Fusion 360 Mill Post Processor for Centroid CNC's with additional Features

Moderator: cnckeith

swissi
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Fusion 360 Mill Post Processor for Centroid CNC's with additional Features

Post by swissi »

***Update: The latest version of this Post Processor can now be found on GitHub. Checkout the User Manual for all the features***

***Change Log:
  • 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
***End of Change Log

I made some changes to Franco’s original post processor (https://www.youtube.com/watch?v=yfGVdfHlDNg). Here are some of the features that can be enabled trough the Post Processors Properties when posting in Fusion 360:
  • 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:
Return.JPG
  • 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:

Code: Select all

: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:
ToolChange.JPG

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 :D

Latest Version MinRev-40783-swissi-001 as of 5/27/2019 is now available on GitHub

Also checkout the User Manual for information on how to use the features.

-swissi
Last edited by swissi on Mon May 27, 2019 4:35 pm, edited 5 times in total.
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Fredsan
Posts: 72
Joined: Wed Sep 27, 2017 3:07 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: The Netherlands

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by 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
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by 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
Last edited by swissi on Fri Apr 05, 2019 3:32 pm, edited 1 time in total.
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Sportbikeryder
Posts: 177
Joined: Thu Jan 26, 2017 11:45 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 10583
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: Yes
Location: North Carolina

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by 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
Posts: 31
Joined: Sat May 26, 2018 8:01 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 0943
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: Franklin,NC

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by n2xd »

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

John
swissi
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by 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:
Return.JPG
  • 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
Last edited by swissi on Fri Apr 05, 2019 3:33 pm, edited 1 time in total.
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Fredsan
Posts: 72
Joined: Wed Sep 27, 2017 3:07 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: The Netherlands

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by 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
Posts: 349
Joined: Wed Jan 03, 2018 10:04 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D2695C8301-0122180576
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: NW Arkansas

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by 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...
.
axis definitions.JPG
Clint in NW Arkansas

The more I learn, the more I realize I don't know...
Sportbikeryder
Posts: 177
Joined: Thu Jan 26, 2017 11:45 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 10583
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: Yes
Location: North Carolina

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by Sportbikeryder »

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
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
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: Fusion 360 Mill Post Processor for Acorn with additional Features

Post by 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
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Post Reply