Note
CNC-Step have also their own post-processor. It did not exist at the time when this post was coded. It can be found in the post library for Autodesk Fusion (https://cam.autodesk.com/hsmposts). You need to search for "kinetic" since the post is not shown when scrolling down (there are too many listed). After seraching for "kinetic" the most recent version of the official CNC-Step post can be downloaded.
A modified Autodesk Fusion 360 post-processor for the HIGH-Z S-720/T milling machine running the KINETIC-NC software, which both are from CNC-Step. Autodesk Fusion post-processors are written in JavaScript and the documentation of the existing classes, functions, etc. is described in the Autodesk CAM Post Processor Documentation.
The post processor is based on the classical format RS-274D better known as G-code. The original version of this RS-274D implementation for the FUSION 360 post-processor comes from Benezan Electronics. You can download their post-processor here. For convenience I saved a copy in this repository.
The reason why the Benezan post-processor works for the KINETIC-NC software is that the KINETIC-NC software is based on the BEAMICON2 software of Benezan.
Thus, above postprocessor ran successfully in FUSION 360 and produced proper G-code for the KINETIC-NC software. This in turn controls the HIGH-Z S-720/T machine.
I made some modifications to the post-processor in order to make it more convenient for my typical operations. Be aware that the modifications are tested only the KINETIC-NC software. KINETIC-NC supports an additional set of specific commands which are not part of the RS-274D standard. There is also a macro language featurem, which can be used to automate recurring tasks.
Adding some commands to the post-processor is quite easy (after the obligatory learning curve). Only two - already existing - functions are employed. The main function needed is writeln() which comes with the Autodesk JavaScript API. The second one is writeComment() which is a wrapper around writeln() that just adds brackets before and after the text (this is the comment format understood by KINETIC-NC).
- Initial section
- Auto-read x-position of actual G54
- Request user to confirm or enter alternative offset
- Safe tool position
- Before and after tool change
- At program end
- Implemented via subroutine calls
- Jump labels between sections (e.g., 2D adaptive clearing, pockets, etc.)
- Allows to execute individual sections separately
- Repeat / Next within each section
- Allows easily to redo sections multiple times
- Remove entries not understood by KINETIC-NC
- Remove % from last line
Adding a section to FUSION_360_KINETIC-NC_HIGH-Z_720T.cps which will always be written to the *.nc file when using this post-processor:
writeln("");
writeComment("Initial section");
writeln("G54 (needed here so that offsets are being read)");
writeln("#100=#900 (use x-offset of G54 for G53)");
writeln("#101=0 (safe y for G53)");
writeln("#102=0 (safe z for G53)");
writeln('PRINT "x-offset = ";#100;"mm"');
writeln('ASKBOOL "Continue with x-offset" I=2');
writeln('IF #0=0 THEN');
writeln(' ASKFLT "Enter x-offset" I=0.0 J=720.0');
writeln(' #100=#0');
writeln(' PRINT "x-offset = ";#100;"mm"');
writeln('ENDIF');
writeln("");writeln("");Adds an empty line because the string "" is empty.
writeComment("Initial section");Write a comment line into the *.nc file. The result in the file will look like this (the round brackets are added be the function writeComment to the text) and KINETIC-NC interprets this as a comment:
(Initial section)Below lines add variables #100, #101, #102 to the *.nc file:
writeln("G54 (needed here so that offsets are being read)");
writeln("#100=#900 (use x-offset of G54 for G53)");
writeln("#101=0 (safe y for G53)");
writeln("#102=0 (safe z for G53)");The values stored in these variables can be used later in the *.nc file, e.g. for traversing like so:
G53 G0 Z=#102 Y=#101 X=#100In the past I added those lines always manually at the beginning of the *.nc file in order to move safely to the workpiece without crashing into any clamps. For my typical setups I then just needed to adapt the initial x-coordinate in the initial section.
In order to overcome this, it is now completely automated based on the settings of G54. This is the workpiece (stock) offset in most of my setups. KINETIC-NC stores the coordinates of the offsets in non-volatile variables (they are saved across sessions even when the machine is off). The offsets for x, y, and z are stored in the variables #900, #901, #902 respectively.
I normally use only the x-coordinate of the offset (#900) because this fits for 90% of my setups. So in the initial section #900 is assigned to #100 which is used in the subroutine (see below) to do the safe movement to/from the workpiece. I could have used #900 directly in the subroutine, but this way I have more flexibility, for example in cases where I do not want to use the G54 offsets.
When the G-code requests to change the tool, the spindle needs to drive back to machine zero, the new tool (inserted manually) needs to be measured and later the spindle should go back to the workpiece.
This line from the original post-processor:
writeBlock("T" + toolFormat.format(tool.number), mFormat.format(6));writes the following into the *.nc file:
N1000 T8 M6Which means command number 1000 (for example), tool number 8 (for example) and M6 is tool change. So I know when the post-processor writes this line a tool-change will happen. Thus I surrounded it (shown below) by two lines which trigger a subroutine that performs the safe traversal to/from machine zero.
So I added a safe path (by calling a subroutine) which moves the spindle automatically according to these variables before and after each tool change:
writeComment('Go to safe position before tool change');
writeln('M98 P1234 (call subroutine 1234)');
onCommand(COMMAND_COOLANT_OFF);
writeBlock("T" + toolFormat.format(tool.number), mFormat.format(6));
writeComment('Go to safe position after tool change');
writeln('M98 P1234 (call subroutine 1234)');In the G-code this renders to:
(Go to safe position before tool change)
M98 P1234 (call subroutine 1234)
N25 M9
N30 T18 M6
(Go to safe position after tool change)
M98 P1234 (call subroutine 1234)As can be seen also the coolant off (M9) needed to be wrapped. Found this by testing.
Note
A tool change requires the tool to be measured again. For this I added the G79 command to the M66 macro, which resides in the following folder on the PC:
C:\ProgramData\KinetiC-NC\macros
In KINETIC-NC the M66 macro is called when there is an M6 command (tool change) in the G-code and the machine has no automatic tool change capability. So in order for this version of the post-processor to work smoothly you need to update your M66.txt accordingly.
KINETIC-NC allows following subroutine syntax:
- M98 → call subroutine
- P1234 → label of the subroutine (caller syntax)
- O1234: → label of the subroutine (subroutine function starts here)
- M99 → exit subroutine
The calls for adding the subroutine G-code within the post-processor look like this:
writeComment("Subroutine 1234");
writeln("O1234:");
writeln("G53 (machine coordinates)");
writeln("G0 (go fast)");
writeln("Z=#102 (safety height)");
writeln("Y=#101");
writeln("X=#100");
writeln("G54 (workpiece coordinates)");
writeln("M99 (End Subroutine 1234)");Which would render in the *.nc file as:
(Subroutine 1234)
O1234:
G53 (machine coordinates)
G0 (go fast)
Z=#102 (safety height)
Y=#101
X=#100
G54 (workpiece coordinates)
M99 (End Subroutine 1234)The subroutine uses the variables defined at the beginning of the *.nc file. So I just need to update these variables once. Then for all subsequent tool changes there should be a safe path "to and from". When I use the same code but have a new workpiece clamped at another position, I again just update the G54 offset(s).
The subroutine call can also point to an external file (not used in this post processor):
CALL "[email protected]"
In the same way, more functionality can be added to the post-processor or different dialects of the same post-processor could be created depending on the requirements.
KINETIC-NC allows skipping portions of the code by using the SKIP command. This comes in handy when in a longer NC program a certain section should be done later again, but some other operations not. In order to support this upfront, the respective code is added by the post-processor as comments, so that it just has to be uncommented when being used.
Note
A label cannot exist on its own unless it has been defined in by the SKIP command before.
Note
Labels need to use other characters than those used in G-code
Following lines show an example of how this is prepared in the G-code by the post-processor:
(Uncomment to skip until specified label)
(Skip label must exist, than jump label is accepted)
(SKIP Q0001)
...
...
....
(Q0001:)If needed the code can be activated by editing the code like:
SKIP Q0001
...
...
....
Q0001:The code between the SKIP command and the label is not executed. The SKIP command is typically used with IF..THEN constructs.
Note
The colon is needed only at the label itself. In the line where the SKIP command is, it is not allowed.
KINETIC-NC allows loops over portions of the G-code. In order to facilitate this feature, the REPEAT and NEXT keywords are automatically inserted close to the top and at the end of each section.
The following code snippet from the thread example file shows this:
(Chamfer)
M98 P1234 (call subroutine 1234)
N1605 M9
N1610 T13 M6
M98 P1234 (call subroutine 1234)
N1615 S5000 M3
N1620 G54
(Edit repeat count according to needs)
REPEAT=1
N1625 M9
N1635 G0 X27.95 Y12.5
N1640 G0 G43 Z15 H13
N1645 G0 Z5
N1650 G1 Z-2.5 F333.3
N1655 G1 X28.75 F1000
N1660 G3 X21.25 I-3.75 J0
N1665 G3 X28.75 I3.75 J0
N1670 G3 X27.6126 Y15.1901 I-3.75 J0
N1675 G1 X27.0553 Y14.6162
N1680 G0 Z5
N1685 G0 X40.6 Y12.5
N1690 G1 Z-2.5 F333.3
N1695 G1 X41.4 F1000
N1700 G3 X38.6 I-1.4 J0
N1705 G3 X41.4 I1.4 J0
N1710 G3 X39.2421 Y13.6771 I-1.4 J0
N1715 G1 X39.6752 Y13.0045
N1720 G0 Z15
NEXTJust change the number after the REPEAT keyword from 1 to a bigger number and the section should be executed the respective number of times.
Tip
In order to debug the post-processor code in FUSION 360, tick the "Open Nc-file in editor" option in the post-processor before saving. When the code change fails, the corresponding error message(s) are shown in the editor. Another indication that something went wrong, is an empty properties window at the lower right of the post-processor dialog.