Empty Error in Dimension Change

[bhodder]

Hi,

I am working on a design that was created by another team member. When I attempt to change the diameter constraint on a pocket the sketch gets an error and does not change it in the 3D rendering. The error shows no details and I cannot determine what the issue is. Is there a way to find the details of the error? If you hover over all it says is "Error".

Thanks!

[bejant]

Hi,

viewtopic.php?f=3&t=2264

That diameter change probably caused the faces and edges to get renumbered, breaking the model. Can you upload it to the forum so someone can examine it?

[bhodder]

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6706 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: f86a4e411ff7848dea98d7242f43b7774bee8fa0
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

I am trying to change the value in "Sketch" under Pocket004. The error shows once you try to save a value but you can see that it does not change the model.

3_Pod.FCStd

(51.21 KiB) Downloaded 29 times

[chrisb]

bejant was right. When you make Fillet invisible and CableGroove visible (select in the tree, toggle with space bar) you can see that the change has an effect. Alas, the numbering of edges and faces has changed, so that subsequent features don't work any more -> the object becomes invalid and FreeCAD shows the last usable state.
That is a so called topological nameing issue, you find lots of informations here in the forum, e.g. here are some hints how to proceed: https://forum.freecadweb.org/viewtopic. ... 14#p155014

[Willem]

Hi, the topological problem can be repaired in sketch004. The outer circle is a link to external geometry and this can be deleted. An extra dimension of 5,96 mm should be added to make the sketch full constrained again. After this Sketch has an error again and must be re-attached with a face of "Cable Hole" to repair the topological numbering. Now Sketch can be edited to change the diameter of 18 mm to another value

Schermafdruk van 2017-02-23 23-23-48.png (23.93 KiB) Viewed 1205 times

[bhodder]

Thanks all, that was the problem. In fact, I had to do it on several sketches and faces after fixing the first one.

Again, thanks for all the help.