topic Re: Chamfer skipping section in Fusion Design, Validate & Document Forum

Chamfer skipping section

Anonymous — Sun, 17 Oct 2021 21:54:43 GMT

I'm attempting to add a chamfer on this model. It mostly works but misses the first "bump" depending on where I click it. In this picture I selected the edge between the end and the bump. If I select the line between the bumps the the bumps on both sides are missed, while the others are fine.

Re: Chamfer skipping section

jhackney1972 — Sun, 17 Oct 2021 22:00:06 GMT

Please attach your model to a Forum reply or your original post. If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section of a forum post to attach it.

Re: Chamfer skipping section

Anonymous — Sun, 17 Oct 2021 22:15:41 GMT

Thanks for the help. here is the model

Re: Chamfer skipping section

jeff_strater — Sun, 17 Oct 2021 22:51:28 GMT

from the image, it looks like that last cylinder might be a separate body. If so, you'd need to Combine it with the rest of the design for the Chamfer to work as you want it to.

Re: Chamfer skipping section

jhackney1972 — Sun, 17 Oct 2021 23:05:06 GMT

@jeff_strater , it is not a separate body, the whole is extruded from one sketch. The only way I can find effectively to do it was to use a Surface cut and the Mirror and Pattern. Model is attached.

Edit: If you need further explanation on what I did, I will create a Screencast for you.

Re: Chamfer skipping section

Anonymous — Thu, 21 Oct 2021 02:50:11 GMT

Thanks so much for the help. Sounds like I did something reasonable in my model and this issue was more of a limitation/bug in the program.

thanks again

Re: Chamfer skipping section

Rafal.Chlod — Thu, 21 Oct 2021 10:03:25 GMT

From my understanding, Fusion tries to make a chamfer around the cylinders, rather than just diagonally as along the main contour. Since the cylinders has 1,5mm diameter, the 1mm chamfer will not be physically possible and the program starts to get lost. I tried to make smaller chamfer and the result is on the screenshot bellow.

Looks like the jhackney1972 solution is the best method to do it the proper way.

Re: Chamfer skipping section

HughesTooling — Thu, 21 Oct 2021 11:06:37 GMT

@Rafal.Chlod @jeff_strater I thought I'd try a different approach adding the circular ribs to the chamfered body but no matter what I select this fails. Pretty sure this should work.

Even fails with a square! I reported another example a few days ago where extrude to fails if you try Extrude To a conical surface. See attached file and try editing the extrude.

Re: Chamfer skipping section

jeff_strater — Thu, 21 Oct 2021 20:47:04 GMT

a couple of things with this model.

First, @Rafal.Chlod is correct - Chamfer is defined as an edge chamfer, so it will try to go around the cylinders, not across it, as it seems you want it to, @Anonymous . You can see this at a chamfer distance of 0.3:

and, at 0.4, it starts to get "lost":

and some of the cylinders get sliced (which, I understand, is what you might want, but I would argue is incorrect behavior). Unfortunately, increasing the chamfer width does not turn all those cylinders into "sliced" cylinders

@HughesTooling regarding your approach. What is missing is better handling of automatic face extension. Today, I think, only planes and cylinders can be auto extended in Extrude. The face you need to extend is a cone. So, the workaround is to do it manually:

Re: Chamfer skipping section

TheCADWhisperer — Fri, 22 Oct 2021 06:50:11 GMT

@Anonymous

Re: Chamfer skipping section

HughesTooling — Fri, 22 Oct 2021 08:17:34 GMT

@jeff_strater Here's the workaround I've used in this situation. I extrude part way up the chamfer then delete the top faces and then the conical face is extended. So not a problem in general with extending surfaces, just Extrude To option seems a bit fragile.

Mark

Re: Chamfer skipping section

jeff_strater — Fri, 22 Oct 2021 13:15:06 GMT

that's not what I meant, @HughesTooling , I was referring to the "auto extend" inside of the Extrude command:

I was trying to use this face as the "to object" here:

but that auto-extend inside Extrude only works on limited face geometry