Membrane elements

FabioC

Dear users,

 

I am running a modal analysis in Optistruct for a simple 2D plate in order to validate some Matlab scripts.

I use CQUAD4 elements (PSHELL 2D property) in HM.

Results from OS are consistent if I compare them with a 6-DOF per node element in Matlab.

Now, I would like to compare the same case for membrane elements (2-DOF per node) but I am not able to find a way to model a membrane in HM.

Any suggestion about a different element?

 

Thank you

Regards

Fabio

Simon Križnik

Hi,

https://community.altair.com/community?id=community_question&sys_id=9c96007a1b2bd0908017dc61ec4bcba4

 

for Optistruct the following behavior are valid:

 

- To model a membrane plate, use only MID1

- To model a plate with bending stiffness only, use only MID2

- For bending with transverse shear flexibility, use MID2 and MID3

- Use MID3 to include an extra shear term in the element stiffness calculations (i.e. includes transverse shear flexibility).

- For a solid homogeneous plate, MID1, MID2, and MID3 should reference the same material ID

- MID4: The MID4 field (bending and membrane deformation coupling) should be defined only if the element’s cross section is unsymmetric. Default is blank = symmetric cross section.

 

(Note: Mass is not calculated if MID1 is blank.)

 

In summary, the results of leaving an MID field blank are:
●MID1: No membrane or coupling stiffness or Mass
●MID2: No bending, coupling, or transverse shear stiffness
●MID3: No transverse shear flexibility
●MID4: No bending-membrane coupling

 

 

The standard for typical shells (thickness about 1/15 of size) is to use the same ID for MID1, MID2 and MID3.

 

 

To define a membrane, please leave MID2 and MID3 blank on the PSHELL property, or use PARAM,SHL2MEM.