Centroid Community CNC Support Forum

• 5/27/2019 MinRev-40783-swissi-001: Version number has changed and includes now the MinimumRevision number the Post Processor is based on with the extension of swissi-001 counting up. This version is now based on the latest Centroid General Mill Post Processor MinimumRevision = 40783. These new features have been added:
  * Add a Command to the Beginning and/or End of job
  * Check Approach has been changes to Check Tool Offset and supports now the option of M0 or a M200 message
  * Comment Formatting can be chosen between (Comment) or :Comment
  * Write #300 Tool Info Line has been changed to Write CNC12 Info Variables and supports now a variety of Fusion360 parameters
  * Rotary Axis support has been improved
  * Support for Manual NC commands Comment, Display, Pass Through and Call Program has been added to the Post Processor
  * Logic has been added that checks for conflicting Tool Information e.g. using the same Tool Number but with different geometry.
  
  Checkout the User Manual for an updated list of all the features and how to use them

• 4/6/2019 Rev-9: Changed the 4th Axis property to support A, B and C Axis. Made property for "End of Job Position" of X, Y and Z Axis more user friendly (no change in functionality). Feature description below has been updated

• Add Debug Information: Adds debug information to the Gcode file that shows which line has been created by which function of the post processor. Great to troubleshoot problems.

• Check Approach: Adds an M00 after a Tool Length Compensation Move that stops your machine to check if any mistakes have been made in tool length compensation. Very valuable if you run a new setup with new tools.

• Z-Position at End of Job: You have now the choice to select any of the configured Z-Axis values in either G28, G30, G30 P3 or G30 P4. There is also an option to select "No Movement" which could be very risky. Only select this option if you know what you are doing. Note that this property only impacts the Z-Axis. The X/Y axis have their own property and can be configured differently from the Z-Axis. For those who don't know, these return values can be configured in CNC12 under Setup[F1]->Part[F1]->WCS Table[F9]->Return[F1]. Here's a screenshot:

• XY-Position at End of Job: This gives you the option to position the X/Y axis to any of the return values configured in G28, G30, G30 P3 or G30 P4.

• Force Program Name to be Numeric: Setting this to false will allow you to use non-numeric Program Names. Note that when you enforce numeric Program Names, you will no longer get an instant error message from Fusion 360 if the Name is non-numeric. It will let you start the post but the post will fail with an error log that will tell you that the Program Name needs to be numeric.

• Dwell after Spindle Start (% Factor of rpm): This will add a G4 command after a spindle start. This factor is a percentage of the spindle speed. If the spindle speed is 6’000rpm and the factor is 100, the dwell will be 6 seconds. A factor of 50 will be 3 seconds. If the factor is set to 0, no G4 command will be added.

• Rotary Table Axis: This property allows to enable the 4th Axis as A, B or C Axis. You can select if your Rotary Axis is along the +X or -X Axis (A-Axis), along the +Y or -Y Axis (B-Axis) or along the +Z or -Z Axis (C-Axis). Do not enable it if you don’t have a Rotary Axis on your machine. The 4tth Axis will be configured with the default settings for a Rotary Axis. If your Rotary Axis has special requirements, check the Autodesk Instructions how to Setup a 4th Axis.

• Enable Clamp On/Off (M10/M11): Enable this if your Rotary Axis is using clamps. The post processor will add the M10/11 commands.

• Write tool list: This will write the Fusion 360 Tool Information of all the tools being used in this job on top of the Gcode file:

:T1  D=4. CR=0. TAPER=90deg - ZMIN=-1. - spot drill - 4mm Spot Drill
:T3  D=8. CR=0. - ZMIN=-12.5 - flat end mill - 8mm Flat Endmill
:T6  D=4. CR=0. - ZMIN=-6. - flat end mill - 4mm Flat Endmill
:T9  D=6. CR=0. TAPER=45deg - ZMIN=-1.3 - chamfer mill
:T12  D=6.5 CR=0. TAPER=118deg - ZMIN=-14.953 - drill - Drill 6.5mm 118 Degree

• Write #300 Tool Info Line: This will add the Tool Information from the Fusion 360 Tool Library; including the Tool description if any is available, in front of every tool change. This information is assigned to the CNC12 user variable #300 and can be used to display this tool info with every M6 tool change. The tool change information that will pop up on screen if a M6 tool change is reached will have the tool info from Fusion 360 on the first line and the corresponding tool information from the CNC12 tool/offset library on the 2nd line. This makes it possible to verify that the Fusion 360 tool info matches the CNC12 tool/offset library configuration. A customized mfunc6.mac file is necessary to get this functionality. A sample mfunc6.mac file is attached in the zip file posted below. The on-screen Tool Change message will look like this:

• Z-Position at End of Job: You have now the choice to select any of the configured Z-Axis values in either G28, G30, G30 P3 or G30 P4. The possible values are 1=G28, 2=G30, 3=G30 P3, 4=G30 P4, 5=No Movement (use at your own risk). All other numbers will default to G28. Note that this property only impacts the Z-Axis. The X/Y axis have their own property and can be configured differently from the Z-Axis. For those who don't know, these return values can be configured in CNC12 under Setup[F1]->Part[F1]->WCS Table[F9]->Return[F1]. Here's a screenshot:

• XY-Position at End of Job: This gives you the option to position the X/Y axis to any of the return values configured in G28, G30, G30 P3 or G30 P4. The possible values are 1 to 4 as with the Z-Axis. Any other number will remove the X/Y positioning at the end of a job and will not move the X/Y axis.

• Force Program Name to be Numeric: Setting this to false will allow you to use non-numeric Program Names. Note that when you enforce numeric Program Names, you will no longer get an instant error message from Fusion 360 if the Name is non-numeric. It will let you start the post but the post will fail with an error log that will tell you that the Program Name needs to be numeric.

cbb1962 wrote: ↑Fri Apr 05, 2019 7:23 pm Great Job Swissi!

Is anything about this post-processor Acorn specific? Maybe this should be the factory post-processor on the Fusion website...

According to this graphic, I will be needing a B axis option in the future...
.
axis definitions.JPG