Hypertherm Automation
5 Technology Drive, Suite 300
W. Lebanon, NH 03784 USA
Phone: 603-298-7970
Fax: 603-298-7977
PHOENIX®SOFTWARE FOR
YPERTHERM SHAPE CUTTING CONTROL
H
PROGRAMMER’S REFERENCE
Version 8.5 for Touch Screen CNCs
January 2009
D
ISCLAIMER The information in this document is subject to change without notice and should not be
construed as a commitment by Hypertherm Automation. Hypertherm Automation
assumes no responsibility for any errors that appear.
T
RADEMARKS Hypertherm Automation is a wholly owned subsidiary of Hypertherm, Inc.
Command, HT 4400, HD3070 HyDefinition Plasma and HD4070 HyDefinition Plasma
are registered trademarks of Hypertherm, Inc.
FASTLaser is a trademark of Hypertherm, Inc.
EDGE, HyperCAD, HyperNet, HyperNest, Phoenix, and ShapeWizard are registered
Nester, Remote Help, Sensor, and Voyager are trademarks of Hypertherm Automation.
HASP is a registered trademark of Aladdin Knowledge Systems Ltd.
Indramat is a trademark of Bosch Rexroth.
Pacific Scientific is a trademark of Danaher Motion.
Pentium and Celeron are registered trademarks of Intel Corporation.
Virus Scan is a registered trademark of McAfee Associates, Inc.
Microsoft, the Microsoft logo, and Windows are registered trademarks of Microsoft
Corporation.
NJWIN is a registered trademark of NJStar Software Corporation.
SERCOS Interface is a trademark of SERCOS North America.
Norton AntiVirus and Norton Ghost are trademarks of Symantec Corporation.
Other trademarks are the property of their respective holders.
C
OPYRIGHT 2009 by Hypertherm Automation. All rights Reserved
Printed in USA
ii
Contents
Editing Part Programs ............................................................................................... 1-1
The CNC contains a built-in Shape Library with more than 68 commonly used shapes.
These shapes are parametric. Parametric shapes are shapes whose size or geometry
you can edit. The shapes in the library are color-coded from easy (green) to difficult
(black).
To select a simple shape:
1. On the Main screen, press Shape Manager
2. Double click a shape.
or
Press a shape and press OK.
3. If the selection is incorrect, press Cancel and select the shape again.
Keypad operation:
1. Use the arrow keys to navigate to a shape.
2. Press Enter.
The shape is displayed with the default parameters or the parameters from the last
time this shape was edited. For more information on the available shapes, see Library Shapes in the Operator’s Manual.
1-1
Programmer’s Reference
Text Editor
The text editor screen allows you to write or edit a part program in either ESSI or EIA
format. The current part that is in memory is displayed when this screen opens.
Changes can be made by pressing on the desired line of code. An alphanumeric
keyboard displays to allow you to enter changes.
To edit code:
1. Select or press a line of code.
On the CNC, the alphanumeric keypad displays.
2. Enter changes to existing lines of code or add new lines.
3. Press OK to save your changes.
If you want to save the changes to the hard drive, select Files > Save to Disk.
4. Press Cancel to return to the previous screen without saving your changes.
Show Original
Text
Delete Part Deletes the current part from the Text Editor so that a new part can be
Allows you to view and edit the part program in its original format.
constructed.
1-2
Editing Part Programs
Shape Wizard
ShapeWizard® is a proprietary graphical part editor that provides a user-friendly,
graphical interface for editing part programs.
You can view not only the segment that is being edited, but other changes that are
made, as well.
There are a number of features on the Shape Wizard screen to facilitate editing part
programs:
• The shape you selected is displayed in the Preview Window and the corresponding
code is displayed in the EIA Text window.
• As you edit lines of code, the changes are visible in the Preview Window.
• You can add or modify EIA RS-274D codes in a part program in the EIA Text
window.
• If you don’t know EIA RS-274D codes, you can edit or create segments by making
entries and selections in the Segment Data fields below the EIA Text window.
• Zoom keys decrease or increase the size of the part in the Preview Window.
To edit a part program in the EIA Text window:
1. Press or click on a line of code to highlight it.
1-3
Programmer’s Reference
2. Press or click Manual Line Edit.
The alphanumeric keypad is displayed for line edits.
3. Type over a line to replace the text.
The ASCII text that you enter must be a valid EIA RS-274D code or an error
message will display.
4. To view data about the segment of the part that you have highlighted, select the
View Segment Data Below checkbox.
5. You can use the Segment Type field and related fields to change the highlighted
segment type and add it to the program.
6. While a line is highlighted in blue, you can use soft keys to replace a segment or
add a new one:
Replace
Segment
Insert Before
Segment
Insert After
Segment
Remove
Segment
7. As you edit a line of code, the picture of the part in the Preview window is updated.
The corresponding segment is highlighted in red if it is a cut segment or in blue if it
is a traverse.
Replaces the segment highlighted in gray in the Text Editor
window with the segment selected from the Segment Type
window.
Inserts the segment selected from the Segment Type window to
be inserted before the segment highlighted in gray in the Text
Editor window.
Inserts the segment selected from the Segment Type window
after the segment highlighted in gray in the Text Editor window.
Deletes the segment that is highlighted in gray or blue in the EIA
Text window from the part program.
1-4
Editing Part Programs
Teach Trace
The Teach Trace function of the CNC allows parts and remnants to be traced rather
than programmed. The position information from the traced part remains as a part
program that can be saved to disk.
The Teach Trace algorithms in the CNC can recognize both arcs and lines. This
reduces the overall memory required to store these parts and improves the
smoothness of the cut.
The traced part in memory is in EIA format and can be cut, saved or edited using any
of the part options.
Teach Trace has two modes, Remnant Trace and Teach Trace. The screen opens in
Remnant Trace mode. Press the Select Teach Trace Mode soft key to use Teach
Trace.
Remnant Trace Mode
In Remnant Trace mode, you can trace the outline of a plate remnant and save it as a
file so that it can be used later and nests of parts can be cut from the remnant.
To trace a remnant:
1. On the TeachTrace screen, press the Select Remnant Mode soft key.
1-5
Programmer’s Reference
2. Jog to the point on the Remnant window where you want the trace to begin. Use
the joystick or jog keys to move the torch over the plate.
3. Press or click First Point.
4. Jog to the next point and press or click Next Point.
Repeat this step until you have traced all but the final point.
5. When the pointer is over the last point you need to trace, press or click Last Point.
Trace Remnant draws a line between this point and the first point to close the
remnant.
6. Press or click OK to let TeachTrace create the remnant.
TeachTrace connects the last point to the first point automatically and returns to the
Preview Window.
7. Press or click Files then Save to Disk.
8. Select a folder for the new remnant file from the Save to dropdown list.
It is helpful to create a folder named Remnant to hold your remnant files.
9. Enter a file name in the File Name field.
10. Press or click OK.
Teach Trace Mode
1-6
Editing Part Programs
The Teach Trace function must be used with an optional stand-alone optical tracing
system.
1-7
Programmer’s Reference
To trace a part:
1. Press Select Auto Mode to trace the part automatically.
2. Press Select Manual Mode to trace the part manually.
This also enables the Change Move Speed button so you can change the speed at
which the sensor moves.
3. Select traverse or pierce.
You can switch between traverse and pierce during the tracing procedure.
4. Position the optical sensor near the part drawing.
5. Press Start.
Use the sensor positioning controls to direct the sensor towards the part.
6. After the sensor has located the part, the tracing system will follow the part outline
until completion.
7. If you are using manual mode, you can press the Change Move Speed button
repeatedly to select a speed for the optical sensor.
8. When the tracing system is finished tracing, press OK.
You can cut, save or edit the part.
1-8
Editing Part Programs
Start Corner Allows you to select where the part you trace will begin for proper
viewing on the screen.
Tracing Pitch Determines how precisely to learn a part. The Tracing Pitch can be
adjusted to favor the resolution or size of the taught part. This value
does not affect the actual position resolution of the part.
A good starting point for most tracing systems is 0.01”.
Arc Radial
Error
Auto Closure
Detect
Closure
Over/Under
Lap
Kerf Direction Selects the kerf for cut segments.
Traverse/Pierce Switches between the traverse and cut segments of the part as it is
Specifies the arc error tolerance to be used when checking the
current segment for dimensional accuracy. All ESSI or EIA programs
are comprised of lines, arcs, and circles. Arc Radial Error is used to
ensure that the starting and ending radial vectors are within
tolerance to describe a valid geometry.
Allows the CNC to detect that it has returned to the starting point.
With this feature on, the CNC stops the motion of the tracer when
the part is complete and programs a lead-out.
By specifying a positive value for this parameter, the CNC does not
stop the tracer until it has gone past the start point by the value of
this parameter.
Specify a negative value to stop the tracer as soon as the tracing
head position is within this parameter’s distance of the starting point.
This is only available if the Auto Closure Detect is On.
taught.
Select
Auto/Manual
Mode
Change Move
Speed
Select
Remnant Mode
Refer to the instructions provided with your Optical tracing system for additional
details.
Use this button to change trace modes.
If you select manual mode, you can also use the Change Move
Speed button to change the trace speed.
Press this button to change the trace speed in manual mode.
Press this button to use remnant mode to create remnants.
1-9
Programmer’s Reference
HyperCAD
HyperCAD is an easy to use 2D drawing application specifically designed for shape
cutting. The software’s powerful CAD utilities let users import DXF and CNC files or
draw from scratch. Files can be converted to graphical parts for editing and saving or
go directly to cutting.
HyperCAD is a simple CAD/CAM application that lets you move easily from drawing to
cutting. Its features include:
• English or Metric Units
• Part/sheet viewing capabilities
• Scaling, mirroring or rotating of parts
• Repeating and copying of shapes
• Moving/modifying of lead-ins and lead-outs
• Add-on of chamfers, fillets and notches
• On-screen, full-part cutting simulation
• Built in Help functions
This feature is offered as a limited use trial version. Contact your CNC vendor for
information on enabling unlimited use of this feature. This package may be used on the
CNC equipped with mouse and PC keyboard or offline on a PC.
1-10
Editing Part Programs
Automatic Nesting
Note: This software feature on the CNC is protected by a hardware key. If the
hardware key has been removed from the CNC, the following message appears when
the Nest Parts soft key is pressed.
Nesting Screen Layout
The preview window is located in the upper left corner of the Nester screen and is
used to preview manual nests. During an automatic nest, this area remains blank.
The plate size that is used during automatic nesting is based on plate information that
has been selected at the main setup screen.
The Files window in the upper right corner displays the list of part programs and
quantities of parts that have been selected for nesting. In the lower right, there are
fields to specify the location and name of the nest file.
1-11
Programmer’s Reference
Automatic Nesting Setup
To set up automatic nesting:
1. From the Main screen, select Shape Manager > Nesting > Setup.
2. Use the following setup parameters to configure the automatic nesting process.
Note: If the Setup soft key is not available (grayed out), the feature has not been
enabled on your CNC. Contact your CNC vendor for details on how to enable the
Automatic Nesting feature.
Nesting Switching Automatic to enable automatic nesting.
Part Spacing Sets the spacing between parts during automatic nesting process.
Plate Edge
Spacing
Program Origin Select the nest start location from the dropdown list.
Cut Direction From the dropdown list, select the direction in which the parts will be
Nest Direction Select the direction in which nests are arranged during the automatic
Sets spacing around the edge of the plate.
cut in the automatic nest.
nesting process.
1-12
Editing Part Programs
Return to Nest
Start
Use Remnant If remnants are created and saved for future use, select On to use
Generate and
Cut Offcut
M65 Auto
Reload
When enabled, the Return to Nest Start feature inserts a traverse
segment from the end of the nest back to the start point.
one of these remnants for automatic nesting.
Select On to generate offcuts for standard, rectangular nests.If this
feature is enabled, offcuts are created when 30% or more of the
sheet remains after nesting. The offcut is cut after a pause at the end
of the nest on the last nested rectangular sheet.
Select On to allow new sheets to be reloaded automatically.
When this feature is selected, there is a pause at the end of each
sheet until the operator presses Start to Resume. Then, a new sheet
automatically loads and runs.
Auto reload works with standard, rectangular nests only.
Using Automatic Nesting
To begin using Nesting:
1. On the Shape Manager screen, select Nester > Setups.
2. On the Setup screen, select Automatic for the Nesting option.
3. Configure the setup parameters.
4. Press OK to return to the Nesting screen and begin adding parts to the nest.
Adding a Part
To add a part to a nest part list:
1. On the Nesting screen, press the Add Part soft key.
1-13
Programmer’s Reference
2. On the Add Part screen, use the soft keys at the bottom to select the source of a
part file; Shape Library, disk, or host.
1-14
Editing Part Programs
3. Select the part you want to add:
• In the Shape Library, double-click or press a shape.
• On the Load from Disk screen, select the source of the file from the Load from
dropdown list and then select the file from the Files list.
• On the Download from Host screen, select the source of the file from the
Download dropdown list and then select the file from the Files list.
1-15
Programmer’s Reference
4. To narrow down the list of files in the Files list, click or press the Show Certain Files
soft key.
5. On the keyboard that displays, enter wildcard characters and a portion of the file
name you are looking for. For example, if you enter *Rect, you will see the following
list of files:
6. To return to the complete list of files, click or press Show All Files.
7. Select the Preview checkbox to view the part you selected in the Preview window.
8. Click or press Cancel to return to the Add a Part screen without adding the part.
9. Click or press OK to add the part to the nest.
10. On the Part Setup screen, enter values in the setup parameters, as necessary for
the part you selected.
1-16
Editing Part Programs
11. Click or press OK.
12. In the Part Configuration popup, enter the number of parts to include in the nest
and indicate whether the part will be mirrored in the nest, for greater efficiency, or
used as a wildcard part.
Wildcard parts “fill in” a sheet on which the nest occupies at least 75% of the sheet.
13. As you add new parts to the nest, file names and quantity are listed in the Files
window on the Nesting screen.
14. Save the nest of parts:
a. Select the file location from the Save to dropdown list.
b. Enter name for the nest file in the File name field.
c. Click or press OK to begin the automatic nesting process.
A window displays the progress of the nesting process.
1-17
Programmer’s Reference
Note: The nest process progresses quickly and all shapes may not be visible on the
screen. Other drawing anomalies may be noted during the nesting process.
If more parts are selected than can fit on one plate, multiple plates or sheets (nested
program) files are generated and saved in the selected folder with the selected file
name, but a numeric suffix is added. For example, if you saved the part file as Nest,
the nesting process may generate multiple part files named NEST1.txt, NEST2.txt,
NEST3.txt, and so on. The numbers in the file names indicate the number of individual
sheets that are needed for the nest selection, based on the sheet size parameter.
Deleting a Part
To delete a part from the part files list:
1. Select the part name in the files list.
2. Press the Remove Part soft key before you begin the nesting.
1-18
Editing Part Programs
When you have finished nesting your parts, you can view the entire nest in the Preview
Window of the Main screen:
Note: Parts with open loops or other invalid geometries may not be able to be
automatically nested. It may be possible to manually nest parts which have been
rejected by the Automatic Nesting function.
1-19
Programmer’s Reference
Nest Summary
After a nest is completed, the software provides a summary of the Automatic Nesting
process.
Statistical analysis of the process is provided for the number of sheets, time to execute
nest, total nest utilization and total number of shapes nested.
Note: Sheets that are generated with the same part configuration are listed as “Sheet
No. # (total #)”.
1-20
Editing Part Programs
To view the summary:
1. Scroll down to view an analysis of the parts, the individual sheets produced, and a
listing of the net utilization for the specific sheet.
2. Press OK to accept the nest and have the first sheet become the current part.
1-21
Programmer’s Reference
3. Press Cancel to reject the nest and return to the main nesting screen to add or
remove parts from the nest.
1-22
ASCII Codes
This appendix provides the 128 ASCII codes (American Standard Code for Information
Interchange) as defined by ANSI (American National Standards Institute) Standard
X3.4-1977.
Control Codes
Hex Dec Character Name Description
00 0 ^ @ NUL Null
01 1 ^A SOH Start of Header
02 2 ^B STX Start of Text
03 3 ^C ETX End of Text
04 4 ^D EOT End of Transmission
05 5 ^E ENQ Enquiry
06 6 ^F ACK Acknowledge
07 7 ^G BEL Bell
08 8 ^H BS Backspace
09 9 ^I HT Horizontal Tab
0A 10 ^J LF Line Feed
0B 11 ^K VT Vertical Tab
0C 12 ^L FF Form Feed
0D 13 ^M CR Carriage Return
0E 14 ^N SO Shift Out
0F 15 ^O SI Shift In
10 16 ^P DLE Data Link Escape
11 17 ^Q DCI Device Control 1
12 18 ^R DC2 Device Control 2
13 19 ^S DC3 Device Control 3
14 20 ^T DC4 Device Control 4
15 21 ^U NAK Negative Acknowledge
16 22 ^V SYN Synchronous Idle
17 23 ^W ETB End Transmission Block
18 24 ^X CAN Cancel
19 25 ^Y EM End of Medium
2-1
Programmer’s Reference
1A 26 ^Z Sub Substitute
1B 27 ^[ ESC Escape
1C 28 ^\ FS File Separator
1D 29 ^] GS Group Separator
1E 30 ^^ RS Record Separator
1F 31 ^_ US Unit Separator
20 32 SP Space
2-2
ASCII Codes
All Codes
Hex Dec Symbol Hex Dec Symbol Hex Dec Symbol
00 0 ^ @ 2B 43 + 56 86 V
01 1 ^A 2C 44 , 57 87 W
02 2 ^B 2D 45 - 58 88 X
03 3 ^C 2E 46 . 59 89 Y
04 4 ^D 2F 47 / 5A 90 Z
05 5 ^E 30 48 0 5B 91 [
06 6 ^F 31 49 1 5C 92 \
07 7 ^G 32 50 2 5D 93 ]
08 8 ^H 33 51 3 5E 94 ^
09 9 ^I 34 52 4 5F 95 _
0A 10 ^J 35 53 5 60 96 `
0B 11 ^K 36 54 6 61 97 a
0C 12 ^L 37 55 7 62 98 b
0D 13 ^M 38 56 8 63 99 c
0E 14 ^N 39 57 9 64 100 d
0F 15 ^O 3A 58 : 65 101 e
10 16 ^P 3B 59 ; 66 102 f
11 17 ^Q 3C 60 < 67 103 g
12 18 ^R 3D 61 = 68 104 h
13 19 ^S 3E 62 > 69 105 i
14 20 ^T 3F 63 ? 6A 106 j
15 21 ^U 40 64 @ 6B 107 k
16 22 ^V 41 65 A 6C 108 l
17 23 ^W 42 66 B 6D 109 m
18 24 ^X 43 67 C 6E 110 n
19 25 ^Y 44 68 D 6D 111 o
1A 26 ^Z 45 69 E 70 112 p
1B 27 ^[ 46 70 F 71 113 q
1C 28 ^\ 47 71 G 72 114 r
2-3
Programmer’s Reference
1D 29 ^] 48 72 H 73 115 s
1E 30 ^^ 49 73 I 74 116 t
1F 31 ^_ 4A 74 J 75 117 u
20 32 4B 75 K 76 118 v
21 33 ! 4C 76 L 77 119 w
22 34 “ 4D 77 M 78 120 x
23 35 # 4E 78 N 79 121 y
24 36 $ 4F 79 O 7A 122 z
25 37 % 50 80 P 7B 123 {
26 38 & 51 81 Q 7C 124 |
27 39 ‘ 52 82 R 7D 125 }
28 40 ( 53 83 S 7E 126 ~
29 41 ) 54 84 T 7F 127
2A 42 ‘ 55 85 U
←
2-4
1BEIA RS-274D Program Support
The control supports EIA RS-274D part programs. An EIA RS-274D program lists the
sequence of lines, arcs, speeds, kerf and I/O functions that are used to create a part.
While the user is free to program in EIA using the standard text editor, it is
recommended that the ShapeWizard® Graphical Programming environment be used
instead.
Following is a list of the EIA codes that are directly supported, mapped, or currently
unsupported by the control. Mapped EIA codes are automatically converted upon
program load into directly supported EIA codes. Unsupported EIA codes are ignored.
All other EIA codes generate an error.
10BDirectly Supported EIA Codes
EIA Code Description
Fvalue Machine Speed (if Speed Override enabled)
Nvalue Line Number
(text) Comments
Xvalue X Axis Endpoint or other Data
Yvalue Y Axis Endpoint or other Data
Ivalue I Axis Integrand or Part Option Data
Jvalue J Axis Integrand or Part Option Data
Ovalue Svalue Output (1-64), State (0-Off or 1-On)
Wvalue Svalue Wait for Input (1-64), State (0-Off or 1-On)
G00 Rapid Traverse Linear Interpolation
G00 AvalueSets Tilt angle – A is the angle value in degrees
G00 XYval Aval Performs Linear Interpolation of Tilt angle along line segment.
G01 Avalue
Sets Tilt angle value in degrees with a speed command in RPM
Fvalue
G00 Xn Yn Traverse command where n = value to move the desired axes a
distance.
G00 Zx.xx Tx Index Sensor™ THC height “Z” distance for torch “T”. Manual mode
only.
3-1
Programmer’s Reference
G00 Cxx Move to rotate “C” position
G01 Cxx Fxx Move to rotate “C” position with Speed “F” command in RPM
G00 C180- Rotate Axis offset 180 degrees will continue to rotate in the proper
direction
G00 C-180- Rotate Axis offset -180 degrees will continue to rotate in the proper
direction
G01 C180- Fxx Rotate Axis offset 180 degrees with speed
G01 C-180-
Fxx
G01 Linear Interpolation (at Cut Speed)
G02 Clockwise Circular Interpolation
G03 Counterclockwise Circular Interpolation
G04 Preset Dwell (uses Setup Dwell Time)
G04 XvalueProgram Dwell in Seconds
G08 XvalueRepeat Subroutine X Times
G20 Select English Units (inches)
G21 Select Metric Units (mm)
G40 Disable Kerf Compensation
G41 Enable Left Kerf Compensation
Rotate Axis offset -180 degrees with speed
G42 Enable Right Kerf Compensation
G43 Xvalue Kerf Value
G41 D1-200 Enables Left Kerf using a Kerf Table variable
G42 D1-200 Enables Right Kerf using a Kerf Table variable
G43 D1-200 Sets the current Kerf value via the Kerf Table using prior set Left /
Sets the Plasma Supply current through Outputs or Serial Link for
Vprocess (504,514,524,534) at Fcurrent value
V504 – Current Setting Plasma 1
V514 – Current Setting Plasma 2
V524 – Current Setting Marker 1
V534 – Current Setting Marker 2
Auto Align 3 Point Method with Long Offset Distance, Fast Speed,
Slow Speed values respectively
G92 Set Axis Presets
G97 Program Repeat Pointer
G97 Tvalue Program Repeat Pointer. Executes the repeat T times
G98 Repeat at G97, or start of program if no G97
G99 Part Options
M00 Program Stop
M01 Optional Program Stop (uses Setup Parameter)
M02 End of Program
M07 Cutting Device On
M08 Txx.xx Cutting Device Off (Temporary Optional Time Delay from –1 to 99.99
seconds)
M09 Enable Marker 1
M10 Disable Marker 1
3-3
Programmer’s Reference
M11 Marker Offset 1 On
M12 Marker Offset 1 Off
M13 Enable Marker 2
M14 Disable Marker 2
M15 Cut On
M16 Cut Off
M17 Oxy Gas On
M18 Oxy Gas Off
M19 Cancel All Stations
M26 Station Select On
M27 Station Select Off
M28 CBH / Rotator(s) Disable
M29 CBH / Rotator(s) Enable
M30 End of Program (same as M02)
M31 Reset Functions (Cut Off, Marker Off, Kerf Off)
M32 Unclamp / Unlock All Stations
M32 TvalueUnclamp / Unlock ‘T” Station, where T = 1 through 19
M33 Unclamp / Lock All Stations
M34 Clamp / Unlock All Stations
M34 TvalueClamp / Unlock ‘T” Station, where T = 1 through 19
M35 Clamp / Unlock All Stations Mirror
M35 Tvalue Clamp / Unlock Mirror “T” Station, where T = 1 through 19
M36 Tvalue Process Select “T” where T value selects the process
1 – Plasma 1
2 – Plasma 2
3-4
3 – Marker 1
4 – Marker 2
5 – Laser
EIA RS_274D Code Support
M37 Tvalue
(1-20)
M38 Tvalue
(1-20)
M40 Start of Subroutine
M40 Xvalue Start of Subroutine. Executes the repeat X times
M41 End of Subroutine
M48 Speed Override Enable
M49 Speed Override Disable
M50 Height Sensor Disable
M51 Txx.xx Height Sensor Enable (Temporary Optional Time Delay in seconds
M52 Height Sensor Disable and Raise Torch
Select Station “T” where T = 1 through 20
Deselect Station “T” where T = 1 through 20
before Enable)
M53 Height Sensor Enable and Lower Torch
M63 User Defined 1 On
M64 User Defined 1 Off
M54 User Defined 2 On
M55 User Defined 2 Off
M56 User Defined 3 On
M57 User Defined 3 Off
M58 User Defined 4 On
M59 User Defined 4 Off
M65 End of Program (same as M02) or Auto Reload
M72 Marker Offset 2 Off
3-5
Programmer’s Reference
M73 Marker Offset 2 On
M75 A Axis/Tilt Go to Home Command - Rapid Index
M76 C Axis/Rotate Go to Home Command - Rapid Index
M77 Go to Home position Y Axis
M78 Go to Home position X Axis
M79 Tvalue
(1-4)
M90 Aligns CBH / Rotator to Tangent angle of next cut segment
M90- Align rotator negative, when not using shortest path motion
M274 Marker Offset 3 Off
M275 Marker Offset 3 On
M276 Marker Offset 4 Off
M277 Marker Offset 4 On
M278 Marker Offset 5 Off
M279 Marker Offset 5 On
M280 Marker Offset 6 Off
M281 Marker Offset 6 On
Go To Home Position (1-4)
M282 Marker Offset 7 Off
M283 Marker Offset 7 On
M284 Marker Offset 8 Off
M285 Marker Offset 8 On
M286 Marker Offset 9 Off
M287 Marker Offset 9 On
M288 Marker Offset 10 Off
M289 Marker Offset 10 On
3-6
EIA RS_274D Code Support
M290 Marker Offset 11 Off
M291 Marker Offset 11 On
M292 Marker Offset 12 On
M293 Marker Offset 12 On
M301 Assigns the current X/Y position to Home Position 1
M302 Assigns the current X/Y position to Home Position 2
M303 Assigns the current X/Y position to Home Position 3
M304 Assigns the current X/Y position to Home Position 4
M305 Assigns the current X/Y position to Home Position 5
M306 Assigns the current X/Y position to Home Position 6
M307 Assigns the current X/Y position to Home Position 7
M308 Assigns the current X/Y position to Home Position 8
M309 Assigns the current X/Y position to Home Position 9
M310 Assigns the current X/Y position to Home Position 10
M311 Assigns the current X/Y position to Home Position 11
M312 Assigns the current X/Y position to Home Position 12
3-7
Programmer’s Reference
Mapped EIA Codes
EIA CODE DESCRIPTION MAPPED TO
G04 FvalueProgram Dwell G04 Xvalue
G05 Set Axis Presets G92
G21 Linear Interpolation G01 (at cut speed)
G22 CW Circular Interpolation G02
G23 CCW Circular Interpolation G03
G41 KvalueLeft Kerf with Value G41 with Kerf Value
G42 KvalueRight Kerf with Value G42 with Kerf Value
G97 TValue Subroutine Loop G08 Xvalue and M40
G45 Lead In to Kerfed Part G01, G02, or G03
G70 Select English Units G20
G71 Select Metric Units G21
G98 End of Subroutine Loop M41
M03 Cutting Device On/Off M07 (Oxy Fuel) or M08 as
appropriate
M04 Cutting Device On M07
M05 Cutting Device Off M08 (Oxy Fuel)
M06 Cutting Device Off M08
M06 Enable Marker 2 M13
M07 Disable Marker 1 or 2 M10 or M14 as appropriate
M08 Enable Marker 1 M09
M09 Disable Marker 1 or 2 M10 or M14 as appropriate
M10 Enable Marker 2 M13
M14 Height Sensor Disable M50
3-8
EIA RS_274D Code Support
M15 Height Sensor Enable M51
M20 Cutting Device On/Off M07 or M08 as appropriate
(Plasma)
M21 Cutting Device On/Off M07 or M08 as appropriate
(Plasma)
M20 Output 9 On O9 S1
M21 Output 9 Off O9 S0
M22 Output 12 On O12 S1
M23 Output 12 Off O12 S0
M24 Wait for Input 7 On W7 S1
M25 Wait for Input 8 On W8 S1
M25 CBH Enable M29
M26 Wait for Input 7 Off W7 S0
M26 CBH Disable M28
M27 Wait for Input 8 Off W8 S0
M67, M02 Kerf Left G41
M68, M03 Kerf Right G42
M69, M04 Kerf Off G40
M65, M70 Cutting Device On M07
M66, M71, M73 Cutting Device Off M08
M70 Marker Offset 1 Off M12
M71 Marker Offset 1 On M11
M70T01 Marker Offset 1 Off M12
M71T01 Marker Offset 1 On M11
M70T02 Marker Offset 2 Off M72
M71T02 Marker Offset 2 On M73
3-9
Programmer’s Reference
M70T03 Marker Offset 3 Off M274
M71T03 Marker Offset 3 On M275
M70T04 Marker Offset 4 Off M276
M71T04 Marker Offset 4 On M277
M70T05 Marker Offset 5 Off M278
M71T05 Marker Offset 5 On M279
M70T06 Marker Offset 6 Off M280
M71T06 Marker Offset 6 On M281
M70T07 Marker Offset 7 Off M282
M71T07 Marker Offset 7 On M283
M70T08 Marker Offset 8 Off M284
M71T08 Marker Offset 8 On M285
M98 End Comment )
M99 Start Comment (
M221 No Mirror, No Rotate G99 X1 Y0 I0 J0
M222 Mirror Y, No Rotate G99 X1 Y0 I0 J1
M223 Mirror X and Y G99 X1 Y0 I1 J1
M224 Mirror X, No Rotate G99 X1 Y0 I1 J0
M225 Mirror X/Y on -45 Deg G99 X1 Y270 I1 J0
M226 Rotate 90 Deg CCW G99 X1 Y90 I0 J0
M227 Mirror X/Y on +45 Deg G99 X1 Y270 I0 J1
M228 Rotate 90 Deg CW G99 X1 Y270 I0 J0
M245 Output 1 On O1 S1
M246 Output 1 Off O1 S0
M247 Output 2 On O2 S1
3-10
EIA RS_274D Code Support
M248 Output 2 Off O2 S0
M249 Output 3 On O3 S1
M250 Output 3 Off O3 S0
M251 Output 4 On O4 S1
M252 Output 4 Off O4 S0
M253 Wait for Input 1 On W1 S1
M254 Wait for Input 1 Off W1 S0
M255 Wait for Input 2 On W2 S1
M256 Wait for Input 2 Off W2 S0
M257 Wait for Input 3 On W3 S1
M258 Wait for Input 3 Off W3 S0
M259 Wait for Input 4 On W4 S1
M260 Wait for Input 4 Off W4 S0
Unsupported EIA Codes
EIA CODE DESCRIPTION
G30 Mirror Off
G46 Table 0 Select
G94 Feed per minute
G95 Feed per rev
G99 Freestanding G99
G103 QnameStop Current Program/ Load New Program
G201 Incremental Line In2
G202 Incremental CW Arc In2
G203 Incremental CCW Arc In2
G211 Incremental Line In3
3-11
Programmer’s Reference
G212 Incremental CW Arc In3
G213 Incremental CCW Arc In3
G221 Absolute Line In2
G222 Absolute CW Arc In2
G223 Absolute CCW Arc In2
G231 Absolute Line In3
G232 Absolute CW Arc In3
G233 Absolute CCW Arc In3
G240 Programmable Kerf
G247 Table 1 Select
G248 Table 2 Select
G249 Table 3 Select
G250 Table 4 Select
G276 Internal Variable Load
G277 External Variable Load
G278 X Axis Home
G279 Y Axis Home
G280 X Home Return
G281 Y Home Return
M66 PLC Control Code
M75 Ignored if not using CBH, Tilt Rotator(s)
M76 Ignored if not using CBH, Tilt Rotator(s)
M210 X Sign Toggle
M211 Y Sign Toggle
M212 X and Y Swap and Toggle
3-12
EIA RS_274D Code Support
M231 Aux. State Reset
M261 Aux. Torch Master On
M262 Aux. Torch Master Off
The unsupported EIA codes previously noted are ignored when read. Some of these
codes may be supported in the future. Any EIA codes that are not listed above will
result in a translator error upon loading the EIA program. Known EIA codes that will not
be accepted include, but are not limited to:
Pvalue Program Number
Dvalue Indexed Kerf Operations
VvalueInternal Variable Load
13BEIA Comments
Comments may be placed into the part program to be displayed on screen and viewed
by the operator. The comment line must first be preceded by a program stop command
(EIA M00 code or ESSI 0 code).
EIA Example:
M00 – Pauses Program
(Comment) – Text to be displayed
3-13
Programmer’s Reference
3-14
ESSI Code Support
The CNC supports ESSI part programs as defined by the International Standards
Organization in ISO 6582. An ESSI program lists the sequence of lines, arcs, speeds,
kerf and I/O functions used to create a part. While the user is free to program in ESSI
using a standard text editor, it is recommended that the ShapeWizard® Graphical
Programming environment be used instead.
While the user is free to download ESSI programs to the control, it is important to note
that all Part Programs will be internally converted to EIA for execution in the control.
Following is a list of the ESSI codes that are mapped into the control, or currently
unsupported by the control. Mapped ESSI codes are automatically converted upon
program load into directly supported EIA codes. Unsupported ESSI codes are ignored.
All other ESSI codes will generate an error.
Mapped ESSI Codes
ESSI CODE DESCRIPTION MAPPED TO EIA
% Start of Program Not Used-Automatic
+/-value… Line or Arc G00, G01, G02 or G03 as
appropriate
0 End Program or Stop M02 or M00 (if 64 is End Program)
3 Start Comment (
4 End Comment )
5 Enable Rapid Traverse Not Used-Automatic
6 Disable Rapid Traverse Not Used-Automatic
7 Cutting Device On M07
8 Cutting Device Off M08
9 Enable Marker 1 M09
10 Disable Marker 1 M10
11 Marker Offset 1 On M11
12 Marker Offset 1 Off M12
11+1 Marker Offset 1 On M11
4-1
Programmer’s Reference
12+1 Marker Offset 1 Off M12
11+2 Marker Offset 2 On M73
12+2 Marker Offset 2 Off M72
11+3 Marker Offset 3 On M275
12+3 Marker Offset 3 Off M274
11+4 Marker Offset 4 On M277
12+4 Marker Offset 4 Off M276
11+5 Marker Offset 5 On M279
12+5 Marker Offset 5 Off M278
11+6 Marker Offset 6 On M281
12+6 Marker Offset 6 Off M280
11+7 Marker Offset 7 On M283
12+7 Marker Offset 7 Off M282
11+8 Marker Offset 8 On M285
12+8 Marker Offset 8 Off M284
13 Enable Marker 2 M13
14 Disable Marker 2 M14
15 Marker Offset 2 On M73
16 Marker Offset 2 Off M72
21 No Mirror, No Rotate G99 X1 Y0 I0 J0
22 Mirror Y, No Rotate G99 X1 Y0 I0 J1
23 Mirror X and Y G99 X1 Y0 I1 J1
24 Mirror X, No Rotate G99 X1 Y0 I1 J0
25 Mirror X/Y on -45 Deg G99 X1 Y270 I1 J0
26 Rotate 90 Deg CCW G99 X1 Y90 I0 J0
4-2
ESSI Code Support
27 Mirror X/Y on +45 Deg G99 X1 Y270 I0 J1
28 Rotate 90 Deg CW G99 X1 Y270 I0 J0
29 Enable Left Kerf Comp G41
30 Enable Right Kerf Comp G42
38 Disable Kerf G40
39+value Machine Speed Fvalue
40+valueProgrammable Kerf G43 Xvalue
41 Preset Dwell G04
41+valueProgram Dwell in mSec G04 Xvalue
45 Ht Sensor Enable/Lower M53
46 Ht Sensor Disable/Raise M52
47 Ht Sensor Enable M51
48 Ht Sensor Disable M50
51 CBH Enable M29
52 CBH Disable M28
53 Cutting Device On M07
54 Cutting Device Off M08
63 Reset Functions M31
64 End Program M02
65 End of Program/ Reload M65
67 Ht Sensor Disable M50
68 Ht Sensor Enable M51
70 Select English Units (in) G20
71 Select Metric Units (mm) G21
79+1 Go To Home Position 1 M79 T1
4-3
Programmer’s Reference
79+2 Go To Home Position 2 M79 T2
79+3 Go To Home Position 3 M79 T3
79+4 Go To Home Position 4 M79 T4
81 Incremental Mode G91
82 Absolute Mode G90
83 Set Axis Presets G92
90 End of Program M02
97 Program Repeat Pointer G97
97+value Subroutine Loop M40 Xvalue
98 Repeat at 97, Subroutine loop G97, G98 or M41 as appropriate
or start of program if no 97
99 End of Program M02
245 Output 1 On O1 S1
246 Output 1 Off O1 S0
247 Output 2 On O2 S1
248 Output 2 Off O2 S0
249 Output 3 On O3 S1
250 Output 3 Off O3 S0
251 Output 4 On O4 S1
252 Output 4 Off O4 S0
253 Wait for Input 1 On W1 S1
254 Wait for Input 1 Off W1 S0
255 Wait for Input 2 On W2 S1
256 Wait for Input 2 Off W2 S0
257 Wait for Input 3 On W3 S1
4-4
258 Wait for Input 3 Off W3 S0
259 Wait for Input 4 On W4 S1
260 Wait for Input 4 Off W4 S0
282 Marker Offset 3 On M275
283 Marker Offset 3 Off M274
284 Marker Offset 4 On M277
285 Marker Offset 4 Off M276
286 Marker Offset 5 On M279
287 Marker Offset 5 Off M278
288 Marker Offset 6 On M281
ESSI Code Support
289 Marker Offset 6 Off M280
290 Marker Offset 7 On M283
291 Marker Offset 7 Off M282
292 Marker Offset 8 On M285
293 Marker Offset 8 Off M284
Unsupported ESSI Codes
ESSI CODE DESCRIPTION
103+Name Stop Current Program/ Load New Program
237 X Sign Toggle
238 Y Sign Toggle
239 X and Y Swap and Toggle
266 Table 1 Select
267 Table 2 Select
268 Table 3 Select
4-5
Programmer’s Reference
269 Table 4 Select
276 Internal Variable Load
277 External Variable Load
278 X Axis Home
279 Y Axis Home
280 X Home Return
281 Y Home Return
The unsupported ESSI codes above are ignored when read. Some of these codes may
be supported in the future. Any ESSI codes that are not listed above will result in a
translator error upon loading the ESSI program.
ESSI Comments
Comments may be placed in to the part program to be displayed on screen and viewed
by the operator. The comment line must first be preceded by a program stop command
(EIA M00 code or ESSI 0 code).
ESSI Example:
0 – Pauses Program
3 – Start Comment
Comment – Text to be displayed
4 – End Comment
4-6
Advanced Feature Codes
Kerf Table Codes
CODE DESCRIPTION
G59 D1200Xvalue
G41 D1-200 Enables Left Kerf using a Kerf Table variable
G42 D1-200 Enables Right Kerf using a Kerf Table variable
G43 D1-200 Changes current kerf value via Kerf Table using previously set left or right
Sets kerf table variable from 1-200
kerf
Tilt / Rotator Part Codes
CODE DESCRIPTION
G00 Avalue Sets tilt angle as a preparatory command – A is the angle value in
degrees
G00 XYvalue
Avalue
G00 Avalue
Fvalue
Performs Linear Interpolation of Tilt angle along line segment.
Sets tilt angle – Angle value in degrees with a speed command in
RPM
M28 Disables Follower
M29 Enables Follower
M90 Preparatory Cmd - Aligns Rotator to Tangent angle of next cut
segment
M90- Align rotator when not using shortest path motion
M75 A axis/Tilt Goto Home Cmd - Rapid Index
G00 Cxx Move to rotate “C” position
G01 Cxx Fxx Move to rotate “C” position with Speed “F” command
G00 C180- Rotate Axis align 180 degrees will continue to rotate in the proper
direction
5-1
Programmer’s Reference
G00 C-180- Rotate Axis align -180 degrees will continue to rotate in the proper
direction
G01 C180- Fxx Rotate Axis align 180 degrees with speed
G01 C-180-
Fxx
Rotate Axis align -180 degrees with speed
Automatic Torch Spacing Program Codes
CODE DESCRIPTION
M32 Unclamp / Unlock All Stations
M33 Unclamp / Lock All Stations
M34 Clamp / Unlock All Stations
M34Tvalue Clamp / Unlock ‘T” Station, where T = 1 through 19
M35 Clamp / Unlock All Stations Mirror
M35Tvalue Clamp / Unlock Mirror “T” Station, where T = 1 through 19
M77 Go to Home position Y Axis
M78 Go to Home position X Axis
Station Select Codes
Stations (Lifter / THCs) can be selected and de-selected using the following EIA-274D
program codes.
CODE DESCRIPTION
M19 Tvalue Cancel All Station Selections
M37 Tvalue Select Station 1-20 (Tvalue)
M38 Tvalue De-Select Station 1-20 (Tvalue)
Additionally, these Station Select program codes may be overridden using the user
selected THC inputs to the CNC. The feature to override the part program must be
enabled at the Cutting Setup screen.
5-2
Advanced Feature Codes
Process Select Codes
Process selections can be made using a EIA-274D program code in the following
format.
T1 = Plasma Process 1
T2 = Plasma Process 2
T3 = Marker Process 1
T4 = Marker Process 2
T5 = Laser Process
Station Configuration Variables
The following options are available for station configuration:
Lifter
None Sensor THC Command THC
(with Serial Link)
HD4070 Integrated THC 1
or 2
(used only with the HD4070
power supply)
Other
(any standalone lifter
station)
Power Supplies
None HD4070 Torch 1or 2 Powermax series
Max100/ 100D HT4001 FineLine 100
Max200 HT4100 FineLine 200
HT2000 HT4400 Other (any other Plasma
system)
HD3070 HPR130
5-3
Programmer’s Reference
Marker
None ArcWriter FineLine 100 & 200
HD4070 Torch 1or 2 HPR130 Other (any stand alone
Marker)
Laser
Rofin RF 40 & 50 Rofin DC 35 Rofin TR 60 Other
Automatic Torch Spacing
The automatic torch spacing feature uses codes within the part program, and
designated outputs, to perform precise positioning of individual torch stations for multitorch cutting processes.
This feature must be enabled in Machine Setups. The Auto Torch Spacing Override
feature in Cutting Setups must also be enabled.
In this process, the primary torch station has a fixed mount to the transverse axis and
the other secondary torch stations have the ability to clamp to the mechanics of the
transverse axis during use or lock to the gantry or beam when not in use.
For the example, in the following illustration, Torch 1 is the primary station and Torch 24 are the secondary stations.
Typical use is as follows:
1. Unclamp and unlock all stations (except the first which is fixed and slides the others)
2. Go to Home Command on Transverse Axis (M77 or M78 depending on orientation)
5-4
Advanced Feature Codes
3. Clamp and Unlock all carriages and G00 index inward on transverse (optional
command - may used to space all stations away from edge / OT switch of machine)
4. Lock and Unclamp all and G00 index to space first station (remember-first station
has no clamping/locking on board)
5. Unlock and Clamp next station and G00 index to space the next station.
6. Repeat Step 5 until as many stations as needed are spaced.
Note: Homing also automatically includes the commands necessary to push the
stations to the side and lock or clamp them whenever the transverse is homed, if Auto
Torch Spacing is enabled. Unclamp/ Clamp and Unlock / Lock commands execute a
one second delay before moving.
5-5
Programmer’s Reference
Automatic Torch Spacing Program Codes
Code Description
M32 Unclamp / Unlock All Stations
M33 Unclamp / Lock All Stations
M34 Clamp / Unlock All Stations
M34Tvalue Clamp / Unlock ‘T” Station, where T = 1 through 19
M35 Clamp / Unlock All Stations Mirror
M35Tvalue Clamp / Unlock Mirror “T” Station, where T = 1 through 19
M77 Go to Home position Y Axis
M78 Go to Home position X Axis
G00 Xn Yn Traverse command where n = value to move the desired axes a
distance.
Automatic Torch Spacing I/O
Station Lock
1-19
Station Clamp
1-19
Station Mirror
1-19
Locks the unused torch station to the gantry or beam when not in use.
Clamps the selected torch station to the transverse axis for standard
cutting.
Clamps the selected torch station to the transverse axis for mirrored
cutting.
Automatic Plate Alignment Codes
Three point alignment distance and speeds can be defined with the following EIA format
program code:
G66D100B300C30
G66 3-point alignment command
DvalueDistance between two plate edge reference points
BvalueRapid feed rate for distance (D) motion
CvalueSlow feed rate for the distance to the edge
5-6
Advanced Feature Codes
Example Part Program
The transverse axis is configured as the X axis
Three station cut of 20 inch vertical rip.
Code Description
G70 English Units
G91 Incremental Mode
G99 X1 Y0 I0 J0 Axes Preset zero Scaling
M32 Unclamp / Unlock All Stations
M78 Home X Axis (move all stations to Home position)
M34 Clamp All / Unlock All
G00X2Y0 Traverse X axis 2 inches (to move off edge/ switch)
M33 Unclamp All / Lock All
G00X10Y0 Traverse X axis 10 inches (to set 10 inch space – station 1)
M34 T1 Clamp Station 1 / Unlock Station 1
G00X10Y0 Traverse X axis 10 inches (to set 10 inch space– station 2)
M34 T2 Clamp Station 2 / Unlock Station 2
G41 Left Kerf
M07 Cut On
G01 X0 Y20 Line segment (Y axis 20 inches)
M08 Cut Off
G40 Kerf Off
M02 End of Program
5-7
Programmer’s Reference
5-8
Subparts
Subparts allow you to call and execute a separate part file within a part program using a
simple line of text.
To configure a subroutine part for use, the user must first create a folder on the CNC
hard drive named “SUBPARTS”. To create a folder on the hard drive, select Load From
Disk. With the folder location highlighted, press the + key to create a new folder.
Save the part program in the SUBPARTS folder.
To execute the part, insert a line of code within the part program with the following
format.
PFILENAME
Start the line of code with the letter P to indicate that a Sub Part is to be executed,
followed by the filename for the desired part program.
For example, to execute subpart L-Bracket after completing a simple 5” x 5” square with
a programmed traverse, the part program would look something like the following
example:
When it is executed, this program will be represented as the original part plus the
additional subpart and will include the programmed traverse.
Note: Subparts can also contain subparts. After being translated by the CNC, the final
text of the part will contain the complete text of the original part and subpart.
6-2
Marker Font Generator
The Marker Font Generator feature can be used to label or identify parts with a marking
device before cutting. This is accomplished by use of a simple command string within
the part program code to call existing text characters (fonts) and execute marking of the
selected text.
The program code uses a specific format and is structured to provide information to be
used when marking. Information on the font source location, scale factor, angle, marker
tool, tool offset and text are entered as information blocks in the command string. Each
section or information block in the command string is separated by a space. The format
of this command code is outlined as follows:
Note: If a value is not present for a specific information block, the default values will be
used. The default values are:
Font (F): Internal
Angle (A): 0
Offset (O): #1
Scale (S): One
Marker (M): #1
Example of a simple command string:
<F2 S2 A45 M2 O2 <TEST 123>
< The program command must begin with the “<” symbol to indicate that the
Marker Font Generator feature is being used.
F The first block of information is the Font Source location. The “F” is followed by
a digit to indicate the location where the font is stored:
1 = an internal font in the control software
2 = a font located on the CNC hard drive
3 = a font from diskette or USB memory.
If no font is found at the selected location, the default internal font will be used.
For the example given, the font location would be from the hard drive.
S The second information block determines the scale of the text. The “S” is
followed by a number that indicates the scale factor. For the example given, the
scale factor is twice the original font dimensions.
A The third information block determines the angle of the text. The “A” is followed
by a number that indicates the degree of angle. For the example given, the
7-1
Programmer’s Reference
degree of the angle is 45.
M The fourth information block determines the Marker Tool to be used. The “M” is
followed by the number of the marker tool (Marker Enable Output) to be used.
Up to two marker enables are supported.
O The fifth information block determines which tool Offset to be used. The “O” is
followed by a number indicates that one of the nine different tool offsets
previously configured in control setups is to be used. The example shown
indicates that tool offset number two should be used.
< > The final information block is used to specify the marker text to be executed.
The text must be enclosed in the ”<” and “>” marks to be valid and understood
as the selected text. For the example given, the marker text executed would be
“TEST 123”
When the previous code example is translated by the CNC, it generates the Marker
Text “TEST 123” onto the plate as shown here in Shape Wizard.
To improve the ease of use for the part program designer and control operator, the
marker font generator always inserts a traverse segment to return to the original start
point at the beginning of the marking text.
7-2
Marker Font Generator
Internal Fonts
The internal fonts located within the control software are 1” high and are limited to
characters available on the control keypad. Alphabetical characters are limited to upper
case letters only.
External Fonts
External fonts can be loaded from a floppy disk or from the control hard drive. When the
CNC generates the text, the CNC searches for part files to correspond to the selected
character. The part file names must be based on their ASCII numeric equivalent and
have a .txt file extension.
For example, for the marker text “Ab 12”, the control searches for the following files to
generate the text:
Text ASCII No. File Name
Capital A 65 Ascii65.txt
Lower case b 98 Ascii98.txt
Space 32 Ascii32.txt
No 1 49 Ascii49.txt
No 2 50 Ascii50.txt
For more information on ASCII codes, refer to the ASCII Codes chapter.
Font programs may be saved on the control hard drive by creating a folder labeled
“Fonts” using the “Save to Disk” feature and saving the font programs within this folder.
Remember, if a corresponding part file to text requested is not found at the selected
source location, the internal font file will be used.
Custom Fonts
Custom fonts can be used when using the marker font generator. To construct these
font files, certain guidelines should be adhered to.
1. Programming format must be EIA
2. Only M09 and M10 can be used to enable and disable the marker.
3. Only G00, G01, G02 and G03 codes can be used.
4. The program must end in an M02.
5. The proper file name must be assigned to the font program.
6. The font program must begin in the lower left and end in the lower right.
7. Font programs should have the consistent dimensional limits (i.e. 1’ high, etc.).
The darker lines in the drawing represent the Traverse segment and the lighter lines
represent the Marking lines. You can see by this illustration that at the end of the font
program, a traverse is used to continue motion to the bottom right corner.
Note: The Burny 3/5 style of programming for the Marker Font Generator feature is also
supported for the default internal font source.
7-4
Sensor THC Programming Support
The Sensor THC allows you to configure THC setup parameters through part program
codes.
The following parameters are available using EIA-274D G59 codes:
• Arc Voltage
• Pierce / Start Time
• Pierce/ Start Height Factor
• Cut / Mark Height
• Transfer Height Factor
Use the following format to set up the Sensor THC in a part program:
G00 Zx.xx Tx Index Sensor THC height “Z” distance for torch “T”. Manual mode only.
8-2
Plasma Supply Programming Support
HPR and HD4070 Support
The same cut chart data that is used on the cut chart setup screen can also be used
within a part program to configure the power supply for use. This code is used to select
the set point for each variable.
Only the variables that you are changing need be inserted into the part program. You do
not have to insert a line of code for each cut chart variable within a part program.
Part program codes for the power supply should be grouped together at the beginning of
the program. The three variables that can be set through the part program are Material
Type, Current Setting and Material Thickness.
Cut parameters for the power supply can be configured using the EIA-274D G59 code
with the following format:
G59 V503 F5
G59 Any G code
V5xxThe variable identity:
V503 – Material Type Plasma 1
V513 – Material Type Plasma 2
V523 – Material Type Marker 1
V533 – Material Type Marker 2
V504 – Current Setting Plasma 1
V514 – Current Setting Plasma 2
V524 – Current Setting Marker 1
V534 – Current Setting Marker 2
V507 – Material Thickness Plasma 1
V517 – Material Thickness Plasma 2
V527 – Material Thickness Marker 1
V537 – Material Thickness Marker 2
9-1
Programmer’s Reference
FxThe variable value, which depends on the variable identity:
For material type V503, V513, V523, V533:
Add .0x for Specific Material x (for example: V503 F1 .01 for mild steel,
specific material 1)
Note: Programming a code for a nonexistent process will result in an invalid process.
HD3070 Support
The same valve setting data that is used on the Auto Gas setup screen can also be
used within a part program to configure the HD3070. This code is used to select the
valve and indicate the valve set point.
Use a EIA-274D G59 code with the following format:
G59 V65 B5
G59 Any G code
Vxx The valve identity:
V65 = Preflow Shield Gas - Valve 1
V66 = Preflow Shield Gas - Valve 2
V67 = Cut Shield Gas - Valve 3
V68 = Cut Shield Gas - Valve 4
63 4” 4” 100mm
V69 = Cut Plasma Gas - Valve 5
V70 = Cut Plasma Gas - Valve 6
V71 = Remote Plasma Gas Type
Bx The valve value, which depends on the valve identity:
For Valves V65 – V70, a whole integer is used to set the desired
percentage value.
For Valve 71:
0 = Oxygen
1 = H35/N2
2 = Air
9-5
Programmer’s Reference
For this example, the part program code (G59 V65 B5) would set the autogas preflow
shield gas valve to 5%. Multiple G59 codes can be used to set and adjust all the
necessary valves.
FineLine Support
The same Cut Chart data which is used at the Cut Chart setup screen may also be used
within a part program to configure the FineLine power supply. This code is used to
select the set point for each variable.
It is not necessary to have a line of code for each cut chart variable within a part
program. Only those variables that are changing need be inserted into the part program
(e.g. Material Thickness or Material Type).
Part program codes for the FineLine should be grouped together at the beginning of the
program. The three variables which can be set through the part program are Material
Type, Current Setting and Material Thickness.
Configure cut parameters for the FineLine using an EIA-274D G59 code with the
following format:
G59 V503 F5
G59 Any G code
Vxxx
The variable identity:
V503 – Material Type Plasma 1
V513 – Material Type Plasma 2
V523 – Material Type Marker 1
V533 – Material Type Marker 2
V504 – Current Setting Plasma 1
V514 – Current Setting Plasma 2
V524 – Current Setting Marker 1
V534 – Current Setting Marker 2
V507 – Material Thickness Plasma 1
V517 – Material Thickness Plasma 2
V527 – Material Thickness Marker 1
V537 – Material Thickness Marker 2
FxThe variable value, which depends on the variable identity:
For material type V503, V513, V523, V533:
Add .0x for Specific Material x (for example: V503 F1 .01 for
mild steel, specific material 1)
The Serial Messaging feature may be used to pass commands embedded within a part
program through a selected serial port to an external device. Both RS-232 and RS-422
are supported. TCP/ IP protocol is not supported at this time. There are 2 Serial
Messaging ports available.
Overview
Serial Messaging has a fairly basic communication protocol that has three simple
formats to send ASCII codes as command strings. During the messaging function, a
status indicator for “Message Transmit”, “Message Delay” or “Message Verify” will be
displayed in the Watch window.
Options
• While the selected message is sent to the external device, the part program will be
temporarily suspended. After completion of the transmission, the part program will
then automatically resume. No acknowledgement from the external device is
required. An additional Time Delay may also be added.
• A message is sent concurrent to execution of the part program and no delay is
encountered. No acknowledge is required. No Delay Time is allowed.
• The message is sent with a suspension of the program during transmission as in the
first option, but an Acknowledge from the external device (ACK) is required before
the part program can continue. A Non-Acknowledge (NAK) response from the
external device will prompt a retransmit of the message from the control. An optional
Time Out value may be added to the program code. If no Time Out code is used in
the program code the Default time out value at the Ports setup screen will be used.
Additionally, an optional automatic retry feature may be enabled at the Ports setup
screen.
To enable use of this feature, assign Messaging to the selected port(s) at the Ports
setup screen.
After you enable serial messaging, the flow control parameters that communicate with
the external device must be selected.
10-1
Programmer’s Reference
The following parameters must be configured. Hardware and flow control configuration
information must match the external device.
Time Out The Time Out value may be used for the Message Type 22 (which
requires an acknowledgement from the external device after the
message) if there is no Time Out value used in the command string of
the program code.
Baud Rate Select a communication speed from 1200 to 115200 Baud.
Flow Control Select to use None, Xon/Xoff or Hardware.
During Jog on
Path
Select whether messages will be sent when jogging Forward or
Backward on Path while at the Pause screen.
Notes:
• All messaging will stop when the Stop Key has been pressed or
the Remote Pause input becomes active.
• The Message Type 21 will transmit the message concurrent to the
associated motion segment during Backup on Path.
Parity Select None, Odd or Even.
10-2
Data Bits Select 7 or 8 Data Bits.
Serial Messaging
Retry on Time
Out
For the Message Type 22 (which requires an acknowledgement from
the external device after the message) an automatic retransmit of the
message may be sent. The user may select the number of retries
allowed before faulting from a lack of response from the external
device. The fault prompt “Message Error” will be displayed when in a
Time Out condition.
Programming Code
The ASCII message string follows a unique program message format. Each command
begins with a “>” character and ends with a “<” character. These characters are used as
delimiters to frame the command (Message Type, Optional Format and Optional Delay
Time/Time Out) instructions for the message.
Message Information
The format of this command code is outlined as follows:
>20+Format+Delay Time/Time Out+Port<Message
>2xMessage Command type (see Message Command Type section):
>20 = Direct message with Delay
>21 = Direct message without Delay
>22 = Message that requires Acknowledge
Format Optional format value that allows the user to add:
Line Feed and Carriage Return commands, etc., message
string.
0,1,16,17,32,33,48,49,64,65,80,81,96,97,112,113 are
supported (see Format Value section).
Delay Time/
Time Out
Port Optional serial port number:
Message The message content (see the message text section.)
Optional delay time/time out value
Time in seconds (see Time Out Value section.)
0 = Default port 1
1 = Port 2
Note: Serial message format is always written within comment
characters and the command portion of the program code is between
the “>” Character and the “<” Character.
10-3
Programmer’s Reference
ESSI Example:
3
>20,1,1,0<Message
4
EIA Example:
(>20,1,1,0<Message)
Note: You can use the plus sign (+), hyphen (-), comma (,) or space as a delimiter
between fields for the command instruction.
Message Command Type
>20< This command delays the part program until all bytes have been
transmitted, then optionally waits the Delay Time, if specified.
>21< A message is sent concurrent to execution of the part program and no
delay is encountered. No acknowledge is required.
>22< The message is sent with a suspension of the program during
transmission as in option one, but an Acknowledge from the external
device (ACK = Hexadecimal 06) is required before the part program
can continue. A nonacknowledge (NAK = Hexadecimal 15) response
from the external device will prompt a retransmit of the message from
the control.
An optional Time Out value may be added to the program code. If no
Time Out code is used in the program code the Default time out value
at the Ports setup screen will be used. Additionally, an optional
automatic retry feature may be enabled at the Ports setup screen.
With the automatic retry feature the message will automatically be
retransmitted if no response is detected. The retry is executed after
the Time Out value has elapsed. The number of retries can be
defined on the Ports configuration screen.
10-4
Serial Messaging
Optional Format Value
The following specialty characters for the format can be sent, in addition to a command
string.
Specialty Characters Supported
HEX Name Description
01 SOH Start of Header
02 STX Start of Text
03 ETX End of Text
04 EOT End of Transmission
0A LF Line Feed
0D CR Carriage Return
BCC “Exclusive Or” Check Byte
Note: Checksum is always an 'Exclusive OR' of the Data because it does not include
any of the 'Format' characters, including the CR/LF option.
Optional Format Character Assignments
Value Assignment
0 No special assignment (must be used in the format location if a Delay
or Port is required but no Format options are required).
Append a Carriage Return (<CR> = Hex value OD) and a Line Feed
(<LF> = Hex Value0A).
16 Append an “Exclusive OR” (<BCC>) to the end of the message.
17 Appends a combination of 16 and 1.
32 Encloses the message with Start of Text (<STX> = Hex Value 02) and
End of Text (<ETX> = Hex Value 03).
The <ETX> follows the message and the optional <CR><LF>>
append codes but precedes the Check Byte <BCC>.
33 Appends a combination of 1 and 32.
48 Appends a combination of 16 and 32.
10-5
Programmer’s Reference
49 Appends a combination of 1, 16 and 32.
64 Append a Start of Header (<SOH> = Hex value 01) and an End of
Transmission (<EOT> = Hex Value04) to the message.
65 Appends a combination of 1and 64.
80 Appends a combination of 16 and 64.
81 Appends a combination of 1, 16 and 64.
96 Appends a combination of 32 and 64.
97 Appends a combination of 1, 32, and 64.
112 Appends a combination of 16, 32 and 64.
113 Appends a combination of 1, 16, 32 and 64.
Optional Delay Time/Time Out Value
The Delay Value issues a delay in seconds at the end of the message for Message
Type 20.
No delay is supported for Message Type 21.
This value also works as a Time Out value for Message Type 22. An error will be
displayed if the message is not acknowledged (ACK Hexadecimal 06) within the
specified time. If no Time Out Delay is defined in the command, the Time Out parameter
on the Ports screen will be used.
The value is in a 3.2 format where a value of 5 is equal to 5.00 seconds. Accepted limits
for the value is range of 0.00 to 999.99 seconds.
If there is no delay, but the optional port below is being selected, then 0 is required to be
entered in the optional delay location.
Optional Port
The Optional Port setting selects which Messaging Port to use. The default messaging
port to use is Port 1 if this parameter is omitted. If the optional port is used, 0 =
Messaging Port 1 and 1 = Messaging Port 2.
Message Text Content
Up to 300 data characters in each command string may be sent. The Command
characters (information between and including the “>” and “<” signs) are included in this
maximum.
Printable and Non- Printing ASCII codes can be used in the message string. For more
information on ASCII codes and the Hexadecimal value, refer to the ASCII Code
chapter.
10-6
Serial Messaging
Non-printing characters are supported by use of a two-character command and can
send a Binary Code in the Range from 0-255. Double byte character to support
combinations will affect the maximum length count with each pair reducing the
maximum data characters by 1. For more information on these values, refer to the Nonprinting Character section.
Non-Printing Characters
Non Printing Characters are supported through use of a pair of two printing codes to
equal the non-printing code. This pair of characters is retained in the program code but
sent as single 8-bit code when transmitted.
There are three types of character pairs and each performs a different operation based
on the first character of the pair. This produces a single modified character for
transmission.
Character Options
• The “&” two-character pair clears the 0x40 bit from the 2nd character code value.
• The “!” two-character pair clears the 0x40 bit and sets the 0x80 bit set in the 2nd
character code.
• The “$” two-character pair clears the 0xC0 bit in the 2nd character.
To transmit the single character with a value 0x01, use the two-character sequence
”&A”. This converts the “A” value of 0x41 to 0x01 by clearing the 0x40 bit.
To transmit 0x81, use “!A” or to transmit 0xC1, use “$A”.
Exceptions / Additions
As the “&”, “!” and “$” are used as key indicators for the non-print characters, there is a
special format used when these characters are used as a print character in the
message text. Simply use the character twice. “&&” = “&”
The ESSI style part program uses several unique characters which requires special two
character codes to be used. For example, the message code “&K” in the part program
will transmit the code value of 0x2B which is the ASCII code for the plus sign (+). In
order to send the + character the code “&K” must be used.
The following are unique codes used in WORD ADDRESS and ESSI programs.
Code Code Value Description
&’ 0x20=space At end of ESSI program
&h 0x28 = “(“ To transmit “(” from WORD ADDRESS program
&i 0x29 = “)“ To transmit “)” from WORD ADDRESS program
&? 0x7F = DEL Non-printable DELETE code
&K 0x2B = “+” To transmit “+” from ESSI program
!c A3 !k AB !s B3 !; BB
!d A4 !l AC !t B4 !< BC
!e A5 !m AD !u B5 != BD
!f A6 !n AE !v B6 !> BE
!g A7 !o AF !w B7 !? BF
$@ C0 $H C8 $P D0 $X D8
$A C1 $I C9 $Q D1 $Y DD
$B C2 $J CA $R D2 $Z DA
$C C3 $K CB $S D3 $[ DB
$D C4 $L CC $T D4 $\ DC
$E C5 $M CD $U D5 $] DD
$F C6 $N CE $V D6 $^ DE
$G C7 $O CF $W D7 $_ DF
$` E0 $h E8 $p F0 $x F8
$a E1 $I E9 $q F1 $y F9
$b E2 $j EA $r F2 $z FA
$c E3 $k EB $s F3 $; FB
$d E4 $l EC $t F4 $< FC
$e E5 $m ED $u F5 $= FD
$f E6 $n EE $v F6 $> FE
$g E7 $o EF $w F7 $? FF
10-9
Programmer’s Reference
10-10
Importing Prepared DXF Files
The DXF Translator software allows the control to load and translate a DXF style
drawing created in Autocad ® or Autocad LT® into an EIA part program. Certain
guidelines must be observed when creating the CAD drawing to allow the control to
load and understand the file. The optional DXF translation utility is enabled through a
password provided by your control supplier.
Drawing Format
There should be nothing on the cut layer except lines, arcs, circles and text
commands. Do not put dimensions or notes on the same layer as cut data.
Elliptical segments, squares and polylines are not supported. Divide these elements
into short arcs or line segments. You can use the ACAD EXPLODE command to
convert POLYLINES into segments.
The end angles of two arcs from any intersection point cannot be within the same
quadrant.
Text commands determine cut sequence, and determine the path through multisegment intersections. Text commands are placed on the drawing with the text feature
of your CAD program. The size of the text is not important. However, the location of
the text is extremely important. Text must be left-justified and text commands must be
snapped to the appropriate intersection or pierce points.
Text commands indicate pierce points and cut direction. Note that the directional
commands should only be used to determine the direction of the next line segment
when more than one exit path exists at an intersection of segments.
Text Commands
1 Indicates the first pierce point (subsequent pierce points follow in numerical order)
+ Indicates a Counter-Clockwise circle
- Indicates a Clockwise circle
Directional Commands
The following commands indicate the next segment’s direction, if it is a line, or the
ending angle, if it is an arc, if the angle is:
R 350° to 10°
RU 0° to 45°
UR 45° to 90°
U 80° to 100°
UL 90° to 135°
LU 135° to 180°
11-1
Programmer’s Reference
L 170° to 190°
LD 180° to 225°
DL 225° to 270°
D 260° to 280°
DR 270° to 315°
RD 315° to 360°
Traverses are automatically determined between pierce points and do not need to be
entered on the CAD drawing.
The following example is a basic bolt hole rectangle with the lead-in and lead-out for
the rectangle as part of the top and side line segments. The numbers indicate the
order of the pierces and the “+” sign indicates a counter-clockwise rotation for the
circles.
5
++
12
++
34
If the lead-in and lead-out are created as additional line segments added to the top and
side line segments, additional text is required to indicate which direction the next line
segment should take as part of the part program, as shown in the following diagram:
5
R
++
12
++
34
11-2
Importing Prepared DXF Files
In this example, the letter “R” has been snapped to the intersection of the four line
segments to indicate that the next line segment after lead-in (pierce 5) would be the
segment which is located at 350 to 10 degrees and then to the other connected
segments on the square. After the left side (vertical) segment has been cut, no
additional text is required to indicate which line should be cut. The Lead-out segment
is the only segment left to cut because the lead-in and the first segment have already
been cut.
Notes:
• There should be nothing on the cut layer except lines, arcs, circles and text or
directional commands.
• Line segments must be connected to complete the cut path.
• If multiple line segments or arcs need to be repeated, each line segment should be
drawn, rather than copied and pasted.
• Features for marking are not available.
• No traverse lines are required. All lines in the CAD drawing are assumed to be cut
lines.
• Left kerf is assumed.
11-3
Programmer’s Reference
11-4
PrintedintheUSA
806270‐000
Loading...
+ hidden pages
You need points to download manuals.
1 point = 1 manual.
You can buy points or you can get point for every manual you upload.