"Topological naming problem"

[bnemec]

This might be one of the best documents about the inherent behavior of history based modeling, why upstream edits break down stream things (features, annotations, assembly relationships). I run into so many "experienced" CAD modelers that appear to have no concept of this behavior that is fundamental in any history based modeling environment.

https://wiki.freecad.org/Topological_naming_problem

The first time I read this I had Solid Edge in mind as I had not used FreeCAD at that point. The exercise can be followed nearly identical in either SE or SW.

Not a plug for FreeCAD or anything, it was just one of the least obscured presentations of the topic. At least for the way my mind absorbs stuff.

[jcapriotti]

The term "Horizontal" modeling comes to mind from many years back. Basically use planes and the original sketch geometry to try and build the model less vertical and more horizontal. The tools we have today allow for this but few have the experience or will to model this way it seems. Really depends on the part and how complex it it.

[JSculley]

Out of curiosity, does SolidEdge fail that exercise in the way that FreeCAD does? Because SOLIDWORKS does not.

[bnemec]

Out of curiosity, does SolidEdge fail that exercise in the way that FreeCAD does? Because SOLIDWORKS does not.

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It does not. I could have been less vague about the details but I wasn't going for the exact behavior of each system. The point I was trying to get to is for the user to understand what edits cause geometry IDs to change in the system you're using. Simple exercises like this will show what does and does not destroy face IDs.

I've been through week long formal trainings for Solid Edge, Inventor and now Solidworks and non of them devoted, in my opinion, enough time to this concept to help users not shoot themselves in the foot. That's why I like this simple training document page to help users understand why FreeCAD drops the ball when a new face is created because a sketch is edited and that causes the other faces to be renumbered. Solid Edge and Solidworks handle this better, but both have room for improvements when it comes to helping the user interact with and understand geometry IDs.

[jcapriotti]

SolidWorks seems to tie the face ID to the underlying sketch entity. I have covered in training that when modifying a model sketch, always edit, never delete sketch entities unnecessarily. I started covering this because users would get frustrated trying to edit a complex sketch and having sketch relations bind/error, and they would just start deleting parts of the sketch and redraw it. Which of course wreaks havoc on everything downstream. Then you have to explain that their change didn't just affect downstream features in the same part, but the part's drawing and potentially mates in every assembly that uses the part.

[FEAnalyst]

Speaking about FreeCAD, TNP is particularly pronounced in that software. That's why they have that comprehensive description. However, there's already a fix for that created by a user and it's currently available in his branch called Link Branch. They are working on implementing this fix in the main version and the next release should have it. Once the implementation is done, the release will become FreeCAD 1.0 instead of 0.21 since it's going to be a huge improvement. Of course, it won't eliminate the problem completely but it should bring it close to the level of commercial CAD software, making work in FreeCAD much better.

[bnemec]

Speaking about FreeCAD, TNP is particularly pronounced in that software. That's why they have that comprehensive description. However, there's already a fix for that created by a user and it's currently available in his branch called Link Branch. They are working on implementing this fix in the main version and the next release should have it. Once the implementation is done, the release will become FreeCAD 1.0 instead of 0.21 since it's going to be a huge improvement. Of course, it won't eliminate the problem completely but it should bring it close to the level of commercial CAD software, making work in FreeCAD much better.

Are you speaking of the branch that's mentioned in the long winded video "FreeCAD Fundamentally Broken..." that is linked at the bottom of the TNP documentation page?

[FEAnalyst]

Are you speaking of the branch that's mentioned in the long winded video "FreeCAD Fundamentally Broken..." that is linked at the bottom of the TNP documentation page?

Yeah, that one. You can download it from here: https://github.com/realthunder/FreeCAD/releases

It contains various other improvements too so many users stick to it.

Its owner is working with FreeCAD devs to implement that TNP fix.

[zwei]

Thanks for the sharing. A really interesting read.

This is actually one of the many reason i had been leaning toward horizontal modelling...
That satisfaction when you change your base/first sketch and nothing break despite having 100+ features

[bnemec]

Yeah, that one. You can download it from here: https://github.com/realthunder/FreeCAD/releases

It contains various other improvements too so many users stick to it.

Its owner is working with FreeCAD devs to implement that TNP fix.

Can the .FCStd files be opened/edited in either of the branches or are they exclusive?

[FEAnalyst]

Can the .FCStd files be opened/edited in either of the branches or are they exclusive?

They are compatible but some features specific to Link Branch may not be recognized properly in the official version. For example, multiple separated solids within a single Body container.