INVALID BODIES PREVENTING SECTIONING

[FreddyB]

Hi,

I have a model that has sectioned through the middle ok all the time i have been working on it. Now I can't as it fails, saying that it will produce invalid bodies.

I have been through the model from end to end and can't see anything with features occurring on or near the mid plane.

I cant section elsewhere as I need a section through the middle not near it. The question is - how do you find out where the problem is?

 

[CorBlimeyLimey]

This problem is often solved by offsetting the section line by .001" or even less.

 

[FreddyB]

Hi CBL,

I agree and have tried it. It usually works but even incrementally offsetting in both directions up to 0.5mm it was still reporting an issue. I have now got it to do it but with a greater offset than I would like. I have tried suppressing a number of parts and even opening them as component parts and sectioning along the same plane but the invalid bodies are refusing to step out and identify.

I just wish that when it says there is a problem (and SolidWorks knows what it is) SolidWorks would identify it!

 

[Updraft]

Freddy,

Are you sectioning by making a cut in the assembly or part files or are you sectioning in a drawing?

- - -Updraft

 

[FreddyB]

In an assembly.

 

[CorBlimeyLimey]

Do you get the same problem when creating the section in the drawing?

Try creating the section (in the assy) with all but one part suppressed and then, one by one, un-suppress the other parts.

 

[MFDO]

I’m encountering this problem frequently. I think if the section line meets a part tangently this happens. I reported this issue to our VAR and they asking for a sample. For this I’ve to keep screenshots/PDFs of all the last successful sectional drawings to provide proof which is not possible.

So what I do is try to move the section line slightly in a simple section In a multi section sketch, delete one line at a time and see or move one line at a time.

Sometimes redoing a section is the fastest than chasing behind to find the failing point.


Michael Fernando CSWP
Tool and Die Designer
SWX 2009 SP3.0 X64
PDMWorks 2009
Logopress3
FastForm Advance
FormatWorks

 

[mjcole]

Freddy,

If you are using an Extruded Assembly Cut try using Flip Side to cut option and see if that works.
I've found that for a single line sketch used for assembly cut SolidWorks will tell you which components could not be cut and they are listed as impossible and removed from the Selected Components to cut.

For the Tangency issue you can find parts tangent to section line with the errors. If you have tangency issues on multiple sides.

Find them using
Errors for standard cut
Errors for Flip side to cut Active

Easier Option Edit the Cut
Under Feaure Scope
Select
(*) All Components
check Propagate Feature to Parts

This Should create the cut and then flag the invalid parts which a Section can't be created from and show them as Errors in Feature Manager.

Another thing to consider. Try doing a 3D sketch in the assembly on the plane and use Intersection Curve to get the required curves.

Michael