Learning Forum

[ebogetti]

Hello,

I am looking to use *ELEMENT_SHELL_COMPOSITE for tow-steered composite modeling and ran a simple cantilever beam test to see if the element type was working as expected.  For my test case, the material is steel (E = 200 GPa), the dimensions are L = 100 mm, w = 10 mm, and h = 3 mm, and a 50 N load is applied the the nodes at the end.  Solving by hand, I expect to get a deflection of about 3.7 mm.  I modeled the problem using *ELEMENT_SHELL and got 3.67 mm.  With the working model, I transfered the elements from *ELEMENT_SHELL to *ELEMENT_SHELL_COMPOSITE and modeled it with 3 "steel plies" each 1 mm thick.  The transfer was done by using EleTol->ElmEdit->Composite, inserting 3 plies, and assigning the material and thickness (I did not touch the direction).  Running this gave a deflection of 4.13 mm.  Any idea how to fix the *ELEMENT_SHELL_COMPOSITE model?  I did try LAMSHT=1 in *CONTROL_SHELL, but the deflection did not change.

[Ram Gopisetti]

Hi Eli, 

How can you compare /expect the same results between two element formulations that are different in how the fields are calculated and work? 

I mean added integration points and differences in the location of them might cause some differences as you are observing here. 

Have a reading from the following slides for further information on elements. 

https://www.dynasupport.com/howtos/element/shell-formulations

Cheers, Ram 

 

 

[Jim Day]

Using *ELEMENT_SHELL_COMPOSITE, the through-thickness integration points are located at the center of each of layer.   *ELEMENT_SHELL uses Gaussian integration by default.   Integration point locations for Gaussian integration are tabulated under *SECTION_SHELL in the User's Manual.   I would expect Gaussian integration to be more accurate.   If you increase the number of layers in *ELEMENT_SHELL_COMPOSITE, I would expect the solution to improve.

[ebogetti]

 

Both models use the same element formulation, ELFORM 16.  I also checked the strain profiles through the thickness using eloutdet which was identical for both and gave the correct profiles.  Everything I checked has been relatively the same except for the deflection.  Most of what is discussed in the page you sent, I have also tried.  While hourglassing did not look like an issue, a college of mine recommended trying hourglass control anyway. That, LMSHT, and SHRF (we suspected maybe an increase in shear force may lead to more deflection) has not effected the delfection for SHELL_COMPOSITE.

Increasing the number of layers did improve the solution.  Just out of curiosity, is it possible to improve the solution in a different way without increasing the number of integration points?

 

[Jim Day]

To confirm, did you try *ELEMENT_SHELL_COMPOSITE with 6 layers of 0.5 mm each instead of 3 layers of 1.0 mm each, and the 6 layer run gave a more accurate deflection?   What was that deflection?

[ebogetti]

Yes, 6 layers of 0.5 mm each had a deflection of 3.78 mm.  Thank you very much.

[Jim Day]

Back to your question, I don't know how to make the integration rule, characterized by 3 through-thickness integration points of equal weight, any more accurate.   If you only have 3 plies in a composite, it's recommended you use at least 2 integration points per ply.