Contours and chamfers on a simple part

[jfhext]

I've got a simple part (https://a360.co/3E0LVuN) that I'm trying to mill from some 1/4-thick G10 material. I have a 1/8-inch flat endmill, and a 60-degree-included-angle chamfer bit. At this point, I feel as if I've tried every possible setting on 2D Adaptive Clearing, 2D Pocket, and 2D Chamfer (using the flat end-mill) to cut the circular groove in the top surface, and everything I can think of in 2D Chamfer (using the chamfer bit) to cut the outer face. Mostly I seem to end up with the dreaded "empty toolpath" error, although sometimes I come up with things that cut away everything EXCEPT the circular groove, or that crash into the outer face and give me a profile that looks like this:

xxx|

xxx\

(i.e., the top bit is vertical, and then there's a chamfer at the bottom). 

I've watched several of Lars Anderson's videos, which are very nice, but when I try to do the same things he did, it doesn't seem to work for me. 

Can anyone make some suggestions, please, or offer a pointer to somewhere where I could learn a bit more?  

[jfhext]

OK, so we all have bad days.

I still don't know how to mill the chamfer, but for the circular slot, I figured out what was wrong:

I went back to look at it, and realized that it was less than 1/8 wide, so I couldn't possibly cut it with a 1/8 mill. And it was less than 1/8 wide because I'd taken the ID and added the groove-width to it... but should have added two TIMES the groove-width, because I was creating the diameter of the outer circle rather than the radius. (D'oh!) Apparently all I had to do, after spending 2 hours on this, was ask a question, and then I'd instantly be able to solve it myself. 

I'd still appreciate any help on the chamfer, of course. 

[seth.madore · Accepted solution]

First off, the gap in the groove is only .08", so that will constantly result in "Empty Toolpath" errors. You need to use an endmill of the same size or smaller. If you do open it up to .125", I would use a 2D Contour, Lead-in/out turned off and a Ramp entry.

For the Chamfer, you can do a couple things:

1) Create 2x 2D Contour toolpaths with the defined tool that you have. The first one is the top Contour, Chamfer size set to zero, Tip offset set to .1. The second contour would be the bottom contour and would have a Chamfer and Tip Offset size set to 0 as well.

2) Define your tool as a Taper Mill and leverage Multiple Depths with Wall Angle.

 

-Edit- Just saw your reply acknowledging the gap issue.

[jfhext]

I take it that the idea of the 'two contours' thing for the chamfer is that F360 can't figure out that it needs to do multiple ever-lower passes as it would do with a flat end-mill or even a ball-end mill. Is that right? So I'm doing it by hand just to get the job done.

Second, I'm worried that we're taking an awfully large bite of material in doing this --- isn't this going to put a lot of bending load on the chamfer bit? Is there a way to cut a slightly-offset-outward version of the chamfer with a somewhat thicker/stiffer ball-end-mill, and then have the chamfer bit just do a cleanup pass (or two passes)?

Thanks for the quick response!

[seth.madore]

Yep, Chamfer tools aren't recognized in the "Multiple Depths", in regards to Wall Taper Angle. I'll try to get a ticket logged to see if we can improve this experience.

Yeah, for roughing it out, you could just toss on a Ramp toolpath with a ball endmill and turn on Stock To Leave.