I have had an issue since 2009 with Autodesk Inventor. We use a lot of Corian-type solid surfaces on our display cases. We have them cut by our CNC in strips to reduce waste, then we assemble them and place the solid surface in the final display case assembly.
The issue is that I need to show a 1/8” round over on the top edge that the customer would touch. I wish the IPT (Inventor part file) would allow me to create a fillet to be “from to.” I have tried to find a way for the fillet to only be located where I need it. Say the CNC part is 72” long but I need the 1/8” fillet to start 4” from the left end and stop 6-1/2” from the right end; the problem in trying to show the fillet in the part file is that the 3-axis CNC is not to cut the fillet. Instead, it is the case builder's responsibility to create that when the solid surface is assembled. So I tried to find a way to create a fillet in the solid surface IAM (Inventor assembly file), but the same issues exist in getting the fillet to stop along a single edge where I need it to.
My solution is to create a sketch on the top face of the assembled solid surface and create several connected lines where I needed the fillet feature to be.
I then created a concave 1/8” arc with two perpendicular lines for the 1/8” fillet shape. The line that creates the path is offset from the cut edge by the fillet radius size, seen as a dashed line and cyan in color.
Depending on which line I choose, the two shown paths will give different results.
I then used the Sweep feature to select the concave arc and lines and sketch the top face as the path to get the desired result. It even created the fillet in the corner.