topic CNC router postprocesser in HSM Post Processor Forum

CNC router postprocesser

Anonymous — Fri, 23 Jun 2017 13:38:07 GMT

How do I get a post for the Powermatic CNC router or is there a generic post that will work?

Re: CNC router postprocesser

Anonymous — Tue, 28 May 2019 18:44:31 GMT

I would also like to know how to do this!

We have 2 powermatic cnc 2 by 4 routers in our classroom. How cool would it be to have middle school students go from Idea to model to part all with the same program.

the File extension that powermatic reads is a .mmg (if this helps)

Re: CNC router postprocesser

bob.schultz — Sat, 01 Jun 2019 17:18:52 GMT

The PowerMatic CNC uses a RichAuto controller and we do have a generic RichAuto post processor in Beta. You can download it here.

https://cam.autodesk.com/hsmposts?p=richauto

The post outputs the NC file with a '.nc' extension. You can change this to '.mmg' by modifying the following line at the top of the post processor.

extension = "mmg"; // *.cnc/*.nc/*.tap/.u00/*.plt/*.mmg/*.txt

Take note that this post is in Beta mode right now and is generic in nature to the RichAuto controller without regards to the machine type, so the output should be checked carefully before running it on the machine.

Re: CNC router postprocesser

mark — Wed, 05 Jun 2019 21:08:43 GMT

Hi, we at NexGenCAM have several HSM post writers and could assist with creating or modifying a generac post for you to make it perfect and edit free. Would you like to talk about it. Feel free to contact me direct at the below info.

Mark Fischer

262-416-7994

mark@nexgencam.com

Re: CNC router postprocesser

cmault — Mon, 06 Jan 2020 18:44:12 GMT

Was able to get the Powermatic to read the program with the rich auto post processor after changing the extension to the .mmg but it was cutting jerky. (had is cut a simple circular pocket but it was making more of a hexagon shape)

Powermatic has a post processor that I downloaded but I cannot see that with fusion 360.

http://www.powermatic.com/us/en/service-and-support/products/cnc/

I am sure that I am close to getting this to work but am missing something somewhere.

Suggestions are welcome

Thank you in advanced

Casey Ault

Re: CNC router postprocesser

bob.schultz — Mon, 06 Jan 2020 23:01:16 GMT

Hello Casey,

When the machine cuts a hexagon instead of a circle, this usually means that it has problems interpreting the circular (G02/G03) records. The post outputs an incremental IJK center point for circular interpolation, which seems to match the post you referenced, as least by the names (VAR ARC_CENTRE_I_INC_POSITION = [I|A|I|1.3]).

You will need to determine for sure what the circular interpolation format is. I would suggest you hand program a simple circular block using an absolute center point for the IJ values and see if this works and possibly an incremental center where whole numbers are used, in case there is a rounding error in the output that you are generating from Fusion.

If you cannot successfully get the control to process a circular record, then you can always disable circular interpolation in the post by changing the following variable at the top of the post processor.

allowedCircularPlanes = 0; // disable circular