ProtoTRAK SM 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 CRT screen will show:
FIGURE 6.1 The DRO screen
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.
29
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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.
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.
d. 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.
g. 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.
h. 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 2.00" of the table in the negative direction, you would
enter: X, 2, +/-, INC SET.
d.
Initiate the power feed move by pressing GO.
e.
The feedrate is automatically set to 10 ipm (or 254 mm per min). Press FEED !
or FEED " to adjust the feedrate from 1 ipm to 100 ipm. (or 254 to 2540)
f.
Press STOP to halt power feed. Press GO to resume.
30
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
6.5
g.
Repeat the process beginning at "c" above as often as you wish.
h.
Press RETURN soft key to return to manual DRO operation.
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.
6.6
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.
6.6.1 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.
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:
31
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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.
6.7
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 ram to Z
retract 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. When you are in 2-axis
CNC operation, only the X and Y will move, the ram will not.
6.8
Tool #
The ProtoTRAK SM CNC allows you to use the offsets 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.
32
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
.
7.0 Program Mode
Part 1: Getting Started & Some General Information
7.1
Programming Overview
The ProtoTRAK SM 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 SM 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.
FIGURE 7.2 The Program Mode header screen
33
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
.
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 SM CNC are usually named for the part that is to be
machined. When programs (or files) are named using the ProtoTRAK SM CNC, the name
can be up to 20 characters long. Programs imported into the ProtoTRAK SM 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.
FIGURE 7.3 Pressing the Help hard key when the Program Name is highlighted calls up alpha keys
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 SM CNC.
Use a keyboard plugged into the ProtoTRAK SM CNC to name the program.
34
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
.
To use the alpha keys and special characters on the ProtoTRAK SM CNC:
•
Use the Clear softkey to erase the entire line; the Backspace softkey to erase the
last character or number.
•
Use the arrow softkeys to move around the table.
•
Once the character you want is highlighted, use the Enter softkey to load the
character into the program name.
•
Use the blank space on the lower right of the table to insert a space into the
program name.
•
Once you finish entering the letters and special characters, press the End softkey.
This tells the ProtoTRAK SM 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..
Scale: Allows a scale factor between .1 and 10. An input of 5 means the part will be 5
times as big as the programmed dimensions. A value of 1.0000 is assumed if nothing is
input.
Dwell Request: Allows you to input a dwell at the bottom of a drill bolt hole or bore
cycle for events you select. Select the appropriate YES or NO soft key. If you select
YES you will be prompted to input a dwell time in seconds from .1 to 99.9 when
appropriate to the event being programmed.
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.
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.
The comment you insert will appear in the RUN mode on the screen just above the X
position dimension 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
35
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
.
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.
Dimension Definition: The ProtoTRAK SM CNC gives you a choice in programming either
tool path or geometry. Part Geometry programming allows you to define the geometry you
want your part to have and then the CNC does the difficult job of calculating tool path for
you automatically. This is a great benefit for most parts most of the time because it means
that the CNC is doing the hard work of determining tool position.
One restriction to part geometry programming is that for events to be connective, they
must lay on the same vertical plane (see Section 5.3 for a definition of vertical planes).
For this reason, the ProtoTRAK SM 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 Haas standard RS274.
A program must be entirely written in Part Geometry or Tool Path programming, you
cannot combine the two methods in one program.
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.
7.4
Auxiliary (AUX) Functions
The ProtoTRAK SM 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.
36
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
.
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:
Input: Function
Comments
0
None
No Auxiliary functions will begin when this event begins to run.
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.
AUX END options:
None
No Auxiliary functions will turn off at the end of this event.
Coolant/Air
Turns the coolant or air solenoid off at the end of this event.
Off
Pulse Indexer Activates a 0.3 second electronic pulse at the end of this event. See note
below.
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.
0
1
3
4
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 SM 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 SM 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 SM 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
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.
37
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
.
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 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 SM 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
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.
38
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
.
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
FIGURE 7.8 Soft keys used while programming an event
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 SM CNC, an Event is a geometry, or a feature of a part.
FIGURE 7.9.1 The header screen has been completed and is on the left side. Select an event type
from the soft keys
39
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
.
When the MORE soft key is selected, the soft keys change to:
FIGURE 7.9.2 When the More soft key is selected, these additional event types are available
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.
FIGURE 7.9.3 Here, a Bolt Hole event was selected. The ProtoTRAK SM CNC is prompting you to enter the
number of holes
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 SM 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).
40
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC 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 SM 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.
6: shifts drawing down.
5: shifts drawing up.
3: shifts drawing to the left.
4: 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.
41
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
.
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.
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 SM 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
The ProtoTRAK SM 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. Many 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 SM 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.
EVENT 1
DRILL OR BORE
# HOLES
X CENTER
Y CENTER
Z RAPID
Z END
RADIUS
ANGLE
# PECKS FOR DRILL
Z REEDRATE
TOOL #
BOLT HOLE
EVENT 1
BOLT HOLE
# HOLES
X CENTER
Y CENTER
RADIUS
ANGLE
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.
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.
Rather than duplicate needlessly, this manual will define all programming in three-axis.
This will serve to explain all issues in programming. For two-axis programming, some
event types and prompts do not appear.
42
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
8.0 Program Mode
Part 2: Program Events
Events are fully defined pieces of geometry. By programming events, you tell the ProtoTRAK SM
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: 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
Tool # is the tool number you assign. SET will use the tool number of the previous event.
8.2
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: the factory setting is for each peck to be successively smaller, taking the
largest cuts at the beginning and the smallest at the end. When the highlight is on this
prompt, you may change this setting by pressing the HELP key. This will take you to a
screen where you may choose to have the same amount of material taken per peck.
Z Feedrate: is the drilling feedrate
Tool #: is the tool number you assign
43
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
8.3
BOLT HOLE Events
This event allows you to program a bolt hole pattern without needing to compute and
program the position of each hole.
Prompts for the Bolt Hole event:
Drill=1, Bore=2: selects whether the hole is to be drilled or bored
# 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.
# PECKS: the factory setting is for each peck to be successively smaller, taking the
largest cuts at the beginning and the smallest at the end. When the highlight is on this
prompt, you may change this setting by pressing the HELP key. This will take you to a
screen where you may choose to have the same amount of material taken per peck.
Z Feedrate: is the drilling feedrate
Tool #: is the tool number you assign
8.4
MILL Events
This event allows you to mill in a straight line from any one XYZ point to another, including
at a diagonal in space. It may be programmed with a CONRAD if it is connective with the
next event (this next event must lie in the same plane as the Mill event).
Prompts for the Mill event:
X Begin: is the X dimension to the beginning of the mill cut
Y Begin: is the Y dimension to the beginning of the mill cut
Z Rapid: is the Z dimension to transition from rapid to feed
Z Begin: is the Z dimension to the beginning of the mill cut
X End: is the X dimension to the end of the mill cut; incremental is 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
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.
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 150, or
mm/min from 5 to 3810
Tool #: is the tool number you assign
44
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
8.5 ARC Events
This event allows you to mill with circular contouring any arc (fraction of a circle) that lies
in the XY plane or a vertical plane (see Section 5.3). Vertical plane arcs are also limited
to those that are entirely concave or convex (in other words, if you think of the arc lying
on the surface of the earth, then it can't cross the equator).
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 SM 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
Z Begin: is the Z dimension to the beginning of the arc cut
X End: is the X dimension to the end of the arc cut; incremental is from X Begin
Y End: is the Y dimension to the end of the arc cut; incremental is from Y Begin
Z End: is the Z dimension to the end of the arc cut; incremental is from Z Begin
X Center: is the X dimension to the center of the arc; incremental is from X End
Y Center: is the Y dimension to the center of the arc; incremental is from Y End
Z Center: is the Z dimension to the center of the arc; incremental is from Z End
Conrad: is the dimension of a tangential radius to the next event (which must lie in the
same plane)
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction of the arc
as viewed looking down for an arc in the XY plane, looking from the front for a vertical
plane, or looking from the right for a vertical YZ plane
Tool Offset: is the selection of the tool offset to right (input 1), offset to left (input 2),
or tool center--no offset (input 0) relative to the programmed edge and direction of tool
cutter movement and as projected in the XY plane
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 150, or
mm/min from 5 to 3810
Tool #: is the tool number you assign
45
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
8.6
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.
8.6.1 Circular Pocket
Press the CIRCLE PCKT soft key if you wish to mill a circular pocket.
Prompts for the circle pocket:
X Center: is the X dimension to the center of the circle
Y Center: is the Y dimension to the center of the circle
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension at the bottom of the pocket; incremental is from the previous event
Radius: is the finish radius of the circle
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling
# Passes: number of cycles to machine to the final depth spaced equally from Z Rapid
to Z End (hint: keep Z Rapid small)
Entry mode: choose between a zigzag ramp and a plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See Section 8.6.5 for more information about the zigzag ramp.
Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut. See
Section 8.6.7 for a bottom finish cut.
Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign
8.6.2 Rectangular Pocket
Press RECTANGLE soft key if you wish to mill a rectangular pocket (all corners are 90o
right angles and the sides are parallel to the X and Y axes).
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
46
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
X3: is the X dimension to the corner opposite X1; incremental is from X1
Y3: is the Y dimension to the same corner as X3; incremental is from Y1
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension at the bottom of the pocket; incremental is from the previous event
Conrad: is the value of the tangential radius in each corner
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling
# Passes: is the number of cycles to machine to the final depth spaced equally from Z
Rapid to Z End (hint: keep Z Rapid small)
Entry mode: choose between a zigzag ramp and a plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See Section 8.6.5 for more information about the zigzag ramp.
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut. See
Section 8.6.7 for a bottom finish cut.
Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
Fin Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign
8.6.3 Irregular Pocket
Press the IRREG PCKT soft key if you wish to mill a pocket other than a rectangle or
circle. The Irregular Pocket event gives you the powerful Auto Geometry Engine to
define a shape made up of straight lines (Mills) and arcs.
The first screen in an irregular pocket event will define the beginning point and some of
its general parameters. The last event of the irregular pocket must end at the same
point as defined in the first event.
X Begin: is the X dimension of the beginning of the pocket
Y Begin: is the Y dimension of the beginning of the pocket
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension of the depth of the pocket.
# Passes: is the number of cycles to machine to the final depth spaced equally
from Z rapid to Z end (hint: keep Z Rapid small)
Entry mode: choose between a zigzag ramp and a plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See Section 8.6.5 for more information about the zigzag ramp.
Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
Fin Cut: is the width of the finish cut. If 0 is input there will be no finish cut. See
Section 8.6.7 for a bottom finish cut.
Fin Feedrate: is the finish cut milling feedrate in in/min from .1 to 150, or mm/min
from 5 to 3810
47
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Tool #: is the tool number you assign
When the initial screen is complete, you will define the perimeter of the pocket with a
series of A.G.E. Mills and A.G.E. Arcs. Programming with the Auto Geometry Engine is
explained in Section 9.0.
No islands may exist in an irregular pocket.
8.6.4 Tool Path in Pocket Events
In Program Run, the pocket path will be either the plunge or zigzag cuts to Z depth along
either the X or Y, followed by the required number of cuts to clear out the interior
material, and then the rough cut along the inside of the perimeter. This will be repeated
for each pass and then followed by a finish pass (if FIN CUT was not zero) along the
inside of the perimeter at the Finish Feedrate and final depth. If a bottom finish cut was
programmed, it will be machined before the perimeter finish cut.
Whether the cuts to clear the interior material of the irregular pocket are along the X or
Y-axis depends on if there are hidden areas of the pocket. The ProtoTRAK SM CNC
always looks to cut along the X-axis first. If there are areas that are hidden to the Xaxis, it will machine along the Y-axis. If there are hidden areas that cannot be machined
continuously in the X or Y-axis, the tool will return to Z retract and then reposition to
machine the hidden area.
8.6.5 Zigzag Z Depth Cuts
In programming pocket events, you have a choice to program the cuts to Z depth either
as a plunge or a zigzag ramp. For rectangular and circular pockets, the tool will start in
the center of the pocket. For irregular pockets, since there is no center defined, the tool
will start in the lower left corner of the pocket. The direction of the ramp will be the
same as the initial direction in either X or Y, depending on how the pocket is to be cut.
The tool will zigzag back and forth along the X or Y over a length of one tool radius while
at the same time moving in the Z direction. When it travels one tool radius along this
direction, it will have traveled a distance of ten percent of the tool diameter along the Z.
This works out to roughly ramping into the part at an angle of 11 degrees.
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 SM CNC will give an error message
during program run and will then default to plunge. This will occur for each pass of the pocket
depth.
8.6.6 Conrad in Pocket Events
A conrad may be added to the last event of an Irregular Pocket. The conrad will be inserted
between the end of the last event and the beginning of the next event.
8.6.7 Bottom Finish Cut
The standard finish cut is along the walls of the part, but you may have the ProtoTRAK
machine a finish cut along the bottom as well. When the highlight is on the Fin Cut
prompt, the blue ? appears next to the Help key. Pressing help gives you the ability to
48
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
choose a Finish cut in Z. You can remove the bottom finish cut by placing the highlight
on the Fin Cut prompt and pressing Help again. When you select Yes to the bottom
finish cut, the following prompt will appear:
Z FIN CUT: the finish cut at the bottom.
8.7
Islands
Within the Pocket event choices, you may also select a circular, rectangular or irregular
island. An island is a shape that is left standing when the surrounding material is
removed. The ProtoTRAK gives you the ability to machine almost any shape as an island
within a rectangular pocket. Both the shape of the island and the dimension of the
surrounding pocket are defined within the island event.
The tool path for machining the island event is that the tool will first plunge or ramp into
the material next to the island, offset by the programmed finish cut, to the depth of the
first pass. The tool will machine the perimeter of the island, offset by the island finish
cut. Then the tool will machine the material in the pocket in a spiral path, moving away
from the island in the programmed clockwise or counterclockwise direction. It will
continue this outward spiral motion until it encounters the programmed rectangular
perimeter (or pocket). It will then follow the perimeter, offset by the pocket finish cut.
It will proceed in this manner through the number of programmed passes. On the final
pass, it will machine the island finish cut, then the pocket finish cut. If a Z finish cut is
programmed, it will do this in the same spiral pattern as the roughing passes between
machining the island and pocket finish cuts. The tool will ramp away from the finish cut
by the amount of the finish cut before it raises out of the part.
8.7.1 Circular Island
Press the Circle Island soft key if you wish to mill a circular island.
Prompts for the Circle Pocket:
X CENTER: is the dimension of the center of the Island
Y CENTER: is the dimension of the center of the Island
Z RAPID: is the Z dimension of the transition from rapid to feed
Z END: is the Z dimension at the bottom of the pocket; incremental is from the previous event
RADIUS: is the finish radius of the Island
DIRECTION: is the milling direction, clockwise or counterclockwise
#PASSES: the number of roughing passes to the depth
ENTRY MODE: choose between zigzag ramp and plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See the previous section for more information about the zigzag ramp.
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.
49
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
X3 POCKET: X dimension for the opposite corner of the rectangular pocket that
surrounds the island.
Y3 POCKET: Y dimension for the opposite corner of the rectangular pocket that
surrounds the island.
CONRAD PCKT: the value of the tangential radius in the corners of the rectangular
pocket that surrounds the island.
FIN CUT PCKT: finish cut along the perimeter of the pocket. If 0 is input, there will be
no finish cut. See the previous section for a bottom finish cut.
Z FEEDRATE: is the Z feedrate from Z rapid to Z end.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts
TOOL #: is the tool number you assign.
8.7.2 Rectangular Island
Press the RECT ISLAND softkey if you wish to machine a rectangular island.
Prompts for the RECT ISLAND:
X1 ISLAND: X dimension for one corner of the rectangular island.
Y1 ISLAND: Y dimension for one corner of the rectangular island.
X3 ISLAND: X dimension for the opposite corner of the island.
Y3 ISLAND: Y dimension for the opposite corner of the island.
Z RAPID: is the Z dimension of the transition from rapid to feed
Z END: is the Z dimension at the bottom of the pocket; incremental is from the previous event
CONRAD ISL: the value of the tangential radius in the corners of the island.
DIRECTION: is the milling direction, clockwise or counterclockwise
#PASSES: the number of roughing passes to the depth
ENTRY MODE: choose between zigzag ramp and plunge. The plunge will machine
straight down Z to the appropriate Z depth. The zigzag ramp will move in a zigzag
pattern to depth. See the previous section for more information about the zigzag ramp.
FIN CUT 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.
50
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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 150, or mm/min from 5 to 3810
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts
TOOL #: is the tool number you assign.
8.7.3 Irregular Island
Press the IRREG ISLAND key if you wish to mill an island other than a rectangle or circle.
The Irregular Island gives you the powerful Auto Geometry Engine to define a shape
made up of straight lines and arcs.
The first screen in an Irregular Island event will define the beginning point and some of
its general parameters. The last event of the irregular 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.
Z FEEDRATE: is the Z feedrate from Z rapid to Z end.
XYZ FEEDRATE: the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
FIN FEEDRATE: the finish milling feedrate for both the island and pocket finish cuts
TOOL #: is the tool number you assign.
51
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
When the initial screen is complete, you will define the perimeter of the island with a
series of A.G.E. Mills and A.G.E. Arcs. Programming with the Auto Geometry Engine is
explained in Section 9.0.
8.8
PROFILE Events
This event allows you to mill around the outside or inside of a circular or rectangular frame or an
irregular profile. The irregular profile may be closed or open. All profiles are limited to the XY plane.
When the irregular profile event is started the ProtoTRAK SM CNC will automatically initiate the
powerful Auto Geometry Engine. See Section 9.0 for programming with A.G.E.
8.8.1 Circle profile
Press the CIRCLE soft key if you wish to mill a circular frame.
Prompts in the Circle Profile event:
X Center: is the X dimension to the center of the circle
Y Center: is the Y dimension to the center of the circle
Z Rapid: is the Z dimension to transition from rapid to feed
Z End: is the Z dimension to the bottom of the frame; incremental is from the previous event
Radius: is the finish radius of the circle
Direction: is the clockwise (input 1), or counterclockwise (input 2) direction for milling
Tool Offset: is the selection of the tool offset to the right (input 1), offset to the left
(input 2), or tool center--no offset (input 0) relative to the programmed edge and
direction of the cutter movement
# Passes: is the number of cycles to machine to the final depth spaced equally from Z
Rapid to Z End (hint: keep Z Rapid small)
Fin Cut: is the width of the finish cut. If 0 is input, there will be no finish cut
Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
Finish Feedrate: is the milling feedrate for the finish cut
Tool #: is the tool number you assign
8.8.2 Rectangular Profile
Press the RECTANGLE soft key if you wish to mill a rectangular frame (all corners are
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
52
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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
Z Feedrate: is the Z feedrate from Z rapid to Z end
XYZ Feedrate: is the milling feedrate in in/min from .1 to 150, or mm/min from 5 to 3810
Fin Feedrate: is the milling feedrate for the finish cut (if programmed).
Tool #: is the tool number you assign
8.8.3 Irregular Profile
Press the IRREG PROFILE soft key if you wish to mill a profile other than a rectangle or
circle. The Irregular Profile event gives you the powerful Auto Geometry Engine to
define a shape made up of straight lines (Mills) and arcs.
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 150, or mm/min from 5 to 3810
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 150, or mm/min
from 5 to 3810
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 7.8.
53
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
8.9
Helix Events
The Helix Event is found after you press the MORE softkey from the Select Event screen.
It allows you to machine in a circular path in the XY plane while you simultaneously
move the Z-axis linearly.
Press the HELIX soft key.
X Center: is the X dimension to the center of rotation of the helix
Y Center: is the Y dimension to the center of rotation of the helix
Z Rapid: is the Z dimension to transition from rapid to feed
Z Begin: is the Z dimension to the beginning of the helix
Z End: is the Z dimension at the end of the helix
Radius: is the radius from the center of rotation to the helix
Angle: is the angle from the positive X axis (that is, 3 o'clock) to the starting position of the helix
# Rev: is the number of revolutions in the helix, for example, 0.75 would be
270 degrees, or 3.25 would be three times around plus 90 degrees
Direction: is the clockwise (input 1) or counterclockwise (input 2) direction of the helix
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
XYZ Feedrate: is the feedrate from beginning to end in in/min from .1 to 150, or
mm/min from 5 to 3810
Tool #: is the tool you assign
8.10 Subroutine Events
The Subroutine Events are used for manipulating previously programmed geometry
within the XY plane.
The Subroutine Event is divided into three options: Repeat, Mirror, and Rotate.
Repeat and Rotate may be connective. As long as the rules of connectivity are satisfied
(see Section 5.9), the ProtoTRAK SM CNC will continue milling between preceding and
subsequent events.
REPEAT allows you to repeat an event or a group of events up to 99 times with an
offset in X and/or Y and/or Z. This can be useful for drilling a series of evenly spaced
holes, duplicating some machined shapes, or even repeating an entire program with an
offset for a second fixture.
Repeat events may be "nested." That is, you can repeat a repeat event, of a repeat event, of
some programmed event(s). One new tool number may be assigned for each Repeat Event.
MIRROR is used for parts that have symmetrical patterns or mirror image patterns. In
addition to specifying the events to be repeated, you must also indicate the axis or axes
(X or Y or XY are allowed) that the reflection is mirrored across. In addition, you must
specify the offset from absolute zero to the line of reflection. You may not mirror
another mirror event, or mirror a rotate event. Consider the figure below:
54
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
FIGURE 8.10.1 Holes 1-4 are mirrored across the Y axis to 5-8, respectively, about a line X OFFSET from
X=absolute 0
ROTATE is used for polar rotation of parts that have a rotational symmetry around some
point in the XY plane. In addition to specifying the events to be repeated, you must also
indicate the absolute X and Y position of the center of rotation, the angle of rotation
(measured counterclockwise as positive; and clockwise as negative), and the number of
times the specified events are to be rotated and repeated. You may not rotate another
rotate event, or rotate a mirror event. Consider the figure below:
FIGURE 8.10.2 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.
55
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
8.10.1
Repeat
Press the REPEAT soft key.
Where:
First Event #: is the event number of the first event to be repeated
Last Event #: is the event number of the last event to be repeated; if only one event is
to be repeated, the Last Event # is the same as the First Event #
X Offset: is the incremental X offset from event to be repeated
Y Offset: is the incremental Y offset from event to be repeated
Z Offset: is the incremental Z offset from event to be repeated
Z Rapid Offset: is the incremental Z rapid offset from event to be repeated
# Repeats: is the number of times events are to be repeated up to 99
% Feed: the percentage of the feeds programmed in the repeated events. 100% is assumed
Tool #: is the tool number you assign
8.10.2
Mirror
Press the MIRROR soft key.
First Event #: is the event number of the first event to be mirrored
Last Event #: is the event number of the last event to be mirrored; if only one event is
to be mirrored, the last event is the same as the first.
Cutting Order: input 1 to cut from the lowest mirrored event to the highest (forward)
and 2 to machine from the highest mirrored event to the lowest (backward).
This way you can keep all the machine motion in a consistent direction as it moves from
the original shape to the mirrored shape and keep all cutting either climb or
conventional.
Mirror Axis: is the selection of the axis or axes to be mirrored (input X or Y or XY, SET)
X Offset: is the distance from Y absolute 0 to the Y-axis line of reflection
Y Offset: is the distance from X absolute 0 to the X-axis line of reflection
8.10.3
Rotate
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
56
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
8.11 COPY Events
Copy Events are programmed exactly like Subroutine Events. The only difference is that
in Copy the events are rewritten into subsequent events. If, for example, in event 11
you Copy Repeated events 6, 7, 8, 9, 10 with 2 repeats, events 6-10 would be copied
with the input offsets into events 11-15, and recopied into 16-20.
Copy Events may be Repeat, Mirror, 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, 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.
Figure 8.11 In the above example, the offset that puts the group of holes in the desired
location is X=-1.50 and Y=-1.00.
8.12 Thread Mill Event
To program a Thread Mill event press the Thread mill soft key. This event includes an
automatic move in and out by 0.050” of the thread. Prompts in the Thread Mill event:
X CENTER: the X dimension of the center of the thread
Y CENTER: the Y dimension of the center of the thread
Z RAPID: the Z dimension where the Z rapid feed slows to Z program feed
Z BEGIN: the Z dimension where the threading pass begins
57
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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 inch. For example, the pitch for a 1/4-20 screw is
1 ÷ 20 = .05 inches
MAJOR DIA: the largest diameter of the thread (the root for an ID thread, the crest for
an OD thread)
MINOR DIA: the smallest diameter of the thread (the root for an OD thread, the crest
for an ID thread)
SIDE: input 1 for inside, 2 for outside
ANGLE: the angle the tool feeds into the beginning depth
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.
8.13 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 activate an indexer (Section
7.4), 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.
8.14 Engrave Event
The Engrave Event allows you to machine numbers, letters and special characters as part
of a part program. See Figure 8.14 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
58
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
able to see 20 characters on the prompts screen). To machine text in a direction other
than the X axis, simply use multiple Engrave Events and place the lower left corner of the
box wherever you would like. The numbers and letters you program will always have a
standard orientation (like the letters on this page) – you cannot program tilted or
inverted letters with the Engrave Event. The letters are of the font shown in the figure
and all capitals.
Prompts for the Engrave Event:
First, define the lower left corner of the box that will contain your text:
X BEGIN: The X coordinate of where you want your text to begin
Y BEGIN: The Y coordinate of where you want your text to begin
Z RAPID: The Z dimension where the Z rapid feed slows to Z program feed
Z END: The Z dimension to the bottom of your text.
HEIGHT: The height of your text. Each character varies in width; the set height of the
character will change the width in order to keep the overall size of the character
proportional.
TEXT: The text to be milled. When you get to this prompt, the Alpha keys will
automatically pop up to allow you to enter the text. Once you have finished entering
text, you must press End (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.
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
Figure 8.14 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.
59
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
8.15 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 - for two-axis operation, the Position and Drill event types are combined.
See Section 8.1 for a description of Position event prompts.
TEACH DRILL- this may also be made into a bore event. See Section 8.2 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 8.4 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.
60
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
9.0 Program Mode
Part 3: The Auto Geometry Engine (A.G.E.) Programming
When you program an Irregular Pocket (Section 8.6.3) or an Irregular Profile (Section 8.7.3) the
Auto Geometry Engine, or 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 SM CNC. It is treated in its own section because it works differently than the other
event types. Unlike other events, the A.G.E. allows you to:
•
•
•
Enter the data you know, and skip the prompts you don’t.
Use different types of data (like angles) that may be available from the print.
Enter guesses for the X and Y ends and centers not available on the print.
With the A.G.E., you can easily overcome limitations in the data the print provides without having
to spend time in laborious calculations.
9.1
Starting the A.G.E.
The A.G.E. is started automatically when you enter the Irregular Pocket or Irregular
Profile event. The first set of prompts you encounter will be the header information.
Once that information is entered, you will see the following screen:
FIGURE 9.1 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
Where:
A.G.E. Mill: A straight line from one X Y point to another.
A.G.E. Arc: Any part of a circle.
61
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
End A.G.E.: Ends the A.G.E. programming for the Irregular Pocket or Irregular Profile.
Abort A.G.E.: Aborts all A.G.E. events. The data for all the events is lost.
9.2
A.G.E. Mill Prompts
Press the A.G.E. Mill key.
FIGURE 9.2 A.G.E. Mill prompts. Enter what you know, skip or guess the ones you don’t
Prompts in A.G.E. Mill programming:
Tangent: this refers to the tangency of the mill to the previous event. See Section 9.11
for a discussion of tangency.
X END: is the X dimension to the end of the mill cut; incremental is X Begin
Y END: is the Y dimension to the end of the mill cut; incremental is Y Begin
CONRAD: is the dimension of a tangential radius to the next event
ANGLE END: is the angle measured counterclockwise from this mill event to the next.
Do not input if the next event is an arc
LENGTH: is the length of the mill from beginning to end
LINE ANGLE: is the angle of this mill line (moving from begin to end) measured
counterclockwise from the positive X axis (that is 3 o’clock)
GUESS: This softkey will appear when the prompt is on X or Y dimensioned data. Press
the Guess key before you press INC SET or ABS SET to enter the data as a guess. See
Section 9.7
62
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
9.3
A.G.E. Arc Prompts
Press the A.G.E. ARC key.
Prompts in A.G.E. Arc programming:
Tangent: this refers to the tangency of the mill to the previous event. See Section 9.11
for a discussion of tangency.
DIRECTION: is the clockwise (input 1), or counterclockwise (input 2) direction of the arc
X END: is the X dimension to the end of the arc cut; incremental is from X Begin
Y END: is the Y dimension to the end of the arc cut; incremental is from Y Begin
X CENTER: is the X dimension to the center of the arc; incremental is from X End
Y CENTER: is the Y dimension to the center of the arc; incremental is from Y End
CONRAD: is the dimension of a tangential radius to the next event
RADIUS: is the radius of the arc
CHORD LENGTH: is the straight line distance from the begin point to the end point
CHORD ANGLE: is the angle spanned by the arc
In addition to the normal Softkeys, this additional one will appear in A.G.E. Arc
programming:
GUESS: this softkey will appear when the prompt is on X or Y dimensioned data. Press
the Guess key before you press INC SET or ABS SET to enter the data as a guess. See
Section 9.7
9.4
Skipping Over Prompts
In the A.G.E., events don't have to be fully defined before you can go to the next one.
You can skip the data you don’t know by using the 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.
9.5
The OK/NOT OK Flag
Each A.G.E. event has a flag that tells you if it has been fully defined. Sometimes data
from later events is needed to define previous events. To the immediate right of the
event 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.
63
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
9.6
Ending A.G.E.
Any time all the events are of an Irregular Profile are OK, the A.G.E. may be ended. If
you are programming an Irregular Pocket, there is an additional requirement that must
be satisfied before the A.G.E. may be ended: the X and Y end point of the last event
must be the same as the X and Y beginning point, so that the pocket is closed.
Otherwise, the ProtoTRAK SM CNC cannot program the tool path to clear the pocket.
The Irregular Profile has no such restriction since profiles may be open or closed.
Once the A.G.E. is ended, the Irregular Pocket or Irregular Profile event is complete and
you may then choose from all the programming canned cycles from the Select an Event
screen. To reopen the A.G.E. Profile or Pocket, simply use the 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.
9.7
Guessing Data
Whenever you are missing X or Y Ends or Centers, you should generally enter a guess.
Guessed data is treated differently by the ProtoTRAK SM 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.
FIGURE 9.7 The X End dimension has been entered as a guess—note the letter G
Guesses should always be entered as absolute dimensions. Once entered, the guessed
data 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
64
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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.
9.8
LOOK and Guess
Guessed data may be entered by pressing the number keys and then SET. However, you
may find it more convenient to use the LOOK graphics to enter guesses.
When 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.
Figure 9.8.1 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.
65
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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.
FIGURE 9.8.2 When the events are calculated based on Guessed data, they are represented by a dotted line
9.9
Calculated Data
Prompts that are skipped or for which guesses are entered may be replaced by data
calculated by the ProtoTRAK SM CNC. Calculated data is shown in red in order to
distinguish it from the data that you entered. You cannot edit calculated data, but you
may edit your original input. By putting the event with the calculated data on the right
side of the screen, you may position the cursor to the prompt and re-input the data.
9.10 Arcs and Conrads
If the print is missing a lot of data, it may be desirable to program arcs as separate
events where possible. This gives the system more information to work with.
9.11 Tangency
Tangency can occur between a mill and arc or an arc and arc. Specifically it means that
the two events share one and only one point. You would answer yes to the TANGENCY
prompt if the event you are programming is tangent to the previous event. The
66
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
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 are assumed to continue in the same direction,
and not double back on the previous event:
like this
not this
67
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
68
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
10.0
Edit Mode
Within Program Mode, you can recall and re-input specific data prompt by prompt. The Edit
Mode contains powerful routines for more extensive program changes.
The changes you make in the Edit Mode affect only the program in current memory. In order to
preserve the changes for future use, the program must be stored again under the same name in
the In/Out Mode.
10.1 Delete Events
To delete a group of events in the program, press Delete Events.
The Data Input Line will prompt for the first event to be deleted. Input the event
number of the first event and press set. Next the Data Input Line will prompt for the last
event number to be deleted. Put in the last number and press Set.
The remaining events will be renumbered.
10.2 Spreadsheet Editing

Spreadsheet Editing allows you to view program inputs in a table and make global
changes to the program. This is particularly useful if you are working with a large
program and you need to make a change to many events.
When you press the SEARCH EDIT softkey, the screen will load a table that contains data
for every event. See Figure 10.2.1
FIGURE 10.2.1 The Search Edit softkey launches Spreadsheet Editing. View the entire program by the
variables you select
69
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
The first time the screen appears, the data is sorted by event number. Each row
represents the data for the event number shown in the first column on the left. The
event number is always displayed in the first column, but the other data displayed on the
table can be changed.
Soft Keys in Search Edit:
PAGE FWD: pages forward through the table.
PAGE BACK: pages backwards through the table.
6534: highlights data for editing. Only data that is highlighted and appears in the
Data Input Line may be edited. Note: the EVT# (event number) and (event) TYPE may
not be edited in Search Edit so the highlighter will not go there.
SORT: enables you to change the sort to any of the data displayed. See Section 10.2.2
CHANGE ALL: enables you to make global changes of data. See 10.2.3
10.2.1
Selecting Data to be Displayed on the Search Edit Table
In order to change the data selected in the table, press the HELP hard key. There will be
a listing of all the data types that may be edited in Search Edit. Press the RETURN soft
key and the table will be reloaded with the data that you selected.
FIGURE 10.2.2 Pressing Help while viewing the spreadsheet lets you change the program parameters
70
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
After you press the HELP hard key, the screen will display all the different parameters
that can be displayed on the spreadsheet. To either select or deselect any parameter,
simply highlight that parameter and press SET. When you are finished, press the Return
softkey and return to the spreadsheet.
10.2.2
Sorting Data
Data may be sorted by any of the data types displayed in the column head. Red letters
show which column is used for sorting the data.
To change the sort, press the SORT softkey, then select the type of data you want to use
for sorting from the softkeys.
The table will be changed to sort the data in ascending order (the smallest value first, the
largest last).
10.2.3
Making Global Changes to Data
Sometimes it is useful to be able to change data in a program without having to go
through each event one at a time. For example, if you were to want to change the tool
number for every milling event, it may be a chore to go through each event in a long
program to make the changes on that event type.
In order to make global changes:
1. Sort the data in a way that groups together the things you want to change.
2. Highlight the data value that is highest on the table (nearest to the top) that you
want changed.
3. Press the CHANGE ALL softkey. All the inputs that are the same as the one you
highlighted and are listed together below the data you highlighted will then be
highlighted.
4. Enter the new value, then press set. All the highlighted data will be changed to the
value you just input.
Example:
From the screen shown in Figure 10.2.1, we will change the Z Feed for each of the mill
events in the program.
1. Sort by event type to get all the Mill events together.
2. Highlight the Z Feed in the first Mill event (Event # 8). See Figure 10.2.3
3. Press the CHANGE ALL softkey. All the Z Feeds in the Mill events are highlighted.
See Figure 10.2.4
4. Type in the new Z Feed value and press INC SET or ABS SET. See Figure 10.2.5
71
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
In this example, the Z feed is changed from 5.0 to 7.0 for all the Mill Events.
FIGURE 10.2.3 After sorting by Event Type, the highlighter is placed on the Z feed of the first Mill Event
FIGURE 10.2.4 Pressing the Change All softkey highlights the Z feed for all the Mill events
72
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
FIGURE 10.2.5 Type the new Z Feed and then SET to change all the highlighted values from 5 to 7.
10.3 Erase Program
Use the ERASE PROG soft key to erase the program from the current memory. Erasing
the program from current memory will not affect any programs that are stored.
If you have made changes to the program and wish to save this modified program, you
will need to store it. See Section 13.4
10.4 Clipboard
The Clipboard feature is a way to copy events in one program in order to put them into a
different program. It is a two-part process that takes place in two different Modes. First,
in the Edit Mode, the desired events are copied, or placed on the Clipboard, from the
source program. Then the events are inserted into the destination program in the
Program Mode.
When you press the Clipboard key from the Edit Mode, you start the process that copies
the events that you want to put into a different program than the one in current memory.
Before you do that, you should write a program or open the program file that has the
events you want to copy. This is called the source program.
Inspect the events you want to copy. Make sure that the dimensioned data uses
Absolute references in the first event to be copied and in all events where it will be
important. Incremental references may be used, but keep in mind where the
Incremental reference will be made from. See the section on Incremental Reference
Position in this manual.
73
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
In addition, you may want to modify this program in order to get all the events you want
together. For example, if you want to copy events 2-5 and 7-12, you may want to
modify the program to delete events 1 and 6 first. That way, you can copy the all the
events as they are now numbered from 1 to 10. Remember that you can modify this
program just for this purpose and it will not affect the original program unless you save it
with the modifications in the Program In/Out Mode.
When the source program is ready, press the CLIPBOARD softkey. A message will
appear that says "Copy Events Onto Clipboard" and the Data Input Line will read "From
Event". Enter the number of the first event that you want copied and press SET.
The Data Input Line will read "To Event". Enter the number of the last event you want
copied and press SET.
The group of events that you have specified is now on the clipboard and will remain
there until you replace it with something else by going through the same procedure.
When power is turned off to the CNC the clipboard information will also be lost.
The events on the clipboard are inserted into a program in the Program Mode. See
Section 8.10.
74
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
11.0
Set Up Mode
The Set Up Mode contains the tool library, the tool path graphics and the machine's reference positions.
Enter the Set-Up Mode by pressing the SET-UP soft key at the Select Mode screen.
FIGURE 11.0 The Set-Up mode
11.1 The Tool Table
From the screen above, press the TOOL TABLE softkey.
FIGURE 11.1 The Tool Table
75
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
11.1.1
The Tool Table Screen
When you first enter the tool table by pressing the TOOL TABLE soft key, you will see the
screen shown in Figure 11.1.
Tool #: the number of the tool from 1 to 99. Tool numbers shown in red are active for
the program in current memory.
Diameter: the diameter of the tool.
Z Offset: the difference between the Z position of the tool and the Z position of the
reference. The Z offset is always relative to a reference point. Before the reference
point is set, the highlight will not go into the Z Offset column because setting a Z offset
before the Z reference is set has no meaning.
Z modifier: a value you enter to make adjustments for the tool depth. See 11.1.7 below.
Ref: the reference position for the Z offset. Before the reference position is set (and the
Ref row reads "NOT SET") the highlight will not go into the Z Offset column. Once it set,
the highlight will not go into the Ref row, that is, you will not be able to highlight and
reset your reference once it says "SET".
The soft keys in the tool table:
DATA DOWN, DATA UP, DATA LEFT, DATA RIGHT: move the highlight around the table.
ERASE TABLE: clears all tool information so you can start over. See 11.1.4 below.
JOG: puts the ProtoTRAK SM CNC into the DRO jog operation (see Section 6.3).
RETURN: reverts to the SET UP mode screen.
The electronic handwheels are active, including the fine/coarse selection, while you are in
the tool table.
11.1.2 The Logic of the Tool Table
The tool table is organized to do the following:
• Make it easy to set up tools.
• Make it easy to replace a tool or add a tool.
• Retain tool information in memory to reduce set-up.
You assign tool numbers as you write a program. These tool numbers may be from 1 to
99. Before machining, the diameters and Z offset of each of the tools in the program
must be defined so that the ProtoTRAK SM CNC can calculate the tool path. Tools that
are used in the program that is in current memory are called active tools and their
numbers are in red in the tool table.
When you save a program, all the tool information for active tools is saved with it. When
the program is opened, the tool information is put into the tool table. This information
will replace any information that already is in the tool table for the same tool numbers.
In addition to information about the tools used in a program, you may load in information
for tools to be used in 2-axis CNC or in the DRO mode for machining manually. When
you tell the ProtoTRAK SM CNC which tool you are using, it will adjust the Z DRO
dimensions accordingly so you don’t have to touch off and reset after a tool change.
The idea of retaining tool information in memory in order to reduce the amount of set-up
needed requires that care be taken to avoid mistakes. Milling work usually requires a lot
of tools, many of which are not preset into fixed tool holders. That means tool
information that is not very recent is probably no good.
76
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Think of the information in the tool table this way: if you clearly remember setting the tools
and entering the diameters very recently, then use the tool table in DRO and CNC run. If
you can't remember setting the tools clearly, erase the table and start over – it only takes a
moment.
This may cause some confusion because the normal sequence for running a two-axis
program is to load in a tool, touch it off and set zero, then press GO. The ProtoTRAK SM
CNC will apply the tool offset after the GO press, making the Z dimension meaningless.
You have two choices:
1. Use the tool table, setting the reference and absolute dimension for one of them per
the instructions above. This will save you from having to touch off tools every time
they are changed in program Run.
2. Don’t use the tool table. Erase the entire tool data so that the ProtoTRAK SM CNC
will not try to apply offsets.
11.1.3
Initial Tool Set-Up
This procedure is used for setting up tools when the tool table is clear.
1.
When you enter this screen for the first time, the words "NOT SET" appear directly under
the Z OFFSET column in the REF row. The Data Input Line reads "TOUCHOFF REFERENCE
POINT". This is prompting you to establish a reference for the rest of your tools.
2.
To establish a reference, put a cutting tool or some other reference setting tool
into the spindle and touch the tool to a surface. We recommend that you use
something besides a tool that you intend to use machining the job. Ideally, you
will have a reference tool that you keep handy for setting up your tools every time.
That way, a reference point can be easily re-established later.
3.
We also recommend that you use the top of the vice or table as your reference
surface because it is constant and never changes.
4.
With the highlight on the screen on the words "NOT SET" and the tool touching some
reference point, press SET.
NOTE: If you do use a tool as your reference tool and it breaks, you must retouch off all tools.
5.
The words will change from "NOT SET" to "SET" and the highlight will shift to the
DIAMETER column of Tool # 1. (Note that you may not be interested in setting up
Tool #1 if it is not one of the active tools of the program. If this is the case, use
the DATA softkeys to move to a tool you are interested in.)
6.
Input the diameter for the tool and press SET.
7.
The highlight will move to the Z OFFSET column. Put this tool in the spindle and
touch it to the same surface as you used to touch the reference tool in Step 2 above.
8.
Press set.
9.
The highlight moves to the Z Modifier column. Input a Z modifier if you wish (see
below) or simply press SET again for the highlight to move to the DIAMETER
column of the next tool.
10. Repeat steps 5 to 8 for each of the tools you want to set up. Remember to touch
the same surface you used to set the reference tool.
Once the reference position is set, you will not be able to move the highlight back to the
word "SET".
77
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Note: You must set an absolute zero reference in the DRO Mode before machining the part. You
may use any tool that you have set up with the above procedure to set your reference and the
ProtoTRAK will automatically compensate for the difference in length for the rest of the tools.
11.1.4
Starting Over: Erasing Tool Information
There will be times when you don't completely trust the information that is in the tool
table. For example, perhaps you have loaded in a program that you wrote a month ago
and you recall that one of the tools you used was held in a chuck. In that case, you
probably want to erase the table and start over.
In order to do this, simply press the ERASE TABLE softkey and answer yes to the prompt.
All the data in the tool table will be erased including the reference. The numbers of the
tools used in any program in current memory will still be red.
11.1.5
Adding a Tool
When the reference is SET and the original touch-off surface is still available, you can add
a tool very easily:
1. First make the tool number active by using it in the program in current memory.
2. Put the new tool in the spindle.
3. Go to the Set-Up Mode, tool table
4. Enter the diameter.
5. Touch the new tool to the same surface as the reference.
6. Press SET.
If the surface is not available, it will be necessary to establish a new reference before
adding the new tool. See Section 11.1.8 below. Once the reference is reset, use the
procedure above on the new surface used to set the reference.
11.1.6
Replacing a Tool
If you need to replace a tool that was not used as the reference, simply do the following:
1. Put the replacement tool in the spindle.
2. Put the highlight in the correct row for the tool number.
3. Reenter the diameter if different.
4. Touch the tool to the same surface that was used to touch off the reference.
5. With the highlight in the Z OFFSET column for the correct tool number, press SET.
If you need to replace a tool that was used as a reference, we recommend that you press
the ERASE TABLE softkey and start all over again. (Not to nag, but that is why it is a
good idea to have a separate reference setting tool and use a constant reference surface.
If you work with programs that use a lot of tools, this practice can really save time.)
11.1.7
Z Modifiers
Z modifiers make it easy to adjust the depth of cut of particular tools without having to
change programmed Z end dimensions or change the tool offsets.
78
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
For example, say an end mill was under cutting the depth of a part by .003". An easy
way to correct this is to enter a Z modifier.
1. Highlight the number in the Z MODIFIER column in the row for the correct tool.
2. Enter the amount of the adjustment you wish to make. To cut deeper, enter a
negative number. To cut shallower, enter a positive number. In the example above,
to correct this undercut, we would enter -.003.
3. Press SET.
The ProtoTRAK SM CNC will apply this modifier each time this tool is used.
11.1.8
Resetting the Reference Point
Once the reference reads SET, you are not allowed to highlight and reset it. If you need
to reset the reference, there are two ways to change the reference to NOT SET. You can
erase the table (and lose all the tool information) or load in a program.
11.1.9
Saving Tool Information
Tool information is saved with the program. If you have made changes to the program
or to the tool table that you wish to keep, you must save, or store, the program in the
Program In/Out Mode.
11.1.10
Opening a Program
When you open a program, the tool information that is saved with the program will be
loaded into the tool table. The numbers for the tools that are used in the program are in
red. The diameters, Z Offsets and Z modifiers that were saved with the program will
overwrite any information that was in the tool table before the program was opened. If
these tools were not set very recently, we recommend that you check them before
running the program.
The Ref row will read "NOT SET". A reference may be set at this point.
If you do not go into the tool table after opening a program and before running, you will
get a reminder message to check your tools.
11.1.11
Making Tool Set-Ups Easy
We highly recommend the following to make tool set-ups easy.
1. Always use the same tool to set your reference. Preferably, you should use a tool
you don’t use to machine, something that you keep in your toolbox.
2. Don’t use a tool that you use to machine your part as a reference. If your reference
tool breaks, you have to reset all your tools.
3. Always use the same surface for touching your tools to. Use the machine table, a
gage block or the vice, something you can always count on being there. If you use
the top of the part, your reference is changing all the time.
11.1.12
The Tool Table and Two-Axis CNC Operation
The information entered in the tool table will also be used when operating the ProtoTRAK
SM CNC as a two-axis CNC. Instead of positioning the head, the DRO information seen in
the Run Mode will be adjusted for the differences in tools. When a new tool is loaded, the
Z dimension will change according to the offsets in the tool table. This change will occur
when the GO key is pressed after the "Load Tool # ___" prompt.
79
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
11.2 Tool Path
When the TOOL PATH soft key is pressed, the program is processed and the tool path
graphics are displayed.
FIGURE 11.2 The Tool Path graphics show the program and tool positions
Most programming errors that would prevent the program from running are detected
when the tool path graphics are selected. For example, if you were to have omitted a
minus sign from a Z End dimension, the system would give you an error message that
the Z End should not be higher than the Z Rapid.
The displayed graphic is automatically sized to fit the screen and an icon that represents
the X, Y and Z orientation is placed at the program's absolute 0 reference point. The path
shown on the screen represents the center of the tool.
• Position and drill events are drawn in yellow.
• Rapid moves are in red.
• Programmed geometry is in blue.
11.2.1
Soft keys in Tool Path
ADJUST VIEW: calls up additional softkeys to adjust the view. See below.
FIT DRAW: will re-draw, automatically sizing to fit the screen (necessary only if an
adjustment changed the drawing from its initial sizing).
STEP: each press of the STEP button shows the next tool move. You may hold the STEP
button down to draw the graphic without repeated button presses. To complete the
drawing automatically, press FIT DRAW.
XY, YZ, XZ, 3D: shows the same drawing on the screen, with adjustments, in the view you select.
80
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Soft keys in ADJUST VIEW:
FIT: same as the FIT DRAW.
6534: moves the drawing in that direction.
ZOOM IN, ZOOM OUT: resizes the drawing.
RETURN: returns to the previous soft keys, retaining the adjustments that were made to
the drawing.
11.3 Reference Positions (REF POSN)
The Reference Positions screen shows the retract status, the home locations and
software limits for all axes.
FIGURE 11.3 Reference positions. The Z Retract is not set. Position the head and press a SET key
11.3.1
Z Retract
The Z Retract is where the head will go for a tool change or at the end of running a
program. Programs may not be run in three-axis CNC until the Z Retract is set. Since
the Z-axis (head) is operated manually in two-axis CNC, it is not necessary to set the Z
retract to run a two-axis CNC part.
As a general rule, always set your Z retract so that your longest tool is above the set-up.
When you first enter the Reference Positions screen, the Z Retract will show "NOT SET"
and the message window will instruct you to move the ram to the desired retract position
and then press SET. You may have to go into the DRO Mode to move the ram to where
you want it and then return to the Reference Positions screen to set this position.
81
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
11.3.2
Home Positions
X and Y home positions are where the table and saddle go when there is a tool change or
at the end of the program. These dimensions must always be from absolute zero. Note
Z home is the same as Z Retract.
11.3.3
Limit Positions
X and Y limit positions (one for plus direction, one for minus) will stop the program if
they are exceeded during run. Note that pressing the LIMIT ON/OFF soft key will turn
the prompted limit off, or back on to its input value. If the limits are turned on, your
program and home positions must fit within the limits you define. If you turn on the
limits and leave them at the default of 0 Absolute, the program will not run.
11.4
Fixture Offsets
Fixture offsets are entered in the Set-Up Mode. From the screen in Figure 11.0, press the
Fix Offset key. The following screen will result.
Figure 11.4 The Fixture Offset screen.
Setting up fixtures is easy. First, establish your base by setting your X, Y and Z absolute
zero. You can do this in the DRO Mode, but the X, Y and Z Absolute position dimensions
are also on this screen for your reference. Fixture #1 is always the base.
Once you set your absolute zero on the base, it is simple a matter of entering the
distance from the base to up to five other fixture locations. You can do this one of two
ways. By entering the numbers with the keypad or by positioning to the next fixture,
putting the cursor on the correct offset value, and then pressing ABS SET.
11.5
Service Codes
These are special codes that may be entered into the ProtoTRAK SM CNC to call up
routines used in installation, setting of preferences, machine checkout and service.
82
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
The following is a summary of the service codes available.
WARNING!
Before using service codes, be aware that some of the routines are very powerful and may
change system settings in a way you don't want. Some of the routines cause
the servos to come on and move at rapid speed.
Category
Software
Service Code
33 software and firmware version
141 load EEPROM file
Machine set-up
Servo calibration
Service code
number
142 save EEPROM file
316 software update – master
317 software update – slave
318 converter activation
37 RS232 Baud rate
123 sensor calibration
132 handwheel test
100 open loop test
129 arc accuracy setting
304 toggle X glass scale or TRAK
sensor on or off
304 toggle Y glass scale or TRAK
sensor on or off
323 RS232 com port
128 backlash calibration constant
127 auto backlash configuration
11 backlash hysteresis test
12 feed forward constant
None
Comments
Displays current software versions and
system settings.
To load in set-up values from a disk in the
floppy drive
To set-up values to a file on a floppy drive
Use with floppy disk
To set for RS232 communication
DANGER! The machine will move!
To enter the preference. Default is .001
Run the machine from the motor encoders
in case of table scale or sensor failure.
Run the machine from the motor encoders
in case of saddle scale or sensor failure.
Change default com port
CAUTION! The servo parameters may
change.
Shortcut to entering the service code
when you know it
83
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
84
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
12.0
RUN MODE
12.1 Run Mode Screen
Press MODE and select the RUN soft key. The display will show:
FIGURE 12.1 The Run Mode. The ProtoTRAK SM CNC awaits your instructions for how to begin
machining Part Number R0424-11
Items on the Run Screen:
Event counter: this will be the current event number and event type.
Repeat: if a repeat event is in the event counter, this will show which repeat number,
for example, if you program a drill with 5 repeats, this will show which repeat of the
event that is being machined.
Feed Rate: programmed feedrate of the current move as adjusted by the feed override.
Green bar: graphical representation of the feed override
Override: % of feed override.
12.2 Two Versus Three-Axis Running
The three-axis run will control all three axes; the two-axis will control the X and Y (table
and saddle) only, with you manually positioning the Z (head).
Most differences that occur as a consequence of either two or three-axis operation are
obvious. Two issues are worth noting:
1. The way the tool table works between two and three-axis operation. See Section 11.1
2. Positioning of the quill is automatic in the 3-axis CNC, but in two-axis, the ProtoTRAK SM CNC
will prompt “Check Z” before a rapid move and “Set Z” for you to position the cutter to the
machine part.
85
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
12.3 Starting to Run
Before running a part, you must establish the position relationship between the part and
quill. That is, you need to identify where the part is on the table relative to the tool or
quill centerline.
This is done by using an edge finder or dial indicator to move the table so that the part
program absolute zero is under the quill centerline. ABS SET this position as absolute
zero in the DRO mode. In addition, load the tool for Event 1 and position it at Z absolute
zero. If this is impossible, position the tool some known distance above absolute zero
and ABS SET this dimension.
The program may be started in the two ways identified as soft keys in the screen in Section 12.1
Pressing the START soft key begins the program at Event 1 and assumes that the
absolute zero that was last set in the DRO mode corresponds to the part program zero.
That is, if you were in the DRO mode and you moved the table to X=0 ABS, and Y=0 ABS
the part program zero would be directly under the quill centerline.
Pressing the START EVNT # soft key allows you to start in the middle of a program.
When you press the START EVNT # soft key, the conversation line will prompt "Input
Event #." Input the number of the first event you wish to run, and press SET. If the
START EVNT # is a Repeat or Rotate, the conversation line will prompt "Starting Repeat
Number" asking which repeat or pass you wish to start.
12.4 Program Run
When you have started by any of the means above, the display will show:
FIGURE 12.4 Press the GO feed key to start running.
86
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Where:
The part number being run is shown in the status line.
•
A "S/F" message will appear in the status line when the Scale Factor is not set at 1.0000
•
The event number and type (and the repeat number, if applicable) being run is
shown at the top of the screen.
•
The current X, Y, Z absolute positions are shown in the information area.
•
The SHOW ABS soft key (which is automatically assumed if one of the other 3 show
keys are not selected) will show the absolute X, Y, Z positions as the part is run.
•
The SHOW INC soft key will show the incremental (or distance to go within the
event) X, Y, Z positions as the part is run.
•
The SHOW PATH soft key will show the tool path graphics as the part is run.
•
The SHOW PROG soft key will show the programmed data for the event being run,
and the next event as the part is run.
The run procedure is very simple. Follow the instructions on the conversation line and
proceed by pressing the GO key.
Once the STOP hard key is pressed, additional softkeys will be available:
12.5 Program Run Messages
During Program Run, all messages that will help you to run the part will appear in the
data input line. The messages you will usually see are:
Load Tool __ __: Means to load the tool requested and press GO to continue.
12.6 Stop
At any time, the program may be halted by pressing the STOP key. This freezes the
program at that point. You may choose to continue running the program by pressing the
CNC RUN softkey or pressing the GO key. You may also run the program by using the
table or saddle handwheels by pressing the TRAKing softkey.
12.7 Feedrate Override
The run feedrate may be changed at any time by pressing the FEED ! or FEED " keys.
Each press modifies the programmed feedrate, as well as rapid by 10%.
12.8 Trial Run
Trial Run allows you to quickly check out your program with no Z movement before you
actually start to make parts. In trial run the table will move at rapid speed regardless of
what feedrates are programmed (the rapid speed may be overridden with FEED ! and
FEED " keys). The table will stop at each "stop" location (for example, at each drill
location) but immediately continue on without your input.
To do a trial run, press the TRIAL RUN soft key from the screen shown in Section 12.1.
The message box will read "Ready to begin trial run. Press GO to start." Be certain the
table is positioned so that if it moves through the part program, it will not reach its travel
limit. Also check that the quill is fully retracted. Press GO to begin.
87
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
12.9
Data Errors
In order to run, a program must make sense geometrically. For example, you can't machine
a .250-inch diameter circular pocket using a .500-inch end mill.
Data errors will nearly always be detected when the ProtoTRAK SM CNC runs through a
program--either as a Trial Run or on an actual part run. They may also be detected in
the Set Up mode when using the Tool Path Graphics routines.
Whenever the ProtoTRAK SM CNC detects a data error a message will appear that will tell
you the error number (you may wish to record this number for troubleshooting purposes)
and the event where the error was detected. This is not necessarily the event that is in
error since the system often "looks ahead" to make sure there is compatibility from one
event to another.
In addition, an explanation is given for each data error type as well as a suggested
solution. Press the RETURN soft key to go back to the Select Mode screen, correct your
error, and proceed.
12.10
Fault Messages
The ProtoTRAK SM CNC performs a number of automatic checks or self-diagnostics. If
problems are found a message will appear: "Fault __ __ __ __". The information area
will display an explanation and suggested solution.
88
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
13.0 Program In/Out Mode
From the Select Mode screen, press the PROG IN/OUT softkey. The first screen you see will ask:
"LIST SUPPORTED PROGRAMS ONLY?"
With a highlighted YES or NO.
FIGURE 13.0 Supported programs are part programs that can run on the ProtoTRAK SM CNC. You do
not have to answer this question every time you are at this screen. Simply press the
softkey for the operation you want.
Supported programs are the programs that will run on your ProtoTRAK SM CNC. It is possible to
view other types of files through the Program In/Out Mode, for example, Microsoft Word® files.
This type of file is not supported on the ProtoTRAK SM CNC in the sense that you cannot open it
and work on it. We recommend a "Yes" response to this prompt. If "No" is selected, it is
possible to view, and inadvertently damage, files that are critical to running the ProtoTRAK SM
CNC (as well as on other networked computers.)
Filenames and File Extensions
Most places in the ProtoTRAK SM CNC, we refer to the program or part. In Program In/Out
Mode, this program or part is called a file. Filenames are program names or part names. They
are the name you give to the programs you write on the ProtoTRAK SM CNC, plus a file
extension. Although the ProtoTRAK SM CNC can have program names up to 25 characters that
use letters and special symbols, most other CNC’s must have file names that are eight or fewer
characters using numbers only.
File extensions are part of filenames that help describe the file. They appear after the filename
and are composed of three letters following a period. For example, .doc is the extension that
appears after a file name for a file stored using Microsoft Word™.
Usually, but not always, the file name indicates what program was used to create the file.
Sometimes this is not the case. Some programs, like those found in early models of CNC, do not
attach a file extension to a file name at all. Also, a user may attach his own extension to a file
name for his own purposes.
89
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
ProtoTRAK and TRAK A.G.E. CNC’s always attach an extension to every file that is stored. The
extension .mx2 is used for files, or programs, (written and) stored on a ProtoTRAK MX2,
ProtoTRAK M2 or TRAK A.G.E. 2 CNC. The extension .mx3 is used for the ProtoTRAK MX3,
ProtoTRAK M3 and TRAK A.G.E. 3 CNC’s. The ProtoTRAK SM CNC uses the extension .PT4,
whether the program is two or three-axis. (Before opening the file, the ProtoTRAK SM CNC is
able to determine what kind of file it is.)
A file extension that is unique to the ProtoTRAK SM CNC is .GCD. The .GCD extension tells the
ProtoTRAK SM CNC that a particular program is a standard RS274, or G Code program. When
you specify this extension, the ProtoTRAK SM CNC will treat that program in a special way. This
is explained in Section 13.9.2.
13.1 Softkey Selections in the Program In/Out Mode
YES: to display only supported programs.
NO: to display all files.
OPEN: to bring a program from storage into the current memory.
SAVE: to save the program that is in current memory to storage.
COPY: to select and make a copy of a file in storage for pasting in another storage location.
DELETE: to remove a file from a storage location without altering the current memory.
RENAME: to rename a file or folder.
BACK UP: to perform a convenient back up of program files to another storage location.
13.2 Basic Navigation of Program In/Out Mode Screens
The screens in the Program In/Out Mode do not have the normal ProtoTRAK look and
feel because they are derived from the Windows operating system. Most functions may
be performed using a mouse or keyboard. Softkeys are provided to operate the system
through the control's keys.
13.2.1
Basic Parts of the Program In/Out Mode Screens
The status
•
•
•
line at the top of the screen will display:
The mode
The program name for the program in current memory (if any).
Whether the ProtoTRAK SM CNC is in two or three axis.
The Look In area shows the storage areas (or drives) and directories that are being
displayed below in the listing area.
In the listing area (the biggest part of the screen) appears all the files and folders for the
location shown in the Look In box. The C Drive of the ProtoTRAK SM CNC is not
accessible for program storage.
The File Name box shows the program file on which the operation will be performed.
Parts of the screen unique to specific operations will be discussed below.
90
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
13.2.2
Softkeys in the Program In/Out Mode Screens
Use the softkeys to move around any of the screens in the Program In/Out Mode:
TAB: Moves the highlight between the parts of the screen. Where applicable,
tabbing to an area will cause a drop-down box to appear, showing all the selections
possible.
DATA FWD, DATA BACK: Moves the highlight up and down through the list. Press
and hold for automatic advancement.
OPEN FOLDER: Use this key to open a highlighted folder that contains program
files. When the highlight is on the root directory, this will collapse the list displayed
and show the next level up. The root directory is represented by a folder with an up
arrow followed by two periods. The root directory will disappear when the most
basic organization for the drive in the Look In box is reached.
13.3 Opening a File
To open a program file from a storage location, press the OPEN softkey from the
Program In/Out Mode screen. The ProtoTRAK SM CNC will always default to the last
folder you had open.
Find the file using the softkeys as described above in the section on basic navigation.
In addition to the basic parts of the screen described above, two additional parts of the
screen appear in the open operation:
File Name: - Displays the name of the file that is highlighted from the list.
Open As: - lists the formats for which the file may be opened. The default is .PT4.
Two additional softkeys appear:
OPEN FILE: Opens the highlighted program file and puts it in current memory.
Only one file may be in current memory at a time, if one is there already, a warning
message will appear before that file is overwritten.
RETURN: Returns to the Program In/Out Mode screen.
When the open operation is finished, the system will return to the Select Mode screen.
13.4 Saving Programs
To save a program file to a storage location, press the SAVE softkey from the Program
In/Out Mode screen.
Find the drive and folder you want to save the program file in using the softkeys as
described above in the section on basic navigation.
Three additional parts of the screen appear once the SAVE softkey is pressed:
91
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
FIGURE 13.4 The Save screen
File Name: displays the name of the file that is in current memory.
Save As: lists the formats for which the file may be saved. The default is .PT4.
Three additional softkeys appear:
CREATE FOLDER: Use this to create a new folder for the program file. This new
folder will be added to the list shown in the listing area, at the same level of
organization as the files and folders shown. Once the CREATE FOLDER softkey is
pressed, a Data Input Line will appear for entering the name of the folder. The name
"Folder1" will be written in the box. To accept this name, press SET. You may input
a name you select by writing over this name. Use the same procedure for naming a
program (see Section 7.3.1).
SAVE FILE: Saves the program file to the location shown in the Look In area.
RETURN: Returns to the Program In/Out Mode screen.
Once the save operation is finished, you will see the file name added to the files in the
listing area.
13.5 Copying Programs
To copy a program file from one storage location to another, press the COPY softkey
from the Program In/Out Mode screen. Only one file may be copied at a time using this
operation. To copy multiple files or folders, see Section 13.8.
92
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
FIGURE 13.5 The Copy screen
The copy operation is in two parts. First, use the navigation procedure described in
Section 13.2 above and highlight the program you wish to copy. Press the COPY FILE
softkey to copy the file. Then go to the new file or drive, open it using the Open Folder
softkey and press Paste file. Once the file has been copied, it can be pasted to as many
other locations as you want.
Additional softkeys in COPY:
COPY FILE: Makes a copy of the highlighted file.
PASTE FILE: Writes a copy of the file to the location shown in the Look In box.
RETURN: Returns to the Program In/Out Mode screen.
When the pasting operation is finished, you will see the file name added to the listing area.
13.6 Deleting Programs
Programs in current memory are removed from current memory in Edit Mode. See Section 10.3
To remove a program file from a storage location, press the DELETE softkey from the
Program In/Out Mode screen.
Use the navigation procedure described in Section 13.2 above and highlight the program
file or folder you wish to delete. Press the DELETE FILE or DELETE FOLDER softkey. A
warning message will appear for confirmation.
Additional Softkeys in DELETE:
DELELE FILE: Press this to delete a file.
93
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
DELETE FOLDER: Press this to delete a folder.
Softkeys that appear with the confirmation message:
YES: Press this if you want to delete.
NO: Press this if you do not want to delete. The delete operation will be aborted
and the previous softkey selections will return.
When the delete operation is finished, the file or folder name will disappear from the listing area.
13.7 Renaming
To rename either a file or a folder, press the RENAME softkey from the Program In/Out
Mode screen.
To rename a file or folder:
1. Use the navigation procedure described in Section 13.2 above and highlight the
program file or folder you wish to rename.
2. TAB to the New Name area and enter a new name. Use the same procedure as for
naming a program (see Section 7.3.1).
3. TAB to the New Extension and enter a new extension.
4. Press either RENAME FILE or RENAME FOLDER.
FIGURE 13.7 Renaming a file. Press the Help hard key to call up the alpha keys
Additional parts of the screen appear once the RENAME softkey is pressed:
New Name: When a file or folder is highlighted, the name will appear here. When the
TAB, the RENAME FILE or RENAME FOLDER softkey is pressed, the highlight will move
here and you will then be able to write in a new name.
94
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
New Extension: A new extension can be given to the file picking from the ones
available. If the file name already contains an extension, you will have to erase the old
one before giving it a new one.
Additional softkeys:
RENAME FOLDER - Press once a new name has been entered into the New Name and
New Extension areas to change the name of the folder.
RENAME FILE- Press once a new name has been entered into the New Name and New
Extension areas to change the name of the file.
RETURN - Returns to the Program In/Out Mode screen.
13.8 Backing Up
In order to protect your important programs, it is a good idea to back them up regularly.
That way, if a floppy disk or hard drive becomes unusable, you will not have to re-write
the program.
To back up your files, press the BACK UP softkey from the Program In/Out Mode screen.
FIGURE 13.8 Backing up. The top part of the screen shows all the items in Drive A.
The bottom part shows the items that have been picked for backing up
The basic procedure for backing up is:
1. Use the navigation procedure described in Section 13.2 above and highlight the
program file or folder you wish to back up.
2. Press the BACKUP FROM softkey. You will see the item appear, along with its
directory path, in the new listing area under the main listing area.
3. Repeat the above for as many items as you wish.
4. Use the navigation procedure to select a different drive or a different folder.
5. Open the drive or folder using the Open folder key.
6. Press BACKUP TO.
95
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
When the back up operation is completed, you will see the items and their directories in
the new location.
Note: It is good practice to back up files to a different drive, rather than to a different folder on
the same drive. For example, if you keep your programs on the ProtoTRAK SM CNC flash drive, it
is a good idea to back them up on a floppy disk or to another computer that is networked into the
ProtoTRAK SM CNC. That way, if the ProtoTRAK SM CNC flash drive becomes unusable, you
will have the part programs somewhere else so that you can reload them when the problem with
the ProtoTRAK SM CNC flash drive is resolved.
13.9 Converters™
Converters are programs within the ProtoTRAK SM CNC that translate CNC program files
of another format into a ProtoTRAK SM CNC file, or a ProtoTRAK SM CNC file into a
different format. With converters, you can run programs written on the ProtoTRAK SM
CNC on a machine that does not have a ProtoTRAK SM CNC and vice versa.
Each ProtoTRAK SM CNC comes with converters for other ProtoTRAK and TRAK CNC’s.
Converters for other brands of CNC’s are sold separately.
Program conversions take place by first translating the file into a neutral run engine, then
from neutral to the desired file format. For this reason, you should think of conversions
as being only one way. The conversion process changes the file in ways that are
harmless and so the results are correct. However, when converted back, it will not be
the same as it was originally written; it will create the same part, but some of the lines of
code will be different.
13.9.1
Activating Converters
Converters must be activated before you can use them. Standard converters include
those that handle the translation between the ProtoTRAK SM CNC and other TRAK CNC’s.
Optional converters are purchased separately. Standard converters and optional
converters that are ordered and shipped with the machine are activated at the factory.
You can tell which converters are activated by looking in the Open As (see Figure 13.9.3)
or Save As windows (see Figure 13.4).
If you purchase a converter after you have installed your machine, you must activate it
yourself using a simple procedure:
1. Go to Set Up Mode, Service Codes, then A. Software.
2. Press the soft key for Service Code 318.
3. A screen will appear that lists all the converters available for the version of
ProtoTRAK SM CNC software that you have. The converters that are active are listed
in black; the inactive converters are grayed out. See Figure 13.9.1.
4. Place the cursor over the inactive converter you want.
5. Press the Install soft key.
6. There is a password that enables you to use the converter. Enter the password in
the Data Input Line and press Set. If you do not have the password, call the SWI
96
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Customer Service Group at (800) 367-3165. You will need to make arrangements to
pay the fee for the converter before you are given the password.
97
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
FIGURE 13.9.1 Service Code 318 displays a list of converters available on the ProtoTRAK SM CNC
software version you are running. On this list, the first three converters are active,
the rest are not active.
13.9.2
Converting From a Different Format into a ProtoTRAK SM CNC
Conversions from a different format into a ProtoTRAK SM CNC occur when the file is opened.
FIGURE 13.9.2 Use the Open As box to tell the ProtoTRAK SM CNC what kind of file it is
Use the Open As box to tell the ProtoTRAK SM CNC what format the file is in so that it
knows how to convert it to the ProtoTRAK SM CNC format. In Figure 13.9.1 the
ProtoTRAK SM CNC could guess that the file to be converted was from a previous version
of ProtoTRAK because of its file extension (.mx3). But since file extensions may be
missing or may not really describe the file format correctly, you can use the Open As box
to declare the file type.
98
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
All files, or programs, open on the ProtoTRAK SM CNC as a .PT4 file (with one exception,
G-Code files, see below). Once the file is opened as ProtoTRAK SM CNC file, you may
store it as ProtoTRAK SM CNC file with the same filename and the extension .PT4.
The drop-down menu in the Open As box shows which converters are available. Open
As types that are grayed out indicate converters that are available for purchase.
13.9.3
Converting From the ProtoTRAK SM CNC to a Different Format
Files, or programs, are converted from the ProtoTRAK SM CNC to a different format using
the Save function of Program In/Out Mode.
FIGURE 13.9.3 Use the Save As box to tell the ProtoTRAK SM CNC what file format you want to end up with
Use the Save As box to tell the ProtoTRAK SM CNC what kind of file you want the current
program (in the .PT4 format) to be converted into.
In Figure 13.9.3 the file name 070501 is being saved on drive A as a .mx3 file. Note that
although the program or part name as shown in the status line is BRKT005, the file name
given for converting the file conforms to the .mx3 format – fewer than eight characters
long and consisting of numbers.
13.10 ProtoTRAK and TRAK CNC Compatibility
File exchange between the ProtoTRAK SM CNC and other ProtoTRAK and TRAK CNC’s is possible
because the ProtoTRAK SM CNC is backward compatible. In other words, the ProtoTRAK SM CNC
can store and retrieve other ProtoTRAK and TRAK CNC files. The actual transfer of the files can
be accomplished by using a floppy disk, zip disk, RS232 and/or Ethernet cable. In order to
transfer files between the ProtoTRAK SM CNC and previous generations of ProtoTRAK and TRAK
CNC, you must have the .MX2 and .MX3 converters activated. See Section 13.9 above.
Note: Previous ProtoTRAK and TRAK CNC’s allow numeric filenames of eight (8) characters or less,
while the ProtoTRAK SM CNC allow alphanumeric filenames (letters and numbers) of up to twenty five
(25) characters. Be sure to use only numeric filenames when storing a file on a ProtoTRAK SM CNC that
will be retrieved by previous ProtoTRAK and TRAK CNC’s. Before conversion, you can easily rename the
file in the ProtoTRAK SM CNC current memory.
99
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
13.10.1
File Formats
The ProtoTRAK SM CNC can store and retrieve the following ProtoTRAK and TRAK CNC
“dot” file formats.
Previous ProtoTRAK and TRAK CNC “dot” file formats:
ProtoTRAK M2
ProtoTRAK MX2
ProtoTRAK MX2E
TRAK AGE2
ProtoTRAK EDGE
.mx2 (pronounced “dot” mx2)
.mx2
.mx2
.mx2
.mx2
ProtoTRAK M3
ProtoTRAK MX3.mx3
ProtoTRAK MX3E
TRAK AGE3
.mx3
.mx3
.mx3
TRAK QMV
.mx3
13.10.2
Opening .MX2 and .MX3 files on a ProtoTRAK SM CNC
Programs written on previous generation ProtoTRAK and TRAK CNC’s may be opened
and run on the ProtoTRAK SM CNC. You will need to have the .MX2 or MX3 converters
activated (see Section 13.9 above). The ProtoTRAK SM CNC will automatically convert
the file (.MX2 or .MX3) to a .PT4 file. The original file will remain on the storage device
unchanged and the converted file will be in current memory. You will have to save the
converted file using the procedure in Section 13.4 above in order to place in into storage.
Since there are some feature differences between the ProtoTRAK SM and previous
generation controls, you will have to pay attention to the following:
Event or feature
Nested Repeats
3 or 4 Sided Pocket
13.10.3
Comment
These are handled a bit
differently between the controls.
The Nested Repeat must
reference all event numbers from
a previous Repeat event, not just
the previous Repeat event
number, otherwise it will be
ignored.
These Events will be recognized
by the ProtoTRAK SM CNC but in
a modified format.
Result
For example
Not Acceptable:
Event #13 Repeat
Event #14 Repeat
Acceptable:
Event #13 Repeat
Event #14 Repeat
Events #1-12;
Events #13.
Events #1-12;
Events #1-13.
The ProtoTRAK SM CNC will convert
the 3 or 4 Sided Pocket routines into an
Irregular Pocket Event.
Running ProtoTRAK SM Files on ProtoTRAK and TRAK CNC Controls
In order to have a program written on a ProtoTRAK SM run on a previous version
ProtoTRAK or TRAK CNC, you will need the .MX2 and .MX3 converters activated (see
section 13.9 above). Save the program as either a .MX2 or .MX3 file (depending on the
control or program you want to run).
Since there are some feature differences between the CNC’s the process will generally
yield a useable .mx2 or .mx3 program but with the following exceptions:
100
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Event or feature
Hidden Areas in
Irregular Pocket
Comment
The ProtoTRAK or TRAK CNC
does not recognize Hidden
Areas in Irregular Pockets.
Tap Events
This routine does not exist in
the ProtoTRAK or TRAK
CNC.
Copy Repeat
Subroutines with
%Feed or %RPM
The %Feed or %RPM
function does not exist on the
ProtoTRAK or TRAK CNC
Tool Path
Programming
Only Part Geometry
programming is supported on
the ProtoTRAK or TRAK
CNC.
This routine does not exist in
the ProtoTRAK or TRAK CNC.
Zig-Zag Entry Mode
Ramps
Event Comments
Thread Mill
Tool Table Info
Irregular Profile
13.11
Event comments are not
supported on the ProtoTRAK
or TRAK CNC.
This routine does not exist in
the ProtoTRAK or TRAK
CNC.
The part programs for
ProtoTRAK or TRAK CNC do
not contain tool table
information. This information
is kept separately.
The ProtoTRAK or TRAK CNC
does not contain an Irregular
Profile Event.
Result
The Irregular Pocket will be converted to an
Irregular Pocket; however, the ProtoTRAK or
TRAK CNC will display an error message that
there are Hidden Areas in the Irregular Pocket.
We recommend that you separate the Irregular
Pocket into two or more Irregular Pockets using
the ProtoTRAK SM before conversion.
The routine will be ignored in the converted
program. We recommend that you reprogram the
Tap Events into Drill or Position events before
conversion.
The %Feed or %RPM information will be removed
from the Copy Repeat Subroutines. The
programmed feed rates will be run. We
recommend that you inspect the feed rates before
running the program on the ProtoTRAK or TRAK
CNC when the %s are other than 100%.
You can only transfer Part Geometry programs to
the ProtoTRAK or TRAK CNC.
The routine will be converted to a Plunge routine.
We recommend that you check your Z feedrate to
make sure it will be correct for a plunge.
Event comments will be ignored.
Thread Mill events will be ignored. We
recommend that you replace these events with
the Helix Events and Mill Events to ramp in and
ramp out of the helix.
Tool table information will have to be set in the
ProtoTRAK or TRAK CNC as usual.
The Irregular Profile Event will be converted to
Mill and Arc Events and the programming of the
finish cut and steps will be lost. We recommend
that after conversion, you add repeat events for
the steps and finish cut, using the technique of
overstating the size of the cutter you will use to
cut the profile.
Running G Code Files
The ProtoTRAK SM allows you to run G Code files directly without having them converted to the
ProtoTRAK SM programming format. You may want to do this if you have a very large CAM file made
up of small XYZ position moves, or if there is complex surface contouring. In these cases, the
ProtoTRAK SM can handle the files more efficiently by running the G Code directly. While running the
G Code file directly does not give you the benefit of the easy programming format of the ProtoTRAK
SM, you are not likely to be able to use this benefit with a very large or complex file anyway.
101
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
To run the G Code file directly, open the file using OPEN AS: G Code .GCD. The entire program
will be brought into current memory. You will be able to view the tool path when you run the
program in the Run Mode, but you will not be able to edit the program or view it in the Program
Mode. In order to edit the program, you will have to use the same application (usually CAM) that
you used to write the program originally.
13.11.1
G00
G01
G02
G03
G06
G07
G16
G17
G18
G19
G20
G21
G40
G41
G42
G61
G64
G80
G81
G82
G83
G84
G85
13.11.2
M00
M01
M02
M03
M04
M05
M06
M07
M08
M09
M30
M79
M98
13.11.3
G
M
N
T
F
G Codes Recognized by the ProtoTRAK SM CNC
positioning (rapid)
linear interpolation (feed)
circular interpolation CW
circular interpolation CCW
CW Helix
CCW Helix
Selects a vertical plane via a bearing angle (value in ‘D’ word) from the X-axis
Selects the XY plane for circular interpolation.
Selects the XZ plane for circular interpolation.
Selects the YZ plane for circular interpolation.
input in inch
input in mm
cutter compensation cancel (for SWI it means center)
cutter compensation left
cutter compensation right
exact stop check mode
cutting mode (no hesitation between events. NOHES=true)
Hole machining canned cycle
Drill canned cycle
Spot drilling canned cycle
Peck drilling canned
Tapping canned cycle
Boring canned cycle
M Codes Supported by the ProtoTRAK SM CNC
program stop with prompt (press go to procd.)
optional stop
end of program (no rewind)
spindle CW
spindle CCW
spindle stop
tool change
mist coolant ON
flood coolant ON
coolant OFF
end program (rewind stop)
Send SWI ‘O’ (ascii 79) commands, value in ‘P’ word
Subroutine Call to block (PWORD), repeat (L WORD)
Valid Characters for Word/Address Sequences
Prepare to execute a G COMMAND
Prepare to execute a M COMMAND
Introduces a block number
Specifies the tool number to use
Specifies a feedrate
ParseGcode
ParseMcode
ParseEventNum
ParseToolNum
ParseFcode
102
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
S
D
E
X
Y
Z
I
J
K
L
P
(
Specifies a spindle rpm
Specifies the diameter for the current tool
Optional parameter
Specifies the X dimension
Specifies the Y dimension
Specifies the Z dimension
Specifies the incremental X dimension
Specifies the incremental Y dimension
Specifies the incremental Z dimension
An Optional Parameter
An Optional Parameter
Introduces a comment
ParseScode
ParseDval,
ParseEval,
ParseXval,
ParseYval,
ParseZval,
ParseIval
ParseJval
ParseKval
ParseLval
ParsePval
ParseComment
13.12 Networking
This portion of the ProtoTRAK SM CNC manual is written to give you a brief overview of
networking and point out the benefits that can be received when setting up the ProtoTRAK SM
CNC control in a network environment. There are many resources available at most bookstores
on this subject.
13.12.1
What is a Network?
A network is nothing more than two or more computers connected by a cable so that
they can exchange information.
Networks are often called LANs (Local Area Network)
13.12.2
Why would you want to use the networking capability of the
ProtoTRAK SM CNC control?
1. To allow an easy way to backup programs to other computers or a dedicated storage
device(s) connected to the network.
2. To transfer files between the ProtoTRAK SM CNC control and other SM, ProtoTRAK or
Fanuc-type controls
3. To import CAD/CAM programs written on other computers connected to the network
4. To access printers on the network
5. To access e-mail over the network
6. To access an internet modem that is connected to the network
7. To run programs that are larger than the ProtoTRAK SM CNC control’s storage capabilities
from network storage devices connected to the network
8. To allow easy access for customer service support (i.e.; software updates and access to
error logs via the internet)
The two most common types of networking are peer-to-peer networking and networking
using a server and clients. Both types of networking can be used in a multitude of
configurations, so for the purpose of this manual, we will focus on their most basic forms.
103
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
13.12.3
A Word of Advice Before Setting up Your Network
Setting up a network can be very tricky. Getting all the necessary components to install
correctly and to communicate with your software properly can literally require hours of
troubleshooting, even by experts. If you are very knowledgeable about networking and/or have
set up a network before, then we encourage you to proceed through the following set of
instructions. If you have little or no experience with computers or networking, then we strongly
urge you to find a computer consultant to help you set up the network with your new ProtoTRAK
SM CNC control. You can find these people in the Yellow Pages.
13.12.4 Peer-to-Peer Networking
The most basic type of networking is called peer-to-peer networking. This involves
simply connecting two or more computers together with a cable attached to a network
interface card, which is installed into each computer.
Network Interface Card (also known as an Ethernet Card): an electronic circuit adapter
card that is placed inside a computer and allows it to attach to a special network cable.
Network Cable: The network cable is what physically plugs into a network interface
card to allow the computers to communicate with one another.
There are many types of network cables. The network interface card inside the
ProtoTRAK SM CNC control requires a twisted-pair category 5 rated network cable, which
looks like a telephone cable and is readily available at most computer supply stores.
In a peer-to-peer network, all the computers that are connected together are thought of as
peers, or equals. The ProtoTRAK SM CNC control can be considered a peer to other CNC’s
or desktop computers.
Peer-to-peer networking features are built right into the Windows 95/98/ME/XP software.
If you are using any of these Microsoft operating systems you do not have to purchase
any additional software to set up this type of network. The ProtoTRAK SM CNC control
uses the Windows 95 OSR2 operating system.
FIGURE 13.12.4 Peer-to-Peer (desktop PC to ProtoTRAK)
13.12.5
Basic Network Set-Up
This section will give you instructions for the most basic set-up of one ProtoTRAK with
one desktop computer. The desktop computer must have an Ethernet card installed.
Use a crossover CAT5 cable to connect the machines. Before you begin, connect a
104
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
keyboard and mouse to your ProtoTRAK and turn the ProtoTRAK on with them connected
so that it will recognize them. If your set-up is more complicated than that pictured in
Figure 12.12.4, you should skip this section and see Section 12.12.6.
1. For the ProtoTRAK VL and VM CNCs, press the Windows key and then press
Windows 98. For the ProtoTRAK SM and SL, press the SYS key, then press CONFIG
NETWORK. This will take you to the Windows desktop.
2. From there, click on START, then go to SETTINGS, CONTROL PANEL.
3. Double click the “NETWORK” icon, and go to the Configuration tab. You should get a
window that looks something like the one below.
Figure 13.12.5.1
There are 4 components that are needed:
•
•
•
•
Client for Microsoft Networks
Realtek PCI Fast Ethernet Adapter
TCP/IP
File and Printer sharing.
4. Double click on Realtek PCI Fast Ethernet, it should be the one with the green icon next to it.
5. Under the Bindings tab, make sure that you have the option checked off which should
read TCP/IP as shown in Figure 13.12.5.2.
105
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Figure 13.12.5.2
6. Exit this window and go back to the first Network window.
7. Highlight the line which reads “TCP/IP—Realtek PCI Fast Ethernet”
8. Click on “Properties”, under the “IP address” tab, select “Specify an IP address”.
Now type in an IP address, making sure to match the first set of numbers with the IP
address of the computer that you are connecting to. (You can obtain your
computer’s current IP number by going to START -> RUN -> WINIPCFG. Otherwise
you can manually enter one).
Figure 13.12.5.3
9. Click on the “DNS Configuration” tab, and make sure that it is disabled.
10. Click on the “WINS Configuration” tab, and make sure that is disabled as well.
11. Click on the “Bindings” tab, and make sure that you have “Client for Microsoft
Network” and “File and printer sharing” checked. You will need these in order to log
on correctly as well as be able to transfer files from one computer to the other.
106
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Figure 13.12.5.4 TCP bindings
12. Close this window and return to the original Network window. Click on the
“Identification” tab.
13. Compare these settings to the ones on your computer, and make sure that
workgroup is the same for both, and that they each have unique computer names.
(See Figure 13.12.5.5)
Figure 13.12.5.5 Identification
14. Finally, close the windows. Restart the ProtoTRAK.
15. On your computer, you want to make sure (using the same steps), that you have
TCP/IP installed, matching workgroups, unique computer names, unique IP
addresses that will work together (192.162.0.1 & 192.162.0.2 for example), Client for
Microsoft Windows, and file and printer sharing enabled.
16. Restart both the computer and your ProtoTRAK. To verify that we have successfully
networked both computers together, on your desktop double click on Network
107
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Neighborhood. You should see each other’s computer name here. If not, contact
SWI customer service or your systems administrator for technical support.
Now you will need to share and map at least one drive in order to be able to transfer
files back and forth between two networked computers. Sharing a drive determines
what folders on your computer you want to share with the rest of the network.
Mapping sets up a drive on your computer as a shortcut to a shared folder across a
network. Depending on your needs, you would most likely want to share a folder on
your PC, and map it on your ProtoTRAK.
17. To share a drive / folder on your computer, first you must locate it using Windows
Explorer. Double click on MY COMPUTER, then on C DRIVE. Find the folder you wish
to share, then using the right mouse button click on it and select SHARING. You can
also share the entire C drive if you’d like (making everything on your hard drive
available for sharing). You should get a window like the one below.
Figure 13.12.5.6 Sharing
18. Make sure you select the option “Shared As”, and most likely you will want to select
Full access type, so that you can open AND save files across the network. Click on
OK when you are finished.
19. To map a drive on your ProtoTRAK, go into Windows 98, then double click on
NETWORK NEIGHBORHOOD on your desktop. You should be able to see the name
of the computer(s) that you are currently networked to. Double click on the one you
wish to map to, and when opened you should see a list of all folders that we enabled
sharing. Right click on one of these folders, and select “Map Network Drive”, you
should get a window like the one below.
108
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Figure 13.12.5.7 Mapping
20. Choose an available drive letter of your choice, make sure that the “Reconnect at
logon” option is checked, and click OK. From now on, the drive letter that you chose
will be assigned as a shortcut to the shared folder (which is actually a folder stored
on the networked computer). On your ProtoTRAK, you will be able to see this drive
when you go to PROG IN/OUT, and attempt to OPEN or SAVE your files. Using the
TAB button to move to the LOOK IN window, you should now be able to save /
retrieve to and from your newly mapped network drive.
FIGURE 13.12.6 Peer-to-Peer (3 desktop PC’s and 1 SM CNC control hooked to a hub
13.12.6
Server and Client Network Overview
A more complex type of network, often found within an office environment, involves the
use of a server and individual clients. Connecting more than two computers requires the
addition of a hub.
109
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
Server: a computer that is dedicated primarily to the task of providing shared resources,
such as hard drives, and printers to other users on a network.
Client: a computer that has access to a network server and shares its resources.
Hub: a device that allows multiple computers to communicate with each other.
We recommend that you use a DHCP switch instead of a simple hub. The switch will
automatically assign IP addresses, subnet masks, and gateway addresses in addition to
performing the distribution functions of a hub.
This will make setting up multiple CNCs or computers easier. Simply use the default
settings shown in Section 12.12.6 and plug the devices into the switch.
110
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
FIGURE 13.12.7 Typical server and client set-up diagram
In many companies, a main database is often kept on the server and is accessed by the
clients. The client can be thought of as an individual desktop computer in an office
cubicle. When the person using a client needs to make a change to a main database, he
accesses the server through the network.
The server uses software specifically designed to manage this type of network set-up.
The most commonly used software is Microsoft Windows NT/2000. This software carries
out the tasks of coordinating the access to shared network resources among the network
client computers. Most clients use a desktop version of Microsoft Windows 95/98/ME/XP.
111
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
13.12.7 Network Description of the ProtoTRAK
The following table summarizes important settings for the ProtoTRAK V series and
ProtoTRAK S series CNCs. It is intended for use by a professional Network Administrator.
Note: The ProtoTRAK has many similarities to a desktop computer, but it is somewhat different
because the use of the computer's resources is optimized for running part programs and a
machine in real time. In order to avoid causing a slow-down or even instability in the operating
system of the control, keep the following in mind while setting up the network:
•
•
Do not use a resource-intensive networking program such as SMS.
Avoid loading in programs that direct background tasks, e.g. anti-virus programs.
ProtoTRAK system
Windows
Processor
Memory- RAM
Disk
Floppy drive
Network
Ports available
System software
SL or SM
95 OSR 2
Pentium 2 - 233
32
Compact flash, optional
second compact flash
Yes
10/100 base T Ethernet
COM1, LPT 1
Not available to user. Instead
use second flash drive,
Network or LPT CDROM
System and network set up
Default password
Default user name
Default computer name
Default work group
Network settings
Default protocols
Network log in
TCP/IP set up
Dns
Gateway
Wins configuration
VL or VM
98 Second edition
Pentium 2 - 233
32
Hard drive, 2 gig or bigger
Yes
10/100 base T Ethernet
COM1, LPT 1
Full Windows distribution on
hard drive in C:\WIN98.
PT4
PT4
PT4SN0001
SWI
Client for MS Networks
File and print sharing
Net beui
TCP/IP
Windows log in*
Enabled share level access control
Obtain IP address automatically
Disabled
Not used
Use DHCP for wins resolution
*do not change
13.13
RS232 Interface
While networking and floppy disks are more modern, reliable and convenient methods, the
RS232 protocol may also be used to transfer files between the ProtoTRAK SM CNC and
other controls and computers. The ProtoTRAK SM CNC will support RS232 file transfer for
Open and Save operations in the Program In/Out Mode. The other operations (such as
Back up) cannot be done through RS232.
112
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
13.13.1
Connections
To transfer a file between the ProtoTRAK SM CNC and a remote computer or control, the two
systems must be connected to each other with an RS232 cable. On the ProtoTRAK SM CNC,
plug the cable into the connector on the left side of the pendant (see Figure 3.2). On the
remote computer or control, the cable may go to any available serial port. The baud rate
for the ProtoTRAK SM CNC is set at 4800; use Service Code 37 to reset the baud rate.
The pin-out for the 9-pin connector is the standard RS232 PC - PC Laplink/Interlink cable
(PC 9 way female - PC 9 way female).
9D Female
RS232 signal
GND
TxD
RxD
RTS
CTS
DSR
SG
DTR
13.13.2
Pin
Case
3
2
7
8
6
5
4
–––––
–––––
–––––
–––––
–––––
–––––
–––––
–––––
Pin
Case
2
3
6
4
7
5
8
9D Female
RS232 signal
Gnd
RxD
TxD
DSR
DTR
RTS
SG
CTS
Receiving a File
Receiving a file via the RS232 is done through the file Open command. See Figure 13.13.1.
Figure 13.13.1 The RS232 port is selected in the Look In box.
Once the RS232 port is selected, pressing the Tab key will position the cursor in the now
empty list of contents. A message window will appear prompting you to enter the file
name of the file you wish to receive. Press Tab again to move the cursor to the File
Name box. You may name the file the same name as the one it has on the remote
computer or control, or you may give it a different name. After entering the file name,
move the cursor to the Open As box and select the format of the file that you wish to
113
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
receive as it exists in the remote computer or control. For example, if you were
transferring a Haas file from a Haas CNC, you would select the file type: HS1.
After you have set up the ProtoTRAK SM CNC to receive the file, press the Open soft key. A
message window will appear to notify you that the ProtoTRAK SM CNC is ready to receive the
file.
If the remote computer or control is a TRAK or ProtoTRAK CNC (or is a computer that is
running ProtoTRAK or TRAK A.G.E. offline software) you can send the file by simply using
the Save softkey (via the RS232) in the Program In/Out Mode. If the remote computer
or control is not a TRAK or ProtoTRAK CNC, consult your manual for sending files via the
communications port.
Modern Windows operating systems have programs such as Windows hyper-terminal and
CAD/CAM systems have the capability of communicating via the RS232 port.
The commands for an MS-DOS system are:
'mode COM1: 4800,e,7,1' – to set up the port where COM1 is the serial port on
the remote computer
and 'copy “filename” COM1: ' – to send a copy of the file to the COM1 port.
As the program is received it will be converted into the ProtoTRAK SM CNC format and
put into the current memory. Once the transfer is complete, the Select a Mode screen
will appear.
13.13.3
Sending a File
Sending a file via the RS232 is done through the file Save command. Transfer will take
place only with a program that is in the ProtoTRAK SM CNC's current memory.
As with receiving the file, the RS232 port must be selected in the Look In box.
Since the file name does not transfer with the program through RS232, you can ignore
the file name box.
Place the cursor into the Save As box and select a file format. The ProtoTRAK SM CNC
will convert the file to the format that you select as it is being sent to the remote
computer or control.
Once the transfer is set up, press the Save soft key. The ProtoTRAK SM CNC will be
placed in a ready state for transferring the file to the remote computer or control. A
second Save key press is required to go from this ready state to actually sending.
The remote computer or control must be set up to receive the file. If the remote
computer or control is a TRAK or ProtoTRAK CNC (or is a computer that is running
ProtoTRAK or TRAK A.G.E. offline software) you can receive the file by simply using the
Open softkey (via the RS232) in the Program In/Out Mode. If the remote computer or
control is not a TRAK or ProtoTRAK CNC, consult your manual for sending files via the
communications port.
Modern Windows operating systems have programs such as Windows hyper-terminal and
CAD/CAM systems have the capability of communicating via the RS232 port.
114
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
The MS-DOS commands for receiving the file are:
'mode COM1: 4800,e,7,1'
and then: 'copy "filename" COM1:'
The receiving computer or control will attach the filename to the program it receives via
the RS232 port.
When the receiving computer or control is ready, press the Save key a second time to
send the file.
Once the file is sent, the Program In/Out Mode Save screen will remain and the Look In
drive will change to the one used previous to the RS232 operation.
13.14
CAD/CAM and Post Processors.
In addition to running G-code files, the ProtoTRAK will also accept CAM files and convert
them into the ProtoTRAK events. This is a great advantage as it allows you to have your
CAD/CAM programmer send files to the machine that the machinist can then work with in
the familiar ProtoTRAK interface. The machinist can modify the program as necessary
without having to go back to the CAD/CAM programmer.
In order to be able to convert the program from a CAM system to a ProtoTRAK program
the CAM program must be two or 2½ axis. A 2½-axis program is defined as a program
where the Z axis is stationary while X and Y is moving. If you want to run a full threeaxis program, you should run a G Code, or .GCD program (see section 13.11).
The above 2½-axis restriction does not mean that the ProtoTRAK is not capable of
running three-axis simultaneous programs written in ProtoTRAK events (as some illinformed competitors would have you believe). This restriction is a matter of practicality.
Because the ProtoTRAK allows you to program in part geometry and therefore will figure
out the tool path for you, the process of converting a three-axis program gives the
ProtoTRAK a tool position problem that it cannot resolve without a lot more data from
you. The other reason is that the output from a CAM systems for three-axis shapes is in
the form of thousands and thousands of straight-line G01 moves that would convert into
the equal number of ProtoTRAK Mill events. This is hardly a manageable program.
Instead of forcing the issue in a silly way, we give you the more elegant solution of
running GCD files. To our competitors, we respectfully point out that the thread and
helix milling canned cycles of the ProtoTRAK are obvious examples of three-axis
simultaneous interpolation.
In order to run a CAM program, the program must be posted through a post-processor
that makes some adjustments to the output of the CAM software so that it is understood
by the ProtoTRAK. The ProtoTRAK uses a post-processor that is very similar to the
Fanuc 6M.
If you are not familiar with writing a post-processor, we recommend that you contact
your CAD/CAM supplier. We will be happy to work with him to get you the postprocessor you need.
115
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
13.14.1
Writing a Post Processor
The following are modifications to a Fanuc 6 post-processor that are necessary for
writing the ProtoTRAK post-processor.
Beginning file format: The ProtoTRAK has no special requirements, it does not need
any special characters.
End of file format: the ProtoTRAK requires the % to show the end of the file.
Characters after the % will be ignored.
Beginning of an operation: the ProtoTRAK requires that the tool number, feedrate
and tool offset appear before, or on the same line, as a move command. In addition, the
ProtoTRAK VM (but not the SM) requires the spindle speed be set. The absolute zero of
the ProtoTRAK is set in a different mode and does not need to be set at the beginning of
each operation. The feedrate is modal, once it is set, it remains the same until changed.
Lines: the line feed (or carriage return/line feed) signals the end of the line (ASCII code
hex 0A or 0D 0A). A semicolon is optional.
Coordinates: may be formatted in inch or metric. The addresses used for specifying
coordinates are X, Y, Z, I, J, K. The valid ranges are:
•
Inch: min -99.9999 to max +99.9999
•
Mm: min -999.99 to max +99.999
Rapid moves: rapid moves are generated by the ProtoTRAK automatically as part of
the definition of an event. For this reason, G0 moves are discarded unless they specify a
location other than the beginning of the following event.
Linear moves: G01 are formatted the same as rapid moves.
Arcs: Arc centers are specified by the address I, J and K for the X, Y and Z axes. The
number following the I, J and K are incrementally referenced from the starting point of
the arc. Radius values are not allowed.
Tool Numbers and Tool Changes: the format of the tool number is from T1 to T99.
During program run, the ProtoTRAK will rapid to home for a tool change and pause for
the tool to be loaded manually and the operator to press GO.
Feed rates: the ProtoTRAK is programmed in inches (or mm) per minute using the 'F'
address.
Spindle speed: the ProtoTRAK SM does not have spindle speed control, so S values are
ignored. The VM uses S values.
File name: use the .CAM extension so the ProtoTRAK will recognize the file as a CAM file
and convert it into ProtoTRAK events when it is opened. File names may include up to
20 alpha-numeric characters.
116
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
13.14.2
Convertible G-Codes
The following G-codes may be used in a CAM file that you want to have converted to a
ProtoTRAK program. G Codes that are not on the list below have no correspondent
operation in the ProtoTRAK events and will be ignored when the program is converted.
If a G Code is essential to your program and you do not see it here, you can do one of
two things.
•
Convert the file from CAM to ProtoTRAK and add an event to the resulting
ProtoTRAK program.
•
Run the program as a GCD file (See Section 13.11).
G Code
G00
G01
G02
G03
G20
G21
G40
G41
G42
G54
G55
G56
G57
G58
G59
G73
G80
G81
G82
G83
G84
G85
G89
G90
G91
G98
G99
13.14.3
Description
Rapid positioning
Linear interpolation
Circular interpolation CW
Circular interpolation CCW
Input in inch
Input in metric
Cutter compensation cancel
Cutter compensation left
Cutter compensation right
Work coordinate system 1 selection
Work coordinate system 2 selection
Work coordinate system 3 selection
Work coordinate system 4 selection
Work coordinate system 5 selection
Work coordinate system 6 selection
Peck drilling cycle
Hole machining canned cycle cancel
Drilling cycle, spot boring
Drilling cycle, counter boring
Face hole machining cycle
Tapping canned cycle (VM only)
Face boring cycle
Boring cycle, dwell at bottom
Absolute programming
Incremental programming
Return to initial point in canned cycle
Return to point R in canned cycle
Supported Addresses
CAM information is communicated through the use of ADDRESS – WORD pairs. For
example in the line “N01G0X1.Y2.” N, G, X, and Y are addresses. The other information
(01, 1, and 2) are Data Words. The line starts with the Address = N and the data word
= 01. The N address is defined as meaning “LINE NUMBER”, therefore N01 means Line
# 1, and so on.
117
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
X, Y, Z
I, J, K
D
M
G
H
N
T
F
P
L
Q
R
S
13.14.5
Dimensions along the specified axis
Distance to arc center I = X, J = Y, K = Z.
Tool Diameter
Miscellaneous Functions
Preparatory Function
Tool Length Offset Selector (silently ignored).
Line Number (silently ignored)
Tool Number
Feedrate
Dwell time for drill/bore canned cycles
Repetition count for drill/bore canned cycles
Depth of cut for drill/bore canned cycles
Reference point for drill/bore canned cycles
Spindle Speed
Format Terms and Definitions
Number formats
A. preparatory function number, denoted <prep-func>
1. format: dd
2. leading 0 suppression
3. range: 0 to 99
B. sequence or line number, denoted <seq-number>
1. format (independent of units): dddd
2. leading 0 suppression
3. range: 1 to 9999
C. Unsigned coordinate word, denoted <coord>
1. format:
metric: ddddd.ddd
inch: dddd.dddd
2. the "+" sign is implied and therefore may be omitted
3. leading 0 suppression
4. if no decimal point is given, the supplied number will be interpreted as an integer
(i.e. a whole number).
5. Fractional portion is optional
6. Range:
metric: 0 to 99999.999
inch: 0 to 9999.9999
D. signed coordinate word, denoted <scoord>
1. format:
negative number: -<coord>
positive number: +<coord> or <coord>
2. range:
metric: -99999.999 to 99999.999
inch: -9999.9999 to 9999.9999
E. tool function, denoted <tool>
1. format : dd (use 2-digit only)
2. leading 0 suppression
3. range: 1 to 99.
118
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
F. miscellaneous or M codes function number, denoted <prep-func>
1. format: dd
2. leading 0 suppression
3. range: 1 to 99
G. feedrate values, denoted <frate>
1. format:
metric: ddddd
inch: ddd.dd
2. leading 0 suppression
3. decimal point not required
4. fractional portion is optional
5. range:
metric: 1 to 6350
inch: 0.1 to 250
H. RPM command (VM)
1. format: dddd
S1000 = 1000 RPM
13.14.6
G Codes that Generate Errors
G Code
G27
G28
G29
G30
G31
G33
G37
G38
G39
G45
G46
G47
G48
G62
G63
G65
G66
G67
G74
G76
G86
G87
G88
G92
G95
Function
Reference point return check
Return to reference point
Return from reference point
Return to 2nd reference point
Skip function
Thread cutting
Tool length automatic measurement
Cutter radius compensation vector change
Cutter radius compensation corner rounding
Tool offset increase
Tool offset decrease
Tool offset double increase
Tool offset double decrease
Automatic corner override mode
Tapping mode
User macro simple call
User macro modal call
User macro modal call cancel
Counter tapping cycle
Fine boring
Boring cycle
Back boring cycle
Boring cycle
Programming of absolute zero point
Feed per revolution
119
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
13.14.7
M Code
M00
M02
M05
M06
M07
M08
M09
M12 & M20
Notes:
1.
2.
Accepted M Codes
Function
A pause is generated. The axes will not move, but the motors will be
engaged. The spindle motor will not turn off.
Executed automatically at the end of all programs. Turns off the servo
motors and all auxiliary functions. The auxiliary function box must be
present for this function to work.
Stops the spindle at the end of the current event. The auxiliary function
box must be present for this function to work.
Tool change. The M06 is ignored, as the tool change on the ProtoTRAK is
accomplished by changing the tool number.
Flood coolant on. This will turn on the auxiliary box A/C outlet before the
event.
Mist coolant on. This will turn on the air supply from the auxiliary box
before the event.
Coolant off. This will turn off the auxiliary box A/C outlet and air supply
after the event.
Send a pause to the indexer and wait for an “in position” response.
All other M codes will be ignored.
Place M Codes on same line as movement G Code.
One M Code per block.
120
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
121
Southwestern Industries, Inc.
TRAK DPMS3, DPMS5, ProtoTRAK SM CNC Safety, Programming, Operating & Care Manual
In order for SWI to process a trainee for certification, all aspects of
the training on the product must be successfully completed to the
satisfaction of the trainer and the trainee. Please fill out and sign
this document when the training is completed and send it to Ruby
Yonan at Southwestern Industries. Upon receipt, the certification
document will be created and sent to the trainee.
Complete the following information:
Full name of
person to receive
certification
Company
name and
complete
address
Name of trainer
Machine Name
Machine Model
Machine Serial No.
Place a checkmark next to each of the completed training areas:
1.
Definitions, terms and concepts for Axes, Planes and Referenced Data
2.
The DRO Mode, and using the machine tool manually
3.
Programming; using all canned cycles
4.
Editing capabilities
5.
Using all of the program storage and retrieval choices
6.
Converting data from other program sources
7.
Setting up tools and using the tool table
8.
Programming, setting up and running a complete part
9.
Understanding networking capabilities
10.
Using Math Help
11.
Using AGE capability in programming profiles
12.
Using Windows functions for non programming functions
13.
A review of related SWI products and compatibility to the SM control
Trainee Signature
Date
Trainer Signature
Date
ProtoTRAK SM Training
Checklist
F10371-2, 05-30-02
Southwestern Industries, Inc
Trav-A-Dial & TRAK
Warranty Policy
Warranty
Trav-A-Dial and TRAK products are warranted to the original purchaser to be free from defects in workmanship and materials for the following periods:
Product
New Trav-A-Dial
New TRAK
Any EXCHANGE Unit
Warranty Period
Materials
Factory Labor
1 Year
1 Year
1 Year
1 Year
90 Days
90 Days
The warranty period starts on the date of the invoice to the original purchaser from Southwestern
Industries, Inc. (SWI) or their authorized distributor.
If a unit under warranty fails, it will be repaired or exchanged at our option for a properly functioning unit
in similar or better condition. Such repairs or exchanges will be made FOB Factory/Los Angeles or the
location of our nearest factory representative or authorized distributor.
Disclaimers of Warranties
•
This warranty is expressly in lieu of any other warranties, express or implied, including any
implied warranty of merchantability or fitness for a particular purpose, and of any other
obligations or liability on the part of SWI (or any producing entity, if different).
•
Warranty repairs/exchanges do not cover incidental costs such as installation, labor, freight, etc.
•
SWI is not responsible for consequential damages from use or misuse of any of its products.
•
Trav-A-Dial/TRAK products are precision mechanical/electromechanical measurement systems
and must be given the reasonable care that these types of instruments require:
•
Replacement of chip scrapers and wipers is the responsibility of the customer. Consequently,
the warranty does not apply if chips have been allowed to enter the mechanism.
•
Accidental damage, beyond the control of SWI, is not covered by the warranty. Thus, the
warranty does not apply if an instrument has been abused, dropped, hit, disassembled or
opened.
•
Improper installation by or at the direction of the customer in such a way that the product
consequently fails, is considered to be beyond the control of the manufacturer and outside the
scope of the warranty.
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF

advertisement