Programming a HMC with Powermill and outputting B-Axis positioning moves

[bmartin]

I am pretty new to PowerMill. In our main shop we use GibbsCam to program our HMC's. I have also used MasterCam and Esprit in prior roles for the same. Right now I am providing programming support to our other shop that uses PowerMill. They do some hand editing due to post issues on each program. Most look pretty straightforwad and I think I can solve. My main struggle with PowerMill is that it does not put out any B-Axis positioning moves for our HMC. We are doing blocks with side-holes and I gotta imagine there is a way for PowerMill to determine a B90 or B-90 is needed based on the planes. Can anyone point me in the needed direction to get that output?

[Sean570]

What is the manufacturer for your HMC?  Obviously the post you use isn't properly configured for the machine. Powermill does have some generic posts that that may or may not work for your machine. But typically you would want to contact your Powermill reseller and ask them for a post or support to fix the one you currently use. 

That said you could edit the post yourself using the Autodesk manufacturing post processor utility, but I would not advise it, unless you know exactly what you are doing and only if it is a minor change. 

[bmartin]

It is a Heckert HMC with a Fanuc control. It is one PowerMill provided for it but I was unsuccessful in making progress with them to get that output the 1st time. I am hoping someone can show how it "should work" and then if that does not work properly for me I can get the post modified. 

[jelrod · Accepted solution]

The output workplane has to be a Z0 orientation. Then your toolpath workplanes will post accordingly.This post posts out theoretical work offsets. If the fixture is correct it’s pretty close. In this case the output workplace has to be oriented correctly and at center of the table for the math to work. I also have another post that just does standard fixture offsets with no G10s. 

 

 

 

[bmartin]

And your post will automatically add the B positioning moves for non "multi-axis" toolpaths?

What I think you are showing is basically what we want to get.

[jelrod]

If the output work plane is oriented correctly then toolpath workplanes post the appropriate B orientation. The example above shows the slot being posted at 270.0 degrees. If the conditions are met and yours is not then your post is wrong. Powermill has no problem doing what you’re asking. 

[bmartin]

I made progress. Our guys that use Powermill have not had experience with HMC's and this type of programming and local support had not been any help. 

With the assurance it could be done, I started experimenting and reading information. I needed to create "Setups" for each face and then it posted out properly. The "workplanes" were created right, so adding the toolpaths to a Setup was easy! 

[jelrod]

I’m glad you’re making progress. I’ve never really used setups. There’s a guy here that likes them but I usually see it as extra work. What matters with this is the relationship of the output workplane in the program setup form to the toolpath workplanes. Those differences index the B axis whether you use setups or not. Or, at least that’s what matters with mine.