Difference between revisions of "Topological naming problem"

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Adding datum objects is more modelling work for the user, but ultimately produces more stable models that are less subject to the topological naming problem.
 
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Revision as of 21:07, 4 May 2019

Introduction

The topological naming problem in FreeCAD refers to the issue of a shape changing its internal name after a geometrical modelling operation (pad, cut, fuse, chamfer, fillet, etc.) is performed. This will result in other parametric features that depend on that shape to break or be incorrectly computed. This issue affects all objects in FreeCAD but is especially notable when building solids with the PartDesign Workbench, and when dimensioning those solids with the TechDraw Workbench.

  • In PartDesign, if a feature is supported on a face (or edge or vertex), the feature may break if the underlying pad changes size or orientation, as the original face (or edge or vertex) may be internally renamed.
  • In TechDraw, if a dimension is measuring the length of a projected edge, the dimension may break if the 3D model is changed in such a way that it affects the edge.

The topological naming issue is a complex problem in CAD modelling that stems from the way the FreeCAD core routines handle updates to the shapes created with OCCT geometrical operations. As of FreeCAD 0.18 there is ongoing efforts to reduce or eliminate such topological issues. These new developments may eventually be included in future versions of FreeCAD.

The topological naming problem most often affects and confuses new users to FreeCAD. Careful modelling and use of supporting datum objects like planes and local coordinate systems is advisable to produce stable models that aren't easily subject to such errors.

Example

1. In the PartDesign Workbench, create a PartDesign Body, then use PartDesign NewSketch and select the XY plane to create a sketch; then perform a PartDesign Pad to create a first solid.

2. Select the top face of the previous solid, and then use PartDesign NewSketch to draw another sketch; then perform a second pad.

3. Select the top face of the previous extrusion, and once again create a sketch, and a pad.

4. Now, the second sketch will be modified so that the length is towards the X direction; doing this will recreate the second pad. The third pad will stay in the same place.

5. Now, modify again the second sketch, so that it leaves the limits defined by the first pad. By doing this, the second pad will recompute correctly, however, when looking at the tree view, an error will be indicated in the third pad.

6. By making visible the third sketch and pad, it is clear that the computation did not proceed correctly. The third sketch, instead of being supported by the top face of the second pad, appears in a strange orientation, resulting in an invalid pad, as this pad would be disconnected from the rest of the PartDesign Body.

Solution

As explained in the feature editing page, a solution to this problem is to support sketches not on faces but on datum planes which are themselves offset from the main XY plane of the PartDesign Body.

In this manner, it doesn't matter if the second sketch changes, as the modified second pad will not affect the support of the third sketch.

Adding datum objects is more modelling work for the user, but ultimately produces more stable models that are less subject to the topological naming problem.