I’m going further based on this previous post (*) as I want to apply LBA/MNA or GMNA method to compare results with DIN 18800-4 or EN 1993-1-6 bearing capacity.

Eigen modes ok, eigen shapes symmetric, Maximum Misses exceeds 340Mpa (maybe some refinement is needed) but …. equivalent plastic strains is way below .3 on fully plastic areas.

¿Am I maybe reading wrong the results in Prepomax?. ¿Does it happen the same to someone else?

I’m using S4 elements . ¿Is it suitable to capture plasticity properly.?

Can you share the .pmx file ? PE is equivalent plastic strain so it should be what you are looking for. Perhaps that approach with layered shell mentioned before would help.

I prefer not to post before solving the discrepancy.

¿Do you mean laminated shell? ¿To add more integration points but keeping the isotropic nature?

*SHELL SECTION,ELSET=EALL,COMPOSITE

0.001,Material1,1

0.001,Material2,2

I would need S8 to do that. ¿Is that worth?. I can go directly to S8 but I would say Xyont has already discard that option. He ended up with solids ¿isn’t it.?

My file is based on tutorial but with BC as shown in the file I posted. I changed from S8 to S4 as you. Is much faster . You should be experiencing the same discrepancy and PEE below 0.3 on plastic areas. I did not pay attention to stresses until now.

Right. I’m using free free BC n1. My imperfection pattern is much symmetric that yours. That’s why shell buckle symmetrically. I’m using the pattern shown on my pictures.

I don’t personally think this Eigenproblem is properly solved but didn’t pay to much attention as we use it as pattern for imperfections. Real life imperfections are not symmetric like mine so …Seems completely valid approach.

I think the purpose is to capture the thru the thickness behavior after the 3D expansion of the layered elements…probably 3 or 4 layers are enough (tbc).

I’m working on these analysis and later i want also to try cylindrical shell under axial compression,
but for me i’m fighting with these simple problem using ccx.
I’m very interested in your approach and your results,
so i can reproduce with a simple plate your analysis.
thnx in advance

¿Could you show BC,s or better, the reference document where this comes from?

¿Is Poisson’s Ratio somewhere?. It affects if BC are hard constrained, and you need it also for computing G in case you want to try the layered approach.

¿Don’t you think this deserves its own “NEW post”? . We will be mixing with cylindrical shell.

Considering simply supported , Poisson’s Ratio 0.3 and Tangent Modulus E/100 for plastic analysis my results are:

RESULTS

REFERENCE

RESULTS

REFERENCE

Methode

sx,Rd [N/mm2]

sx,Rd [N/mm2]

w [mm]

w [mm]

EN 1993-1-5

173

LA

355.1

355

LAB

112.7

112

MNA

355.0

355.0

GNIA (e0=5mm)

??

143

??

21

GMNIA (e0=5mm)

172

176

29.4

31

LA, LBA and MNA has been done with 256 Elements S8.

GMNIA has GNIA has been done with 4096 solid elements C3D20. 4 layers per thickness.

GNIA is not finished. I’m not sure to have solve it properly yet. Maybe someone can help. I’m not sure how to identify the point of interest. I have done a displacement control test to see if reactions help me to determine the solution but there is not a clear knockdown or slope change . I think I should reduce the imperfection value from 5 mm to 2.5mm.
Here ther is a screenshop of my BC.

Hi, @Disla
the BC are hinged
Poisson’s Ratio is 0.3
Predeformation is first buckling mode with e = 5 mm
plasticity is bilinear with tangent modulus = 0
*PLASTIC
235,0

I see you 're very fast, i think if these works with plate buckling,
the same (step and analysis) should work with shell buckling, all steps are equal or simular.

your boundary in the plate are essential for your results? for symmetry?

I gess you mean (355,0)
Perfec plasticity can lead to convergence problems. To avoid going to more sofisticated stress strain curves like the ones shown in the general rules , I’m using E/100=2.1 GPa. (Reference DNV-RP-C208 Non-linear FE analysis Methods . Figure 5-6 )

It is not about symmetry.

Hinged doesn’t seem compatible with the picture. It shows two loads applied simultaneously on each side. As hinged doesn’t allow translation in the horizontal plane that wouldn’t make sense.
Hinged is intended for vertical loads on top of the plate as it resist both the vertical and horizontal reaction forces.

I have applied simply supported/roller.

EDIT: Another detail. Constraining displacements on both sides of a plate, beam or whatever introduces additional stress due to the Poisson’s ratio effect when it tries to accommodate the volume change.

Hello Disla,
at first thank you for your interest and engament,
I appreciate it very much.
To have the simply supported roller will not be purposeful for me.
these will not be working if you have plate buckling of shearing stress,
or if you have both, pressure and shear stress!?
you can apply node or point boundaries in the corner,
two could be enough, one with fixed in x and y and one only in y
these could be a possibilty.
I need some time to reproduce your procedure.
I do not have time at the moment.
But I will definitely come back on these issue.

i’m using S6 shell element just for quick review the analysis models. right, it seems required layering to capture plasticity better as i mention before.

at another post replied i’m also done with solid element to compared the clamping condition of model with shell element.

i did not further study the problem issued by @Calc_em of rigid body and layered shell element connectivity but has experienced problem with nonlinear spring, so i’m only guess probably the same causes.