Fusion post processor

Wednesday, 06 March 2024

Feb '23 update


XoomSpeed Post processor for Fusion 360

Make a donation

Latest update 6th Mar 2024 - download the latest version of the Fusion 360 post processor for Tormach PathPilot.  If your browser opens the file and display it on your screen instead of downloading, right click the link and select 'Save target As...' (MS Edge) instead.  This isn't a bug as such, it's just that your browser recognises the file type and thinks it knows what to do with it.

6th March 2024

Adds the ability to specify a cooling mode to be used in conjunction with an ETS.  If you happen to have a multi mode coolant system and arrange for air coolant to point at your ETS, then this can be a good way to clean chips from the ETS before attempting to measure a tool.

Also fixes a couple of bugs associated with optional CAM operations and the block delete function in PathPilot.  Under some circumstances, in the previous release, turning on the block delete function could result in the coolant mode not being set properly for the operation following the optional one.  Also, if the last operation in a program was marked as optional, then   turning on block delete resulted in the program shutdown sequence also being marked as optional.  Hence things like stopping the spindle, turning off the collant and retracting to the finished location wouldn't happen if block delete was turned on.

27th March 2023

No sooner did I release the February version - the first for 2 years - than someone found a bug that's been there since the beginning of time.  Feed rates have always been output with 1 digit after the point when working in inches and 0 digits after the point when working in mm.  That works fine for everything, except rigid tapping very fine threads where it can result in threads being damaged.  This has now been corrected.

There were also a couple of issues with the newly added ability to add block delete characters,  Again these have been corrected.

21st Feb 2023

A major update.  Major enough to give it its own page, but the highlights are.  To see the in depth description of each new option visit the dedicated page for this release.

  1. Option to add a delay after flood cooling on to allow pump to get up to speed
  2. Added support for Fusion's 'tapping with chip breaking' cycle.
  3. x, y and z coordinates of nominal probe point can be added to the description output of inspection probing results.  Useful when using a CAM pattern to probe multiple values along a given feature.
  4. g-code output can be arranged into separate subroutines for each CAM op. The subroutines are stored at the end of the output file, so the top of the file consists of a sequence of subroutine calls.  This makes it easier to set a restart location if a program has to be stopped and restarted.
  5. Fusion's WCS probing cycles now have more probing speeds than they used to.  There's now an option to replace speeds previously entered as post-processor options with the values specified in the CAM operation if you wish.
  6. CAM operations marked as optional are output with the leading '/' character on each line to enable the block delete function.
  7. The 'optional' property of some Manual NC CAM operations are not visible to the post-processor.  To get round this and enable block delete on ETS tool setting commands, there's now a post-processor option to output all tool measure and tool check options as optional.
  8. A major revamp to the way coolant modes are handled.  There's a new post processor setting to allow you to specify the type of coolant setup you have and, depending on your selection, Additional coolant modes specified in the CAM operations can be handled. (air, mist, flood and mist + flood).
  9. Corrects the handling of a situation where consecutive operations use the same tool number but with different tool length offsets,  In the past, the 2nd op wouldn't generate the required tool change code.

22nd September 2021

  1. The retract options for 'Retract on WCS change' and 'Retract on work plane change' (3+1 machining) were turning off the spindle and coolant and then turning them on again after the move.  this was unintended and is now removed.  This will speed up the code slightly.
  2. An update to Fusion 360 revealed that there was a mistake in the post-processor code.  The new version of Fusion raised a warning when posting code, indicating there was a problem, but the post-processor worked correctly anyway.  The post-processor is now modified to prevent the warning being raised.  The generated code should be unchanged.

10th May 2021

  1. The way in which custom post-processor properties are defined has been updated to match the latest posts from Autodesk.  When viewed in the 'NC program' setup, the properties are now arranged in groups with group titles.  Makes it a little easier to navigate.
  2. If you have a 'Manual NC - comment' immediately before a 'Manual NC - Stop' operation, the comment will be output on the same line as the M0 (or M1 for optional stop).  This will cause the comment to be displayed as a banner across the bottom of the screen.  If the comment happens to be the name of an image file, or video, then the contents will be displayed where the toolpath preview normally is.
  3. Added support for left hand tapping - sadly this doesn't work in the current release of PathPilot.  It's beign worked on!
  4. Added a 'Retract on optional stop' to match the 'Retract on Manual NC stop' option that's been there for a while.
  5. For people with ATCs, there a new pair of properties to allow you to ask for an extra tool change at the end of a program.  Re-loading the first tool in a program can save a little time if you're running the same program for multiple parts one after the other.

18th Feb 2021

Added support for Manual NC commands to turn inspection probing on and off.  When inspection probing is on, WCS probing routines do not in fact update the WCS.  Instead they write the results of the probing operations to a text file named 'inspection.txt' in the user's file area.

This feature is turned on and off by adding a 'Manual NC' operation with an operation type of Action.  Set the action text to Inspection on to enter inspection mode, set the action text to Inspection off to switch back to regular probing mode.

For examples of how to do inspection reports, watch the following.



Added support for partial circle probing operations (boss and bore). (Path Pilot 2.7 and later)
Added support for position and size tolerance checking in all WCS probing functions. (Path Pilot 2.7 and later)
Added Manual NC and tool library support for tool setting/checking.
Replaced 'Use G30' and 'Use G28' post-processor properties with much more flexible properties to control retraction.

Full details of the updates are discussed in this video.


The XooomSpeed post processor provides a number of functions not supported by the standard post processor from Autodesk.

  1. 500 WCS support
  2. Some bug fixes for Smartcool support in drilling operations
  3. Integrated WCS probing operations
  4. In process use of electronic tool setter to set tool lengths and/or check tool lengths for tool breakage
  5. Spindle reversing on PCNC440 (requires a USB I/O module).
  6. Expanded g-code tapping cycles (Required to use a tension/compression tapping head on a PCNC440 with non-standard spindle reversing).
  7. Support for I/O modules in generated g-code. (added 26/06/20)

Some of the above require new custom properties to be added to the Fusion 360 Post process dialog.  These are described below.

Integrated Probing

Supports all the Fusion 360 WCS probing routines (except axis rotation).  You can use this with either wired or wireless probes to perform a number of flexible probing routines to simplify your setup procedures.  Watch the following video for a tutorial on how these work.


Fast probing speed (inch/min) The feed rate used for the first part of the probing operation.  This is always specified in inch/minute, nomatter what units are used for the g-code output.  Suitable values depend on the acceleration/deceleration performance of your machine, but the default is 20 inch/min
Slow probing speed (inch/min) The feed rate used for the final probe.  This will generally be somewhat slower than the fast probe speed to ensure good accuracy of the final result.  Defaults to 1 in/min
Slow probe distance (inch) After the first, fast probe, the probe will retract this distance away from the detected surface before starting the slow probe.  Default vale is 0.040"

In process tool setter support

The in process ETS support allows tools to be measured using and electronic tool setter during a program run.  Tools can either have their lengths checked against the current settings in the controller's tool table, or the tool table can be updated with the newly measured values.

These operations can be performed at the start of a propgram, when each tool is loaded or unloaded or even after every machining operation.


The ETS functions use Tormach's G37 and G37.1 extensions to the standard LinuxCNC g-codes.  Before you use these options, please make sure you have read the G37 and G37.1 documentation from Tormach and make sure you have the G37 locations correctly set up and the ETS referenced.

ETS diameter limit (inch) The maximum diameter tool that can be measured using the ETS.  Generally this is the diameter of the pad on the top of the ETS.  No action will be taken for tools larger than this except in the case of 'drills' and 'spot drills' which can always be checked irrespective of their diameter.  Likewise, probes are never measured by the ETS routines.
Tolerance for ETS checks (inch) For 'check' operations, this is the allowed error between the measured tool length and the tool length in the PathPilot tool table.  It is the value of the 'P' word supplied to G37
ETS op before start What action to take before the start of the first machining operation.  The action will be applied to all the tools used in the program, so long as they are not a probe and they have a tool diameter (in the Fusion library) that is acceptable according to the  ETS diameter limit above.  Options are 'none, 'check' or 'set'
ETS op before a tool is used At each tool change, this operation is performed immediately after a tool is loaded and before the operation begins.
ETS op after a tool is used At each tool change -- except the first - this operation is performed on the tool being unloaded.  This will generally be 'check' in order to detect a tool that's been damaged and abort the program so as to avoid damaging subsequent tools.
ETS op after every machining operation Check/set tool length after every machining operation.  Useful with multiple WCS or CAM pattern setups.  Using the 'Check' option here means that the tool length is checked after each machining operation.  It it's out of spec (Tolerance for ETS checks) then execution stops.  In the case of multiple parts in multiple WCSs the tool length will be checked after each operation on each part and execution will stop the first time the tool is detected to be out of tolerance.

I/O module support

The I/O support options make it possible to signal to one of our USB I/O modules that various useful actions are taking place in your program.  the pre-configure applets supplied with each I/O module can make use of these features to trigger various custom sequences.  User written applets also have full access to this information

I/O ETS in use Signals to the I/O module that one of the ETS functions above is about to take place.  This gives the opportunity for the I/O module to open a cover over the ETS and/or operate an air blast to clean the ETS.
I/O ETS ready Select an input that PathPilot will wait for before starting the ETS function.  The idea here is that the I/O module can request a delay to finish opening a cover and cleaning with an air blast before allowing Pathpilot to continue with the ETS function.
I/O flood cooling Turn this output on any time that flood cooling (M8) is running.  typically this would enable monitoring of a flow switch to verify correct operation of the coolant.
I/O mist cooling Similar to I/O flood cooling above, but this output is active with mist cooling (M7).
I/O Program running The selected output will turn on at the start if your program and turns off again at the end.
I/O Spindle running Indicates that the spindle is turned on (forward or reverse)
I/O tool change in progress Turn this output on when a tool change starts and back off again once the tool change is complete.

Tapping for PCNC440

Tapping operations are normally inpossible for a PCNC440 because spindle reversing is not provided on that machine.

Spindle reversing Normally set to 'M4', use the other options to get spindle reversing working on a 440.  If your 440 has a USB I/O module with one of the outputs connected to the F/R and COM pins on the BLDC drive, then you can have spindle reversing by outputting one of the other options depending on which USB I/O channel you've connected.

Options are
M4, M3 M64 P0, M3 M64 P1, M3 M64 P2, M3 M64 P3

Use M3 M64 P0 if you have used channel 0 of the USB I/O module to control the spindle direction and son on for the other I/O channels.

Expand tapping This will work on all the mills, but is essential on the 440 with non-standard spindle reversing.  Instead of outputting tapping ops as a canned cycle, this outputs long hand g-code to do the job.  When tapping is done in this way, the spindle direction is controlled using the Spindle reversing options above.

Home | Feb '23 update


This site was last updated 03/06/24