Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Need help with chamfering grooves on a mill

Message 1 of 6
154 Views, 5 Replies

Need help with chamfering grooves on a mill

tried a few different ways. cannot even get the regular(bottom) chamfer to work let alone trying the topside chamfer.


anyone have tips? attached is the f360 file.




Message 2 of 6

Hi, we use these tools regularly.  I use 2d contour and fiddle with side and depth allowance until it looks right.  Then I save a template for this tool for ease of use the next time.

Message 3 of 6

Folks that are much smarter than I have done the brain-work and come up with some nice expressions that can handle this with no fiddling whatsoever. Initially, it was one formula, but I didn't like that it put the tip of the tool right on the edge of the selection. As such, I've tweaked it a bit and now there's one for "topside" and "bottom side". 


I've attached the template (zip folder) and the file here.


Nerd alert!

Here's the expression(s) that go in the radial and axial Stock to Leave:



(tool_diameter-tool_tipDiameter)/2-chamferWidth-2*(chamferTipOffset/Math.tan((90-tool_taperAngle) * Math.PI/180))-.005in



-((tool_diameter-tool_tipDiameter)/2*Math.tan((90-tool_taperAngle) * Math.PI/180))+(chamferWidth*Math.tan((90-tool_taperAngle) * Math.PI/180))-.005in



The above is for deburring the backside of a part and it gives you a .005" offset to tool centerline. You need to set your Chamfer Width and Chamfer Offset to zero:



The "Stock to Leave" portions are filled in via the expression.




Seth Madore
Customer Advocacy Manager - Manufacturing
Message 4 of 6
in reply to: seth.madore

**** dude!!!  Thank you so much!  I am saving these equations for future use for sure, awesome!!

Message 5 of 6
in reply to: DarthBane55

Yep, they're quite handy! And, they do adjust for tool angles, even though it's most common to use a 90 degree Double-Angle tool

Seth Madore
Customer Advocacy Manager - Manufacturing
Message 6 of 6

Wow thanks! I’ll give this a try on Monday! 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report