Multiple origins with Mastecam no working - CNC Mill

Mastercam Exporting Issue:

I have set up 4 origins in Mastercam running on a CNC Mill. The 4 origins are defined in the CNC.

When the program is simulated, Mastercam shows everything is fine.

The issue happens when the program is exported as Gcode and imported into the CNC.

While running in the CNC, the 1st origin does fine, afterwards, it moves to a place that is not declared in the CNC or in Mastercam.

If the Mastercam program is exported starting at the 2nd origin, then the machine goes to the 2nd origin and afterwards, cannot accurately find the 3rd origin.

Has anyone experienced this issue?

What type of setup, multiple stations on a table, or is this a rotary application?

You need to have a work offset defined in MCAM that is associated with each plane, and then at the machine that position needs to be set and the position in the work offset register for the appropriate work offset.

Going to need part of a sample program and/or a better description of where the problem is to be able to give you much more advice than that.

I do this all the time, but I occasionally find ways to mess it up

I'll give you an example of the easiest way that I have found that I almost never mess up. Say I have four parts and I want to have a separate offset for each one: G54, G55, G56, G57. I will duplicate the part geometry four times with about the same spacing I am going to have on the mill. This doesn't need to be exact, it is just for visual reference when I am programming.

I then create a WCS for each individual part with the datum at the appropriate spot for each part. On the WCS plane manager I then set the Offset Number in the appropriate column for each WCS. G54 will stay default (0), G55 will be (1), G56 will be (2), and G57 will be (3). In effect it just adds what ever number is in that column to the G54.

I then program each part making sure that the WCS is set for the respective part that I am working on.

Obviously, when I set up the mill, I need to set 4 xyz zeros.

There are a bunch of ways of doing this, but this system seems to work best for me. If I do it this way Verify works for each part, and it always posts correctly.

I used to just use one part in Mastercam, then duplicate the program and change the offset number, but I had a hard time visualizing where I was at. I have also used macros and sub-programs. The system above is the most reliable for my brain.

my brain hurts reading that you translate 4 parts then use a wcs for each location. That's what a transform is for. You can post out g54's and g55's, post out subs , all sorts of stuff in there

Op, are you trying to have multiple parts on table with different Datums/faces or origins, or the same operation repeated at different locations on table using g54, g55, and so on?

Thank you all for replying.

For clarification, the goal is to make 4 identical parts with 4 unique offsets.

Each work offset is defined in software and programmed into the CNC.

Solution:

It turns out, after the toolpath finished at the first origin, the tool would go to clearance height, return to the first origin and then begin the second origin toolpath from there (at feed rate ) ...

The ideal state is for the tool to finish, go to clearance height, rapid to the next origin, and then begin the toolpath.

So the issue is with Mastercam's post processor and how it outputs the Gcode when using multiple origins.

Coding an adjustment to Mastercam's post processor file so Gcode line "G00X0Y0.5" is executed before beginning the next toolpath fixed the problem. - Credit to Mike Johnson.

If anyone has found a simpler solution to this issue, please post!

Huh...first day on the job eh?

It is a problem with your post, I ran into this when I first setup up mastercam on mill then later in lathe. The stock post does not switch origin based on work offset with in planes without flipping a switch in the post. I offer no warranty on this suggestion, as screwing with your post without knowing what your doing will crash the shit out of your machine.

BALNH said:

my brain hurts reading that you translate 4 parts then use a wcs for each location. That's what a transform is for. You can post out g54's and g55's, post out subs , all sorts of stuff in there

Click to expand...

I don't disagree... but I have some OCD issues with how I order tool paths and clearance planes. Doing it the way I suggested gives me a little more control over how things are ordered, and where the machine ends up when it's done etc. Plus all of my verify and back plot works out well. In other words, it makes sense in my brain and I'm happy with it. That isn't to say I don't use translate all the time. I just seem to have more issues when I use it when using multiple offsets, and those issues aren't as apparent when I run verify. But I'll admit when I have 24 parts on a tombstone, I sure as heck use the translate function.

Have you used the transform in MasterCam? A lot of cool stuff in there to make it easier to do what you are trying to do.

We were all new at some point and had to learn, so ask away

The emastercam.com forum has a lot of good info on it and helpful ppl there also, so I would recommend checking that out.

Take your base operations, and try these settings in the screenshot, and see if you like that.

If I am making identical parts, I like to have the machining called by a subprogram. That way if you want to change something, you just change the one sub, not in 4 different places if it is all long coded.