As I’ve mentioned before, there are 4 algorithms for hex meshing, but they have quite strict requirements for the geometry so it often needs special preparation. Those requirements are mentioned in the manual and here: Summary of Gmsh hex meshing rules
Of course, if you share a shell model exported to Abaqus .inp, I can check it in Abaqus too.
Okay, here is the shell model:
In this one, I had to add adjust=no to tie constraints because they were distorting the mesh and causing errors. I also had to reduce their position tolerance to 10 because they were acting too widely, eliminating DOFs of the bottom edges used for BCs.
Anyway, the result I got is 8.5965 (first eigenvalue).
Interesting. I am redoing the simulation using hex elements on the shell. We will see if any accuracy improvement is made on the solid element model for calculix.
Hi,
What units are this:?
*Density
7.29865865E-004
Those are imperial units
7.29865865×10−4 lb/in3≈20.2 kg/m3 ?¿?
Should be arround 7850 Kg/m3.
Something like this:
I avoid imperial units so I asked the OP to check if they are correct in the model. Still, density shouldn’t matter here anymore.
Well, the imperial units for density are indeed weird. But they were fixed in PrePoMax quite some time ago: Density to Mass Conversion (Modal Analysis)
Hello that is from ASME. That is their example calculating allowable load with their design factor of 2.5 for cylindrical shells.
Yeah, it’s taken straight from “PTB-3-2013. ASME Section VIII - Division 2 Example Problem Manual”.
Oh.,. I see. It’s introducing one unit of the external pressure as preload for the buckle step to find some “imperfection”.Then its is added again at the end to find the Buckling Load. That’s cool but naming that “Dead load” without more context is confusing. I would have assumed gravity loads as the “dead load”. I will try to find the full text.
Is this solid only one layer element?
Yes, I did it both by solid and by shell elements.
I did it with hex elements and get around 10.9. It is a slight improvement, but barring a model setup issue, I don’t think it will match the abaqus output.
Better try more layers.
Can you elaborate on what you mean?
For more context, I found another simulation record of this being done in MSC Nastran and their results were around 10.9. So Calculix is tracking with Ansys and MSC Nastran (NOT inventor Nastran to be clear).
So there is some fundamental difference between these and Abaqus I believe. Realistically the results are not too far apart when you consider the use of linear buckling simulations and the applicable safety factors applied to eigen values. If things were close to buckling, a non linear simulation would be required.
