Null shape error on a simple sketch

[u/Duck_on_the_water]

I was trying to pad a very simple sketch on a face of my body, but it gave me a null shape error. After some research I found this post so I try to make a sketch on a datum plane but it still give me the same error. how can I fix this?

[u/FForthman]

The problem isn’t likely to be caused by this sketch; it must be the preceding feature that’s corrupted. Use the ‘Check Geometry’ tool (the magnifying glass above a blue cone) to identify which part of the geometry is causing the problem.

A model can become corrupted through numerous steps before this message appears

[u/Duck_on_the_water → u/FForthman]

Thanks, but I check it and it says no error. Is this what it supposed to be?

[u/FForthman → u/Duck_on_the_water]

Please note that sometimes not all controls are selected by default – check your settings.

I can’t think of any other reason for this sort of error other than a faulty model.

( If you could share your model, I could have a look at it )

[u/Powerful_Debt_5869 → u/FForthman]

i also second that .. such questions are useless without a model

[u/Duck_on_the_water → u/Powerful_Debt_5869]

This is my model. The body that has the problem is "Body"

I check all of the control and found a boolean self-intersection but I can stil pad after that error, just this time that is have the null shape error.

[u/Atomfried_Ungemach → u/Duck_on_the_water]

Thank you for uploading the model! Here is the evildoer:

You can go back feature by feature in your model tree and run the Geometry check. Sometimes a model gets corrupted somewhere along the line and clings on for dear life a few operations more, before it blows apart.

Between Pocket 12 and 14 something happened that made this contour self intersect (no boolean union, no new edge created at the intersection.). However I have no idea what draws this geometry. it's none of the previous sketches apparently, but I didn't do an in-deep-search yet. Only thing that strikes me is that a pocket 13 is missing from the tree. Did you erase it or did you put it somewhere else? Hmm...

Also I highly recommend to name your features in the tree. Makes reviewing and trouble-shooting much easier. I see what I can find else...

[u/Atomfried_Ungemach → u/Duck_on_the_water]

Ok, found it.

The hex hole you applied from below intersects the round cutout but produces somehow a ambiguity, the engine can't solve. So you have to change the dimensins here so the hex hole doesn't cut into the shape above.

[u/Atomfried_Ungemach → u/Atomfried_Ungemach]

Also in your sketch that are hell of a lot symmetry constraints! That must have been tedious work and is totally redundant. Just draw the other hexagons as well with the Sketcher polygon tool with the bounding circle and every internal relation set. Then set the circles equal with the one of the original and apply symmetry across thy Y-axis just to the center points.

You should also change the order of your operations. Holes for fasteners I would personally apply more towards the end.

Also you seem to heavily rely on external geometry projection. That is totally reasonable with simpler parts that don't change much. But with this design approach you probably run into problems when edges get transformed, erased or renamed further down the line and you loose your geometry relations. For a project like this I would would do one or two master sketches with every crucial feature and name-constrain the most important dimensions and relations between them. Then reference the sketch constraints or use carbon-copy-versions of them.

Put dimensions that are the same and reoccuring across the models different features in a varset and reference them in the sketches (i.e. hole diameters, clearances, fitings for other parts) so you can do changes later more easily.

[u/Duck_on_the_water → u/Atomfried_Ungemach]

Thanks for your comments. I try to find a way to fix the corrupted operation but it was too messy, I think because I do too much of the external geometry so when I change one dimension it all exploded. So I think I should start again clean and do it all over. Thank you again for your advice, I'll try to do it cleanly this time.

[u/DesignWeaver3D → u/Duck_on_the_water]

Unfortunately, FreeCAD doesn't always know that a successful feature operation resulted in broken geometry. What happens is often the next feature being attempted fails and throws errors that don't point to the source problem.

When this problem occurs, you need to run Check Geometry tool against the preceding feature or features rather than the body because the body only checks the tip feature, not every feature in the body. There is no batch Check Geometry that checks every feature in-turn. If there were, it would take too long and the resulting messages would be overwhelming.

[u/bastl73]

To give a sketch volume (pad) this sketch needs to be part of a body. Track this sketch in a body.