How to create a big displacement model for membranes
Hello everyone!
I am working on a model with a diaphragm (membrane) that has to be deformed with the air pressure. It should have relatively high displacementes and strains. If someone can help me with the following questions I would appreciate it:
1- which kind of analysis should I choose?
2-How should I define the material properties and which propoerty should I use?
3-Is there any other difference to take into account that differentiates this analysis from a linear static one? (I have always worked with linear static)
Thanks a lot
Answers
-
I am going to share my actual fem model. It is very simple but I can not make it work.
1-It gives me the next problem:
*** See next message about line 9518 from file:
C:/Users/Usuario/Desktop/Respirador/30Diametro-saveas
'MATHE 1'
*** ERROR # 1000 *** in the input data:
Incorrect data in field # 3.2- Is it necessary to give thicknes in this type of analysis?
3- I am not sure about anything in the model. Probably there most thing are not well defined. If someone could revise it and give me feed back it would be perfect.
Thanks again!
0 -
Hi,
1. Use large displacement non-linear static (LGDISP NLSTAT) or transient analysis. Only explicit analysis (Radioss) can converge in case of wrinkling.
2. To get membrane behavior set MID2 and MID3 as BLANK. Membrane has no bending stiffness which can cause convergence difficulties. As a workaround, assign another material of negligible stiffness under MID2 & MID3.
3. Linear static cannot be used because of geometric non-linearity inherent to inflatable structures.
4. It is necessary to assign thickness in any type of analysis.
5. Material MATHE cannot be referenced by properties other than PSOLID/PLSOLID. Therefore it can not be used with shell elements.
6. For computational efficiency this model could employ quarter symmetry as load, BC and geometry are all symmetric.
0 -
As always, thank you very much Simon. Is there any page that you recommnend to learn to model in Hypermesh?
0 -
Glad to help.
I suggest you go through free Altair e-books and start with Practical Aspects of Finite Element Simulation.
You can also learn from learning and Certification program:
https://certification.altairuniversity.com/ > (Learn Modeling and Visualisation)
Check the following youtube channels:
AltairUniversity
Altair India Student Contest
ELEATION By Apoorv Bapat
If you are new to FEA I recommend Finite Element Analysis For Design Engineers by Paul M. Kurowski:
0 -
Thanks, I will begin to read them
One more question about the previous model. Is there a limit where the solution is not going to converge. For displacementes higher than 5 mm aprx the analysis stops with the following error:
*** ERROR # 4965 ***
Maximum number of time increment cutbacks reached,
analysis aborted.Is there a way to solve it?
0 -
This error is due to non-convergence (check the out file for details).
Increase the number of cutbacks allowed (NCUTS) in the load collector with NLADAPT card image and refer this load collector under NLADAPT subcase definition (loadstep).
However, there is a limit when implicit methods become computationally inefficient (buckling, wrinkling, unconstrained rigid body motion, large deformation, rupture, contact with friction,...). These cases can be solved by the explicit method.
0