Interesting Issue with Keep Sharp Corner ?

[Anonymous]

I have a panel that I need to cut that has a short inset for a drawer pull and Fusion 360 could not generate a toolpath for this operation.

I played around with it a bit and any step-down over half the diameter of the tool will work. Anything shallower will not. Perhaps it was my mistake but I was unaware of this rule, or maybe this is a glitch in the CAM. I don't see a reason why these inside corners would not work.

I am trying to use .25" tool and the inset is .095"

Any information would be greatly appreciated.

[Steinwerks]

Definitely sounds like a bug. Can you export the file as a .F3D file and attach it so others can have a look? If you're not able to share the part but able to reproduce the issue in a dummy part that would be just as good.

[Mike.Grau]

Hi @Anonymous,

Thank you for sharing this with us.

Yes, it would be great if you could share an example file and screencast with us.

Could you may share more details what are the steps to create the toolpath in your design? 

You can also send a private link to your design to mike.grau@autodesk.com.

Looking forward hearing from you.

Thanks,

[Mike.Grau]

Hi @Anonymous,

Thanks again for raising our attention to that.

I just want to check if you have had a chance to share your design?

Thanks,

[Anonymous]

Sorry for the delay. Here is an example file i created with different size insets for inside corners. Please notice once the inset is equal to or less that half my tool size the path will not generate.

[Steinwerks]

As best I can tell I think this is due to the algorithm being unable to actually cut a linear section of the selected contour. Changing the Stock to Leave Radial value to even -.00001" (yes, ten millionths) yields a viable toolpath, so at least there is a workaround as that will simply get rounded out in the post processor. Still feels like a bug though.

@Mike.Grau what do you think?

Edit: tested the geometry with a 3/8" end mill and wound up with the same issue: Stock to Leave must exceed the radius of the tool. I this has to do with maintaining tangency with the commanded toolpath geometry. Since the rounded corner does so until it meets the next edge it will happily oblige, but the square corner basically skips an edge and falls apart.

[Mike.Grau]

Hi @Steinwerks,

Thank you for sharing the file.

Yes, I do think this needs to be forwarded to the development team.

I have tested a couple things in the mm range and I could see that the maximum potential fillet radius is determining

the possible diameter for the tool to generate a valid toolpath.

I will log this and share the file with the team.

Thank you for mentioning the work around. I will go ahead and create an article just in case another

user rolls over a similar issue.

Thanks,

[Anonymous]

Thank you @Steinwerks. The stepdown I needed was actually .09" , much less than the radius of the tool, so in this case the work around would not work. I am glad I could bring this to Autodesks attention and hope it can get fixed in the future. There are other ways to achieve this cut but it would be nice to have the issue resolved.

[abrownAG8YF]

FYI this is still an issue in HSMWorks 2019 R3.43434. I'm currently trying to program a 2D contour around the outside of a small part with a 0.5" end mill and I cannot get a tool path output with any sharp corner option enabled. I can share the file if it would help.

[Steinwerks]

Yes, I would suggest attaching an example file.

[abrownAG8YF]

See the attached file. The third operation will output a tool path if "roll around corner" is selected but will not output a path if "make sharp corners" or "roll around corner" are selected.

[abrownAG8YF]

I discovered that if I open up the tolerance and smoothing deviations to a total of 0.0007" the tool path is calculated with the sharp corners as intended. I'm guessing that the contours on the part were causing issues.