Mastercam Post Processor

Hi all, I have access to Mastercam at work. Is there a specific post that I can use for my Onefinity machine? Would the mill default post work?

Thanks!

1 Like

HI Steve - the default should work - you need to see if it produces any gcode command the buildbotics controller doesn’t understand though.
https://camotics.org/gcode.html

-Tom

1 Like

Thanks Tom, I’m still waiting for the rolling folding legs to come in, but once I get everything in and built, I’ll come back with updates. Thanks again!

1 Like

Any update on this?

Have you been able to try it yet?

Sorry , I haven’t had a chance to try this yet. I haven’t had a chance to finish assembling the machine due to space constraints.

Hey, if anyone is interested I have successfully ran a few toolpaths using mastercam. I used the generic haas 3axis mill and post. I ran a pocket, contour, dynamic mill, and a surface toolpath. All looked good, except the surface toolpath. I think I programmed the feed to fast on the surface toolpath and the controller just couldnt keep up. There is a video of it running on my instagram, if anyone’s interested.

Thanks

4 Likes

I also got the generic 3-axis haas machine definition to work, however the post always included the tool-change, tool probe, and tool length compensation canned cycles in them. Those will cause prompts on the Onefinity controller and will result in an offset for zero when the program runs on the router.
Those first few lines of the gcode had to be manually removed. But I got tired of having to do that so I edited the postprocessor file (.pst) script to remove those outputs and everything works now.

1 Like

As a follow-up to the previous post I did have to modify the machine definition in order to get drill operations to post correctly. The Buildbotics controller DOES NOT support canned drilling cycles, so you will have to disable all of the Canned cycle options in your machined definition/configuration in order for the posted Gcode to be in long hand mode for drilling cycles. It was pretty amusing to watch the controller not know what to do with the posted gcode prior to making those setting changes. When running the canned drill cycle gcode the machine would either drill the first point, then rapid move to all of the rest of the points in sequence without running any Z-Axis travel (no drilling), or it would drill the first point over and over again however many times there were points then “finish” the program.
Workarounds for this prior to just editing the machine definition included having to make a separate drill operation for every point, or having to do a lot of copying and pasting of certain portions of the gcode to append G0 commands after every G80.

Be aware that once the settings of the machine definition are changed/saved to remove canned cycles you will usually need to close Mastercam and open it again for the all of the changes to be applied to any existing programs.

1 Like

Hello captainslug, I am new to this form, I have a Onefinity woodworker on order to be deliver in August. I also Own my license key of Mastercam X5. I have a very good relationship with my local Mastercam dealer (Shopware Inc) and they are willing to help me with a post. I just need to know what’s needed and what needs to be removed. I see the earlier post from cybereefguru with the link to the buildbotics gcode commands to get me started. What version of Mastercam you are using? I know my version is very old, but it works for what I use it for.

The portion of the post header that defines tool changing and homing both need to be removed. I just moved overseas and probably won’t have access to my computer for a month or two so I unfortunately cannot provide the postprocessor definition I created that’s compatible. I was making all of my programs in Mastercam X4

I have edited a 3 axis post, Machine definition and Control definition for Mastercam X5. So far it is working well for milling. I have not tried to surfacing or drilling.

1 Like