High feed toolpaths & high feed inserts

[SlaveCam]

As mastercam doesn't support high feed insert geometries (such as H600 wxcu we commonly use) the toolpaths always tend to leave a "bump" on the roughing surface that overloads the cutter on the next depth cut. The only solution is to reduce XY stepover but that results in longer machining time. Is there any better workaround?

[jlw™]

I use the same insert in medium and fast feed. Run the medium feed 3.6in step over, 0.1in deep, fast feed I run 3.6in step over and 0.04in deep. I have all of mine defined as custom tools and then run thru verify to see what's left. I always set "gap" so that it will retract at every backfeed. I never have problems... care to share a file?

[SlaveCam]

Thanks, I don't have a file ready yet.. does Mastercam take the custom tool geometry into account when computing the toolpaths or just the nominal tool diameter? I remember having tried using a custom tool over a year ago but the toolpaths were the same iirc.

[jlw™]

Nominal and it cuts like a square corner. Depending on the shape (everything other than vertical walls or horizontal floors) I tell it to leave 0 stock. that gets it closer.

[SlaveCam]

Well re-defining the tool with a corner R big enough (so that R = (tool max diameter - minimum cutting diameter)/2) did the trick! So looks like it does not cut like a sharp corner...

[zero_divide]

+1 on setting it up as a bullnose endmill.

Also because the last wall pass in the issue you can set up a finishing pass at lower feedrate.