Converting solid parts to shell parts

[Marco]

Good afternoon All,

I’m performing a simulation of a skid, made by solid parts (coming from CAD).

My question is regarding the option inside PPM about “convert”:

This command convert all the solid part into shell, but I don’t understand witch kind of surface the sw take into consideration (outer - mid - inner); because I tried to push the button but (apart from the tree bar) the solid remain phisically the same.

Is there anybody that can answer this question? Because I looked in the forum but I wasn’t able to find this specific topic.

Thank you in advace.

WBR

Marco

Studio_telaio_intero_modificato.pmx (5.1 MB)

[Matej]

The conversion uses all visible/ouside surfaces of a solid to create the shell. And takes a closed shell to create a body. In these conversions, the geometry does not change.

[Marco]

Thank you for the clarification.

So when I have to apply the thickness of the single shell part I have to consider this from outside to inside, am I right?

[FEAnalyst]

In most cases, it’s not what you want for shell modeling and you should extract the midsurface (in CAD software) instead. See this: Simulation of Planar Magnetic membranes; tweeter and midrange - #17 by FEAnalyst

Let me know if you want instructions how to do it in FreeCAD.

[Marco]

So the better way is to extract, from CAD sw, the mid surface of every single part and then load the IGES file inside PPM, am I right?

[FEAnalyst]

Yes, extract midsurfaces (or only top or bottom surfaces, but then you should define offset for shell section in PrePoMax) from each part in CAD software, export to STEP and import to PrePoMax.

[Marco]

I’ve extracted from CAD file the mid surface of every single pieces and import it in PPM.
Last clarification: why there is this simbol “!” on that parts?

WBR

Marco F.

Studio_telaio_intero_modificato.pmx (4.9 MB)

[FEAnalyst]

@Marco

Last clarification: why there is this simbol “!” on that parts?

See this from the announcement about v3.0.0 RC1 version:

@Matej

Parts with small features

A CAD part now shows an icon with an orange exclamation mark in the model tree if it has an edge shorter than 1/1000 of the part’s bounding box diagonal, or a face narrower than that (a thin strip or sliver). Such features force very small elements around them, which slows meshing and spoils the element quality. They are often left behind by imported CAD, splitting or defeaturing. When you select the part, its small edges and their vertices are highlighted. Remove them with Geometry → CAD Part → Repair (remove small faces and edges, fuse faces, join edges), using Preview to see what will be removed. Other options are Fuse Faces and Defeature Solid.

[Marco]

thank you very much for your clarification

I did the correct simulation (I hope so)

Studio_telaio_intero_modificato.zip (7.8 MB)

WBR

Marco F.

[FEAnalyst]

You have many tie constraints, some overlapping and potentially causing overconstraints, leading to errors:

You may need to merge or remove some of them. Try to limit tie constraints to minimum regions.

Also, this part seems disconnected:

Run a frequency analysis to see which connections don’t work as expected.

[Marco]

Thank you for your explaination. Do you think that could be better to manually detect the tie contact between the parts (instead of automatically detection)?

[FEAnalyst]

@Marco

Do you think that could be better to manually detect the tie contact between the parts (instead of automatically detection)?

Automatic detection work really well and tries to merge redundant ties, but of course, it may not be able to properly resolve all cases when there are multiple parts connecting in the same region. Then you can always correct it manually - remove redundant constraints, merge them or swap master/slave assignments where necessary.

[Marco]

Following your suggestion I tried to match manually the Tie contact (with less numbers of items instead automatically check). Now seems to work properly

Studio_telaio_intero_modificato.zip (7.8 MB)

Thank you again

Marco F.

[FEAnalyst]

Yeah, it seems to be properly connected now:

Of course, you may still need to have a closer look at the joints to see if they are connected at the whole perimeter without any gaps or mesh distortions.

[Marco]

Due to the fact that all the parts are welded together, did you mean that I could use the Joint Constraint instead of Tie Constrained?

[FEAnalyst]

Not necessarily, these Joints are new features based on rigid body or coupling constraints and because of known CalculiX limitations, they may not work well with shells (unless they are manually extruded to solids). They could lead to overconstraints as well, but you can try them if you want, possibly on a small segment of the model first.

Tie constraints should suffice, but what I meant is that you may need to examine each connection between parts to see if these constraints work as expected. Modal analysis is a good way to facilitate such checks, but visual inspection may help too.