90° thin walls, how to fillet/chamfer more than wall thickness?

[TLS]

Hi, I'm designing some box shape, with 1.5mm wall thickness

What is the best way to chamfer fillet, I would like to have 7mm chamfer. part design fillet only allows me to maximum fillet the wall thickness.

I can add material to the inside by filleting the inner corner, but the outside corners it only wants to do the thickness of the top/bottom pad (extruded rectangular sketch)

thank you

[ulrich1a]

You could try to make a solid box and chamfer it. After that you can use the thickness-tool from the Part-Workbench in order to make the box hollow.

See here: http://www.freecadweb.org/wiki/index.ph ... _Thickness

Ulrich

[TLS]

Any solutions for my existing design?
Because quite some time went in it, and sizewise everything is ok, I just want to add some 'design' features now to make it more appealing...

[jeno]

An alternative solution is to use sweep for the wall and afterwards add the baseplate, then a boolean union and your done.

[NormandC]

Hi,

part design fillet only allows me to maximum fillet the wall thickness.

That's actually a limitation of the geometric modeling kernel, a software library called Open Cascade, over which the FreeCAD developers have no control. It cannot fillet an edge if the radius makes one of the faces attached to the edge disappear.

Any solutions for my existing design?

Removing the material like jeno suggested is your only option AFAIK.

[sgrogan]

@TLS

Are you looking for something like this?

Chamfer.PNG (49.7 KiB) Viewed 3222 times

[TLS]

Hi Sgrogan, that is indeed still my project

I managed to do something like that with triangular sketches, padding and pocketing. However when I try to do this all around the sketches lose their external edges because of the pockets on the already chamfered edges.

Do you have a trick to do this all around the top lid of the Arduino case?

edit: I see you managed to do this via the chamfer function.... euhm, how?

[ektus]

edit: I see you managed to do this via the chamfer function.... euhm, how?

As a guess: First add material on the inside with a chamfer, then apply another chamfer to the outside edge to remove the material there.


Regards
Ektus.

[sgrogan]

As a guess: First add material on the inside with a chamfer, then apply another chamfer to the outside edge to remove the material there.

With just one additional step.
First select all 4 internal edges and apply a 6.121 mm chamfer. Next switch to the OpenSCAD workbench, select the just created chamfer in the Tree view and apply the RefineShapeFeature This will remove the split face lines at the thickness of the top/bottom pad in your model, allowing you to overcome the limitation NormandC explained. Finally select the four external edges and apply the 7mm chamfer.

cover.PNG (76.45 KiB) Viewed 3175 times

cover.FCStd

(26.28 KiB) Downloaded 37 times

[TLS]

With just one additional step.
First select all 4 internal edges and apply a 6.121 mm chamfer. Next switch to the OpenSCAD workbench, select the just created chamfer in the Tree view and apply the RefineShapeFeature Image This will remove the split face lines at the thickness of the top/bottom pad in your model, allowing you to overcome the limitation NormandC explained. Finally select the four external edges and apply the 7mm chamfer.

Great, thank you Sgrogan