Invalid A2+-assembly of valid objects

[wandererfan]

ping

ping

I may be on to something. Fixing the tolerances in the parts, turning the shells into solids and fusing the result gives something that passes Check Geometry without a peep. Not sure if this is a general solution yet, but it looks promising.

I've attached a couple of well behaved assemblies. The result passes and can be fused to another part without complaints.

If you run into more problematic assemblies, please pass them to me. I can always use more test data.

wf

[Roland]

Not bad, Wanderfan!
Actually very good.

Let's look into this soon.
I am not a coder, but rather a sort of heavy user. I may come across challenges.

Best regards,

Roland

[kbwbe]

I may be on to something. Fixing the tolerances in the parts, turning the shells into solids and fusing the result gives something that passes Check Geometry without a peep. Not sure if this is a general solution yet, but it looks promising.

Hi wandererfan, thank you for your proposal. I think it is only a solution for very small assemblies of non complex parts. Fixing and fusing of all parts of an assembly takes a lot processor time. Think of a complex engine of a car. A second problem is that the fuse operation changes the number of geometric elements. This breaks the constraints due to the topogical naming issue. Also the color handling will break too.

As the link branch has been merged now, it could be a a solution to use links instead of shells within A2p. Or merging A2p with A4.

[easyw-fc]

instead of shells within A2p

in A2p there is an option to use solids instead of shells
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use-solids.png (46.96 KiB) Viewed 1164 times

[kbwbe]

in A2p there is an option to use solids instead of shells

It does not help up from second level assembly. Solid generation fails very often and shells are used as fall back.

P.S: Using Solid union slows down the assembly, breaks coloring and toponaming. As described before.

[easyw-fc]

It does not help up from second level assembly. Solid generation fails very often and shells are used as fall back.
P.S: Using Solid union slows down the assembly, breaks coloring and toponaming. As described before.

Yes, it could be, but it is the only way to get a Solid assembly result without issues.
I used this approach also on A2 wb, to assembly parts that I needed to export to STEP.

[wandererfan]

Hi wandererfan, thank you for your proposal. I think it is only a solution for very small assemblies of non complex parts. Fixing and fusing of all parts of an assembly takes a lot processor time. Think of a complex engine of a car. A second problem is that the fuse operation changes the number of geometric elements. This breaks the constraints due to the topogical naming issue. Also the color handling will break too.

I see this technique being used in TD (behind the scenes). It would be nice if A2P delivered "clean" assemblies, but it isn't essential.

The OCC HLR routines are much happier with valid shapes, so TD produces good views of massaged assemblies. And I'm not sure the topo-naming and constraint breaking aspects are relevant to producing a drawing, since TD is only interested in the end result, not how we got there.

HLR is slow anyway, so the extra processing may not be so noticeable.

[wandererfan]

I am not a coder, but rather a sort of heavy user. I may come across challenges.

If you want to experiment on your own, here are the 2 py routines I have been using in my experiments. Some times, fixToleranceAll.py is enough, sometimes you also need fixShellsAll.py.

Code: Select all

#!/usr/bin/env python
# -*- coding: utf-8 -*-

# fixToleranceAll.py
# fix tolerance of all shapes in assembly document

import FreeCAD
import Part

items = App.ActiveDocument.Objects

pfShapes = list()
for i in items:
    if i.isDerivedFrom("Part::Feature"):
        pfShapes.append(i.Shape)

for s in pfShapes:
    s.fixTolerance(0.001)

print("{} shapes fixed".format(len(pfShapes)))

Code: Select all

#!/usr/bin/env python
# -*- coding: utf-8 -*-

# fixShellsAll.py
# make solids from shells in assembly document

import FreeCAD
import Part

items = App.ActiveDocument.Objects

pfShapes = list()
for i in items:
    if i.isDerivedFrom("Part::Feature"):
        pfShapes.append(i.Shape)

newShapes = list()
for s in pfShapes:
    solids = list()
    for sl in s.Shells:
        sls = Part.makeSolid(sl)
        solids.append(sls)
    if len(solids) == 1:
        newShapes.append(solids[0])
    elif len(solids) > 1: 
        singleSolid = solids[0].generalFuse(solids[1:], 0.001)
        newShapes.append(singleSolid)

for ns in newShapes:
    if type(ns) is list:
        Part.show(ns[0])
    else:
        Part.show(ns)

print("newShapes: {}".format(len(newShapes)))

[Roland]

Thanks for your codes, Wanderfan.
May come in helpful.

Greetz

Roland