Validating simulation

[Sasa]

hello, i’m making a very simple simulation about frequency step (nb of steps 10) on a cylindrical plate to validate analytical and simulation solutions.

this is a shell part. i’m comparing S6 and C3D15 meshes

S6: normal meshing parameters, shell thickness specifies in shell section assignment (1mm)

C3D15: meshed using thickened shell mesh, thickness 1mm, layers 4 (as done in a validating analysis, i know its a different problem, but still - https://www.dlubal.com/es/webfile/000112/2200161/0109-natural-vibrations-of-circular-plate.pdf?hash=a990017082e276e17197ae492c10d4863d9021d1&srsltid=AfmBOopQJAy7wPajM8pubqm6UzfnP2JINE3LPxiGGyo0OraSJR-hv_E2)

but the results i’m getting vary a lot between my two models, but don’t in the validating simualtion i’m using as a refernce. is there sth wrong with my simulation or what?

[Paul18fr]

maybe be can you first share you model?

[synt]

it’s a case of circular plate with fixed edge; the boundary condition is not properly set probably.

*edited

i try to reproduce the problems, and it seems CalculiX need to compared mode shape precisely.

RFem –> CalculiX

1 –> 1

2 –> 2 & 3

3 –> 4 & 5

4 –> 6

5 –> 7 & 8

6 –> 9

CalculiX solid element models with layered require a greater number of modes setting to capture all possible shapes.

[FEAnalyst]

Did you fix the side face or edge of the solid plate ? Did you try with quad/hexa elements too and with some refinement in the plane of the plate as well as in the thickness direction ? Are you using PaStiX or Pardiso solver ? The former may still have some issues witg frequency analyses, the latter is the most reliable.

[synt]

tested for quadratic wedge also, solver is Spooles.

[FEAnalyst]

Does it agree reasonably well with the analytical solution ? The mesh is rather coarse, they use element size of 10 mm in the reference document.

[synt]

overall is identical with references, refined the mesh match closely with RFem results. I’m only doing quick and raw checking with coarser previously.

[Sasa]

okay, so i did some improvements, like fixing the whole side surface (the 1mm thick one) and changing to a full-quad mesh, but now my results are extremly high (the fisrt mode at 48Hz). doesn’t really matter if i fix the side surface or block all the U1,2,3,R1,R2,R3 to zero. may i ask how you did that?

[FEAnalyst]

@Sasa

now my results are extremly high (the fisrt mode at 48Hz)

This means that the stiffness of your model got increased significantly. Restore the previous mesh and you should see it’s due to overstiffening BCs (it’s usually better to make one change at a time). Keep in mind that nodes of solid elements have no rotational DOFs while shell elements do have them (although one called drilling DOF requires special handling).

[Sasa]

so i got back to the working shell part and changed it to solid with thicken mesh (1mm, 4 layers) and changed to BCs on the edge surface to fixed U1,U2,U3 and the rotational unconstrained, which got my model down to 23,5 Hz (at least the 1st mode). that is all i changed. there has to be sth i’m missing though?

[Paul18fr]

here is the model using hex elements (note for such thin plate/disk, shell elements remains the best choice)

disk_vib.pmx (1.1 MB)

[Sasa]

thank you very much! i just changed the mesh on your part (to 10mm for it to match the assignment) and the results dropped to around 7,8 Hz on the first mode and 15,5 Hz on the second. i know the shell parts are better, that was what i was trying to prove. anyway, i think this is were i will end it. thank you very much for all your help!