I can confirm the issue. But i am guessing this likely should work as expected (like it did in FreeCAD 0.16). Therefore i am guessing there is a bug involved somewhere.
This is normal and to be expected. Going back in the design history to add/remove geometry will produce issues for features added after. This is what "topological naming" ongoing projects will try to improve in the future. Being able to go back in design history and by adding/removing geometry. To experience less issues with the features added after.2. When I add faces to earlier features, for example by removing a Fillet that I created to early (or in this example by adding a fillet) the later features become referenced to completely different faces:
I don't mind re-mapping the face when I add/remove faces. After all it's difficult to define what constitutes "the same face" after you have changed the geometry.
If I do that, how do I make pockets starting from a face?you need to stop mapping sketches to faces - entirely
The master sketch is not the only technique mentioned to make models robust, and sometimes it might be too much effort to work around mapping to faces.
The use of a mastersketch is just one piece of the cake, the next are datum-features, but not referenced to shape. Next technique is to use a shape without fillets and chamfers. It could be a pad or part-extrude (as shell), pad parametric downgraded to shell (Lattice2-workbench). Set this shape on top of every design as a skeleton model, based on a master sketch. It will not break and has no problems with topo naming and you can use all faces, edges and vertices as reference for other objects. Copy them to the body you want. If you change the mastersketch and the skeleton modell all dependent geometrie will follow full parametric.chrisb wrote: ↑Mon Apr 16, 2018 4:54 amThe master sketch is not the only technique mentioned to make models robust, and sometimes it might be too much effort to work around mapping to faces.
But in most cases you can use a DatumPlane which references Sketches and on that DatumPlane you can attach a Sketch for creating a pocket. And again, external references which are used in that sketch should use other sketches instead of referencing edges or vertices of a solid.