Fusion post processor

Thursday, 06 February 2020



XoomSpeed Post processor for Fusion 360

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

  1. 512 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 Tormach's 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).

Download the latest version of the Fusion 360 post processor for Tormach PathPilot.

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.

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.



This site was last updated 02/06/20