Clean chamfer on an arc with inconsistent distance

brian_dieckman

Sorry if that title is confusing, and it's probably best to just show you the drawing rather than trying to explain it. 

Here's a link if you want to look at it in Onshape.



The part in blue needs to be chamfered from the outer edge at the top to the inner edge at the bottom. The inbuilt chamfer tool *almost* works... I can set two distances to get one edge perfect, but since the distance between the inner and outer shapes aren't consistent (It's not an inset operation, but two disparate profiles) it's impossible to get the chamfer to go all the way to the outer edge everywhere. (see example below... The chamfer on the upper right corner, right and left edges don't extend all the way to the outer profile.)



Clearly the Chamfer tool isn't the right one to use but after experimenting with Loft and Sweep, I'm getting nowhere.

Thoughts?

Alex_Kempen

I think you might have more success if you're able to make all of the edges in your profile tangent to each other. Unfortunately, your profile is imported (and thus largely unconstrained), so you might have to redraw it - you could also try importing a reference image of your profile, then tracing it out with 2D splines (with curvature constraints) or arcs and lines (with tangent constraints). Once your edges are smoothly connected to each other, you can try chamfering again, or sweeping and lofting if that still doesn't work. 

tim_hess427

@brian_dieckman - I don't think chamfer will work. Here's how I would approach this. 

1. Extrude the inner and outer profiles up as surfaces. Extrude them separately so that you can extrude the outside profile higher. 
2. Use loft to create the angled top surface connecting the tops of the two surfaces created in step 1. 
   
3. Use enclose (or loft, if it's not planar) to close off the bottom surface.

matthew_stacy

@brian_dieckman, see if this approach accomplishes what you're seeking.  Apply the DELETE FACE tool to remove the faces that will be consumed by your chamfer.  Be sure to select the LEAVE OPEN option which will convert the solid (part) back to a surface model. 

Then LOFT a surface from one edge to the other.

https://cad.onshape.com/documents/97f09a1082bf16b2c4edc055/w/0a212b0712a543c4931d4e31/e/c80a893c5308ffc13ac6ff36

Note that your geometry includes a few discontinuities (possibly resulting from improperly constrained sketches) that will have to be corrected before this method can be applied successfully.  I generated a highly simplified example just to illustrate the method.

Happy modeling.