Since update lathe internal boring has weird paths

[rw_skinner]

Previous jobs that worked fine now do strange tool paths after this last update.

For instance, the part I have attached, should have a finished bore of 0.750, but it keeps boring it to 0.733.  I tried several things but it just doesn't want to finish the bore.  Any ideas?

[a.laasW8M6T · Accepted solution]

There is a problem with your model.

The face you have selected as Z in your setup is 0.008 offset to the central bores

When you have created the hole features they were not snapped to the center of the previous bosses.

It would be much easier to create this part as a revolved sketch, then you wouldn't end up with these issues

[rw_skinner]

Slapping Head....   I typically model in a different program and started with Fusion recently.  I totally missed that.  I dragged the hole to the origin and I thought it snapped in place.  I fixed it and then the finish pass wouldn't do the finish bore.  So I deleted the model and started over.  It still won't bore the hole.

[a.laasW8M6T]

Hi,

it is because you have set the inner radius as the model ID so the tool cannot reach in there with the leadouts.

just giving a small offset allows the toolpath to generate in the smaller bore

[rw_skinner]

Thanks again. I'm just curious why previous models have the same bore and have been working fine and I never remember having to do an offset like that. Even the hint says to normally use the model ID. Not arguing, I'm curious why. Lead outs and in's were turned off and it still failed to bore that. I know sometimes I have to play with the clearance on small bores to get it to work so the bar won't collide with the backside of the bore.

[a.laasW8M6T]

I'm not sure TBH, I don't use Fusion for turning so I don't really spend much time with these toolpaths.

If I give it even a 0.001 offset it generates so maybe a bug?

[rw_skinner]

I'm sure it is.  The lathe turning, especially on ID work seems to get most of the little bugs for some reason.  Thanks for finding that small mod to fix it.

[akash.kamoolkar · Accepted solution]

@rw_skinner the inner radius denotes the lower limit of the material to be machined. if it coincides with the model then it means there is no material there to be machined and therefore a toolpath won't be created in that area. All turning strategies have always worked this way.

Regards,

[rw_skinner]

Thanks. I misread the hints that ModelID is the preferred default for OD operations and I should have been selecting Stock ID most likely or rest machining, or maybe what the previous rough cycle diameter was.