How to properly knit two shell parts?

[Anonymous]

Hi everyone !

Very simple assembly model consists two shell parts (pls. see Fig1.png).

A linear static analysis is performed under the surface load applied to Part 2 (2.ipt). I got results shown in Fig2.png. I think these two parts are not propery conneted.

I'd like to know that how to knit two shell (surface model) parts.  Test model's zip file is attached hear.

Best regards,
Akihiro

[John_Holtz]

Hi @Anonymous

You have a very strange situation. Although you applied the constraints to the 4 outside edges (as shown in your Fig1.png), the corresponding inside edges received constraints, too. This is hard to see in InCAD because it does not show the real constraints, just "glyphs" of what the user wants.

Instead of constraining all 4 edges, try constraining the two shorter edges and run the analysis. This will show how the two shorter inner edges are prevented from moving, too. The free outer edges and corresponding inner edges will deform.

I will try to figure out what is wrong with the model. Did you create this model? Or is it an imported model? It should not matter, but I am wondering if it is related.

Also, note that the thickness is entered as 5000 mm. Based on the size of the model, the thickness is wrong.

[Anonymous]

Hi, John

This model was imported from STEP file. And thickness is corrected to 5mm. Fig3 clearly shows that the fixed outer edges and corresponding inner edges do not deform. This result has been mentioned by you.

Therefore I pruned nodes which are involved inner edges (by Nastran file view shown in Fig4).

Run the analysis for a hand-modified Nastran input file, and its results is shown in Fig5.

This result is appropriate deformation mode, I think.

It seems that the constraint conditions on the edges are not properly created in the Nastran input file. The model imported from STEP file influences this results?

Best regards,

Akihiro

[martin_madaj]

Hi John,
it seems that this is a similar issue that I came across a few weeks ago. I reported this to ADSK support and consequently it was sent to the development team.

Best regards,

Martin M.

[John_Holtz · Accepted solution]

Thank you Martin ( @martin_madaj ). I have located the bug report, so I will add Akihiro to the report too.

For everyone's benefit, Martin discovered that the wrong constraints are appearing when using "Continuous" meshing to connect the shell parts together. If continuous meshing is not used, then the constraints are okay.

• I am guessing that this is a problem with shell elements. Has anyone seen this type of problem with a solid model?
• Instead of using "Continuous" meshing to connect the parts, you can use "Contacts > Manual" to define "Edge to surface" bonded contact.

Akihiro ( @Anonymous )

Another customer reported a problem yesterday related to the thickness of shell elements. He enters a thickness of 10 mm, but if he edits the shell elements again, the thickness is 10000 mm! This may be the same reason that I saw your model has a thickness entry of 5000 mm instead of 5 mm. I have not investigated this problem yet, but my suspicion is that there is a problem between the units used for the plate thickness versus the units used for the CAD model. Keep a careful watch for this!

[Anonymous]

Hi John,

I confirmed your workaround. "Continuous" meshing check-box is unchecked, and Surface-Edge contact settings was done.

Run the analysis, there are a lot of T2318 warnings (Please see attached here), however, the result is appropriate deformation. I will use this workaround.

And also I will carefully check an undesired unit and/or thickness conversion .