One chamfer works, one doesn't?

[StarlessCaviar]

I'm having a weird issue that I can't figure out. The chamfer on the "top"side goes all the way through the padded "wing", but the chamfer on the bottom side seems to get stuck on a hidden edge and so it doesn't follow all the way through. I have refine shapes on in properties.

What could be the problem?

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window-stop-v9.FCStd

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OS: macOS 10.16
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24291 (Git)
Build type: Release
Branch: (HEAD detached at 0.19.2)
Hash: 7b5e18a0759de778b74d3a5c17eba9cb815035ac
Python version: 3.8.8
Qt version: 5.12.9
Coin version: 4.0.0
OCC version: 7.4.0
Locale: C/Default (C)

[chrisb]

Hi and welcome to the forum! Good first post (FreeCAD infos, file, image, description).

I guess it is an iss coming directly from the third party OCC geometric kernel, and not much can be done. As a workaround you can cut the excess with a pocket.

[openBrain]

Without direct link to OP, but there is something weird here. When I open file, I'm strictly unable to use the 'Remove' function when editing the chamfers (Chamfer002, Chamfer003) ...

EDIT : Got it ! 'Remove' isn't available when only one edge is added. Not sure this is very user convenient though...

[GeneFC]

I am guessing there is a precision problem when adding the wings. Not sure if it is a "coincidence" problem or a "lack of coincidence" problem.

You might try adjusting the wings to overlap with the basic shape by a tiny amount. (Or similar adjustments.)

Gene

[GeneFC]

Without direct link to OP, but there is something weird here.

Yes, there is something strange. Only one small edge seems to be in the dialog, but several edges are in the chamfer.

Gene

[openBrain]

Yes, there is something strange. Only one small edge seems to be in the dialog, but several edges are in the chamfer.

Gene

I'm not surprised about that as it is a standard behavior in FreeCAD that chamfer edge are extended as much as possible by following the subsequent edges.

[heron]

When making zoom in mark point:

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two edges are visible instead one and the face continues:

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It seems to me that the "Sketch_Wing" for the "Pad_Wing" of your model is not correctly placement.

Greetings.

[domad]

....

Hi StarlessCaviar, hello to the Community!
... the problem is highlighted in the animated * .gif.
I recommend making fillets and chamfers at the end of the modeling flow, never in between.

[StarlessCaviar]

Thanks to everyone for your kind input! I realized the wings were not properly aligned as some of your mentioned. It was because I was trying to keep the drawing parametric, and since I can't set Pads to 0 distance, I had set 0.01 thicknesses but didn't account for that in the sketch for my wings.

If anyone can suggest how to set a Pad to zero in case I want to use it in the future, please let me know!

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[chrisb]

You cannot set the length of a pad to 0, but you can add another pocket, wich cuts it completely off.

Besides, for my taste your first sketch is far too complicated. 350 Constraints are far too much and numerous unnecessary construction lines should be removed. Limit yourself to roughly 100 constraints, use the partial symmetry and add the non symmetric stuff separately.