Face: invalid tolerance value

[56jimalexander]

I've stripped all but the essential components from this model.
The 2 cuts, 2 extrudes, and the sweep all pass a geometry check.
When I do the geometry check on the Thickness, I get an error:
Face23 Invalid Tolerance Value.
It appears that Face23 is the entire Thickness.
I can not find anything that tells me how to change the tolerance value. Is there such a setting?
I can add more features like cuts to Thickness but I am not able to change the thickness value.
If someone could take a look to see if I'm doing something wrong, I could certainly use some advice.

OS: Windows 10 Version 2009
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24291 (Git)
Build type: Release
Branch: releases/FreeCAD-0-19
Hash: 7b5e18a0759de778b74d3a5c17eba9cb815035ac
Python version: 3.8.6+
Qt version: 5.15.2
Coin version: 4.0.1
OCC version: 7.5.0
Locale: English/United States (en_US)

[chrisb]

Thickness is one of the most picky functions in FreeCAD. It frequently fails if B-spline surfaces are involved (which are created by sweeps). The issues come directly from the OCC geometric kernel. There is not much that can be done.
You probably have to remodel the inner part as well and then cut it from the current model.

[56jimalexander]

Thank you Chris. This is helpful.
With respect to the tolerance, is there a way to change the value?

[chrisb]

With respect to the tolerance, is there a way to change the value?

I admit that I have given up to fix broken Thicknesses. It is comfortable if it works out of the box, but if it doesn't it usually costs lots of time and in the end I have to remodel anyway.

[Vincent B]

Thank you Chris. This is helpful.
With respect to the tolerance, is there a way to change the value?

https://wiki.freecadweb.org/OpenSCAD_In ... nceFeature
but I guess that no help at this time.

[TheMarkster]

Suggestion.

Delete Thickness
Select Sketch125, apply Part 2D offset tool with value = -2mm (or what thickness you desire)
Extrude the Offset2D object symmetrically some large amount so it extends above and below the original.

Snip macro screenshot-688f22.png (61.67 KiB) Viewed 2201 times

Label this extrude "inner" or some such and hide it temporarily.

Select the 2 bottom faces and create a Draft Facebinder object. Extrude the Facebinder in the Z direction 2mm, label this "sole".

Snip macro screenshot-cd2aae.png (45.96 KiB) Viewed 2201 times

Do the same with 2 faces on the top, extrude downwards 2mm and label "upper". (or go up here if you prefer)

Snip macro screenshot-94b016.png (66.15 KiB) Viewed 2201 times

Select Cut117, then "inner" and do a boolean cut. Fuse new Cut object with upper and sole. (I had to set Refine = False on the Fusion object or else there were invalid curves on surface errors in check geometry report.)

Snip macro screenshot-8c7757.png (53.61 KiB) Viewed 2201 times

[56jimalexander]

Markster, this looks promising but your suggesting some things I'm not familiar with. This offset thing looks like something I've wanted to do but didn't know where to look. I will be studying your post and giving it a try.
Thank you

[56jimalexander]

Thank you Chris. This is helpful.
With respect to the tolerance, is there a way to change the value?

https://wiki.freecadweb.org/OpenSCAD_In ... nceFeature
but I guess that no help at this time.

I can't find "OpenSCAD". How do I get to that command?

[56jimalexander]

Markster, thank you for the model and the clear explanation.
I duplicated this process successfully. Learning 2D OFFset and facebinding is very benefitial for me.

[TheMarkster]

You might need to install the OpenSCAD binary. Then you will be able to use the OpenSCAD workbench.