I am trying to create a cutting edge on the highlighted surface. I attempted to add a chamfer with no luck. Any ideas?
Try this: Select the inside edge of the highlighted surface, then create a Ruled Surface with the "Normal to surface" option. Make the distance a little bit more than the thickness of the part (just to be safe). Then start a sketch on a plane normal to that curve (the Front plane might work), and sketch a triangle with one side along that ruled surface, another side horizontal, and the hypotenuse representing the cut you want. Now start a Swept Cut using the sketch as the profile, the inner edge as the path, and the outer edge of the ruled surface as a guide curve. Under Orientation/twist type choose Follow path and 1st guide curve. Now when you say ok it might ask for which bodies to keep (it might have created little slivers somewhere) but just pick the main body and see if the result is what you want.
I would attach pictures and an example file but uploading seems to be disabled for me right now.
Not sure I know exactly what you want, but how about this:
Create a 3D sketch and Convert Entities on one of those curved edges. Create a plane normal to that sketch curve and draw a 2D sketch containing the cut profile geometry. Then just sweep-cut this profile along that path defined by the part edge...?
Thank you! Worked well!
When you say "normal" I read perpendicular.
Thicken a trimmed surface body.
Create the cylinder as a surface body.
Trim as needed.
!easy, just split the blue face the distance in from the outside that the chamfer would start from, just use a sketch for that.
Then offset the blue face back into the model the same distance, extend the surface out past the OD and then split the outside face with the offset surface.
now loft a surface between the 2 split edges and then use replace face which gets rid of the sharp corner,
works like a champ every time
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