topic Re: Chamfer Mill - why is it invalid for milling? in Fusion Manufacture Forum

Chamfer Mill - why is it invalid for milling?

lindsay.fowler — Sat, 07 Nov 2020 05:55:09 GMT

Hi All,

I see this was unsolved back in 2017.

I have 2F D4*90 deg *50L bit that I purchased for chamfering.

I entered this in my tool library as a Chamfer Mill (though it look nothing like the one in the picture -there are no V shaped bits in the F360 tool library types)

To machine a chamfer I used 3D Contour ( - because you can't do a CAD chamfer with Chamfer. https://www.youtube.com/watch?v=rOYt1K2pVQc)

Anyhow, Fusion is complaining: "Invalid tool for milling"

Why is it invalid - it's a mill, isn't it?

Thanks for any help.

Re: Chamfer Mill - why is it invalid for milling?

seth.madore — Sat, 07 Nov 2020 10:46:58 GMT

There are a couple of misunderstandings here:

1) A Chamfer tool IS a V-shaped tool. While the static gray image does show something a little bit different than what you might expect, it's still most certainly a V tool, just with a large flat on it and using inserts instead of ground flutes.

2) John didn't say you CAN'T use it with modeled chamfers, just that his preference is NOT to.

For modeled chamfers using the 2D Contour option; select the BOTTOM edge. For modeled chamfers using the Chamfer toolpath, select the TOP edge, but set your Chamfer Size to zero. You still need to input a Chamfer Tip Offset in either case

Re: Chamfer Mill - why is it invalid for milling?

engineguy — Sat, 07 Nov 2020 12:12:17 GMT

@lindsay.fowler

Is this a situation where you want to machine a 45 degree slope that is larger than your V tool face and you want to use the 3D Contour toolpath ??

If so then the easiest way I have found is to create your V pointed tool as a "Tapered Tool", to get the point set the Diameter to something like 0.01mm or less, you may get an error saying that the value is small than your Tolerance setting so adjust either the tool or the tolerance to suit, and set the the shaft value to the actual V bit diameter and you will get a V pointed (Well almost) tool as in the image below that Fusion will accept for the 3D Contour toolpath 🙂

You can rough out first with any mill tool but I prefer a Flat bottom Chamfer type tool but again created in the Taper tool section, you can try whatever you like in the attached example file attached, Flat, Bull Nose, Ball Nose 🙂 🙂 🙂

Stay Safe

Regards

Rob

Re: Chamfer Mill - why is it invalid for milling?

lindsay.fowler — Sat, 14 Nov 2020 03:38:47 GMT

Ok thanks @seth.madore . I did get the chamfer machined, but only using 2D contours. Now with fresh eyes and help from you, I gave the 2D Chamfer operation another try and it worked fine. It hadn't occurred to me to set the chamfer width to 0.

@engineguy that's also very helpful thanks. To answer your question, this was not a case where the chamfer was larger than the cutting edge. I had tried the Tapered Mill and it too was causing me confusion with the same strange error: "not valid for milling".