Fusion 360 Mill Post Processor for Acorn with additional Features (New Version 5)

[swissi]

The official Fusion 360 Post Processor “Generic milling post for CENTROID” which is available in the Autodesk HSM Post Library has fallen behind in support of new Fusion 360 Features.

This version of the Post Processor includes enhanced support for Rotary Axis and Fusion 360 Probing that have been ported over from the more advanced Fanuc Post Processor. Most importantly, Centroid CNC12 specific enhancements have been added, significantly improving the integration between Fusion 360 and Centroid CNC12.

Check out the Enhanced Fusion 360 Milling Post Processor for Centroid CNC12 User Guide for all details.

If you are using Fusion 360 for your CAM you MUST have a look at this User Guide and I promise you will be glad you did as it will give you many ideas to improve your workflow between Fusion 360 and Centroid CNC12.


***Update: Version 5 of this Post Processor has been posted***
1/26/2021 MinRev-40783-swissi-005


***Change Log v5

• The check for redundant Tool # (same Tool# with different tool geometry) is now a Post Processor Property that can be turned on and off. The default setting is to check for redundant Tool#

• The maximum number of tools can now be adjusted in the Post Processor Properties. The default is set to 200 tools matching the CNC12 tool library

• The activation/deactivation of the coolant command (M7/M8 and M9) has been optimized and is now placed at the point when the Z axis is at the clearance height

• When using the Post Processor Property “Check/Update CNC12 Tool Library” it was possible that a message was displayed that the tool diameter in the Fusion 360 tool library is different from the CNC12 tool library but they were displayed exactly the same on the screen. This issue was caused by CNC12 internal rounding errors. The new diameter comparison method is now using a comparison tolerance factor that solved this issue

• Program Numbers that are reserved for CNC12 (9100 - 9999) are creating issues when being used in the Post Processor. This Post Processor will now create a post error with a log message that these program numbers can’t be used

***Change Log v4

• Just a bug fix where the WCS# always defaulted to G54, ignoring other WCS#'s in the setups. Update to this latest version if you are using other WCS#'s than the default G54.

***Change Log v3
New features added (click the links for Implementation Details):

• Improved Logic for Rotary Axis Support (less unwinding between Tool Paths)

• Property to Reset the Rotary Axis at the End of a Job without the need to unwind

• Property to Check/Update Tool Diameter Offsets in the CNC12 Tool Offset Library A Message like this is being displayed when a difference in Tool Diameter between the Fusion 360 and CNC12 Tool library is found:

  

  ToolCompare.PNG (11.2 KiB) Viewed 14053 times

• Support for Fusion 360 Probing (WCS and Geometry). Be aware that the Post Processor alone is not enough to enable Fusion 360 Probing. The Post Processor is just calling probing sub-programs that did not exist for CNC12 and I had to write them with big efforts. If you are interested in the Fusion 360 Probing Cycles for Centroid CNC12, contact me via PM or send email to swissi2000@gmail.com

***End of Change Log

Added Properties that are not available in the standard Fusion 360 Milling Processor for Centroid. Click the Links for Implementation Details on each Property:

• Safe Retracts: Lets you select your preferred Z retract position during job execution. Default is G28. The Z retract position at the end of the job can be selected separately

• Smoothing Profiles: Lets you select a specific Smoothing Profile for your job. G-Code Smoothing is an algorithm that pre-processes G code and smooths out the G-code geometry ahead of time before handing off the moves to the Control Board. 3D Surfacing and V Carve programs benefit greatly from this feature

• Add Command to Begin/End of Job: This allows to add one M Command (CNC12 accepts only one M Command per block/line) or multiple G Commands. If the command does not start with a G or M, the entered text in this Property will be added as a Comment

• 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 Tool Offset: Allows to pause program execution after each tool offset command to let you verify if the correct tool offset has been applied. There are two options available, a M0 stop or a M200 message

• Enable Clamp (M10/M11): Enables the Clamp commands M10/M11 of a rotary table

• Comment Line Formatting: Allows to select the preferred option to insert comments into the job file

• Dwell after Spindle Start: Spindles with a high RPM require some time to reach full speed and need a delay between the spindle start command and the first cutting contact. This property allows to add a Dwell command after each spindle start to give the spindle time to get to full speed before the job continues

• Enforce Numeric Program Name: The default CENTROID Post Processor requires the Program Name to be numeric but CNC12 does allow alpha-numeric names. This property allows to turn off the enforcement of numeric program names to support more descriptive alpha numeric names

• XY-Position at End of Job: Allows to modify the X and Y-Axis return position at the end of a job

• Z-Position at End of Job: Allows to modify the Z-Axis return position at the end of a job

• Rotary Table Axis: Enables a rotary axis in the Post Processor. The default Property setting is No rotary. Do not enable this Property if no A, B or C axis has been configured in CNC12

• Write CNC12 Info Variables: If this Property is enabled, the Post Processor will fill CNC12 User-String-Variables with Information from Fusion 360. The M6 Tool Change file mfunc6.mac that comes with the download of the Post Processor shows an example how the Information in the User-String variables can be used in CNC12. Here's an Example how a M6 Tool Change will look like:
  

  

In addition to these Properties, Logic has been added to the Post Processor for the following Features:

• Inverse Time Feed Rate for Rotational Axis: Regular feed rates in units per minute work well on moves with linear axes but when a rotational axis comes into play, the control would need to be able to track the exact position of the tool tip in 3D space and adjust rotational and linear feeds accordingly to keep the exact demanded feed rate. As only high-end machine controls have this capability, a good compromise is is to use Inverse Time Feed Rates instead.
  
  With Inverse Time Feed Rates the post processor is calculating the length of each move in 3D space and then calculates the time it would take to move this distance with the requested feed rate in units/minute

• Check for conflicting Tool Numbers (same Number but different Tools): Logic has been added that checks for conflicting Tool Information e.g. using the same Tool Number but with different geometry.

• Fusion 360 Manual NC Commands: Supports the insertion of Manual NC commands in Fusion 360 anywhere between Tool Paths. Check the User Guide which NC commands are supported

Here’s the link to the Fusion 360 Milling post processor for Acorn and a sample version of the mfunc6.mac file needed to display the Fusion 360 Tool Information. No Warranties given, use at your own risk


Latest Version MinRev-40783-swissi-005 as of 1/26/2021:

Centroid_Mill_MinRev-40783-swissi-005.zip

(24.36 KiB) Downloaded 573 times

Please report issues, questions and suggestions for additional features in this thread.


-swissi

[Fredsan]

Hi Swissi,

Thanks for the additional features, very handy.

There is still one minor thing I do not like about the Centroid post processor: the program name of the gcode file must be a number, while Centroid can handle 'normal filenames'. It would be very nice, if I can type alphanumerical characters.

Regards,
Fred.

[swissi]

***Update: See first post for latest version***

This version does not require a numeric Program Name:

(remove the .txt file extension)
***File removed***


-swissi

[Sportbikeryder]

Looks good Swissi, good to see some others venturing out into the post processor editing world and sharing.

One thing to add might be a "program end position" or similar instead of the G28. I had one I added in, but for some reason it is no longer in the posts I have been using (I may have deleted it when starting with a new post when I was trying to get the oddball 5 axis TRT-32 tilt table post working). I just ensured the machine had a G90 at the end and then input a G1 with desired X and Y values after I retracted in Z. Can be handy to "present the table say at the middle of the X travel and at the front of Y in order to access the machine table more easily.

John

[n2xd]

How would one go about modifying this post to a BoBcad-cam Post for centroid? Thanks.

John

[swissi]

n2xd,
sorry I can't help you with post processors for BoBcad.

Sportbikeryder, Fred,
I have modified the functionality to position the X/Y/Z axis at the end of a job. I also made it a property to select if you want to force the Program Name to be numeric or if you want to allow non-numeric names. This version now supports the following features:

• 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.

Here's the link to the new version (remove the .txt ending). Feedback is welcome:

***File removed. See first post for the latest version***

-swissi

[Fredsan]

Hi Swissi,

It looks like you can read my mind, I was just about to ask for a G30 P4 at the end of a job

Thanks for the latest version.

Kind regards,
Fred.

[cbb1962]

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...
.

[Sportbikeryder]

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

You can check out this thread for 4th axis.

You will likely be best suited to do a bit of research into modifying the posts yourself. It really isn't that difficult and many can just be cut and pasted from portions of others once you can identify the areas you wish to include or tweak.

viewtopic.php?f=60&t=2981&p=22108#p22108

John

[swissi]

cbb1962,

I have updated the first post with a version that supports A, B and C as the 4th Axis.
Check the feature list in the first post for more details.

-swissi