Tranforming (mirror) toolpaths

[mbonnet]

Is anyone else having problems with the 'transform' feature in the mill toolpath menu? when i choose to create new operations and geometry, i get an error and the toolpath fails. I have our reseller working on this but I need a fix QUICK! On the main tab, I'm setting mirror, create new operations and geometry, then on the Mirror tab, I set x-axis.

[Kannon]

whats your error say?

[Aaron Eberhard]

I'm running across this too.. It's in the new version... Here's what I'm doing to work around it:

 

Note: This only happens if "Copy source Geometry and toolpaths" are checked. Of course, if you don't copy and modify them, then all hell breaks loose with the directions things will cut and travel..

 

The first time you try a mirror command, it will fail, saying something along the lines of "zero operations selected." It will still make the failed toolpath, though, just waiting to be regenerated. if you regenerate, you will cause mastercam to crash. So Delete the toolpath.

 

Next, do the same exact mirror command, set everything the same, copy source geometry and ops, whatever.

 

This time, it will work, it will start creating the mirror toolpath, but will take for bloody ever and a day. That's because it actually created two copies of your geometry. Two surfaces (or solids), two tool control splines (or boundry control splines), etc. Cancel the toolpath generation by hitting ESC key.

 

Now, click once on the geometry (once on surface, one on tool control spline for me), and delete it. It will complain that this is used in a toolpath, but just hit OK.

 

Now regenerate the toolpath, and see what happens, it should work, with all of the normal annoyances of having to reverse the direction from conventional back to climb, the step direction of the cut, etc. At least, we always have to do that with our 5 axis toolpaths.

 

I've already talked about it to Jamie at Tech Support today, so I'm sending him a sample file. Hopefully they can find something quickly, cause it's rather annoying.

 

Cheers!

[sharles]

In version X I was having stupid problems when transform-mirroring toolpaths (like a contour program would start from the bottom and go up). Finally I just decided it was easier to save the whole file to another name and mirror all my geometry. The surface toolpaths only had to be regenerated. The 2d toolpaths simply had to have the chains reversed and make sure the tool was still compensated to the side you want. I don't know if that would work in your case, but it was MUCH more foolproof than the transform commands.

[crazy^millman]

quote:

---

In version X I was having stupid problems when transform-mirroring toolpaths (like a contour program would start from the bottom and go up). Finally I just decided it was easier to save the whole file to another name and mirror all my geometry. The surface toolpaths only had to be regenerated. The 2d toolpaths simply had to have the chains reversed and make sure the tool was still compensated to the side you want. I don't know if that would work in your case, but it was MUCH more foolproof than the transform commands.

---

This to me is the only predictable way in which to do it in Mastercam.

[Colin Gilchrist]

That is also the way we do it.

 

Save the file as a different name. Then create a line on the center of the block of material and Xform-Mirror the geometry about that line.

 

If you mirror about a line you get to keep your work offset origins on the same side of the part. Then you can reverse your chains and regenerate your surface machining.

 

The only time it gets to be a real pain is when you also need to mirror the tool planes.