Local buckling dissapears in tetra-mesh?

Guillermo

Hello.

While I was working with an internal-pressure vessel, I found a significant difference in the results between tetrahedral and hexahedral mesh. It does not matter what solver is used.

Simplifying the issue: I modeled a cylinder, fixed one of the planar faces, applied an internal pressure of 0.29 MPa. Stainless steel (elastic modulus = 1.9E11 Pa, 0.29 Poisson's ratio). The only difference is the mesh.

I guess that the realistic solution is the wavy-shape obtained with the hexahedral mesh (which is obtained when symmetry planes are applied, too). I consider the round shape obtained with the tetrahedral mesh an "unstable shape": any disturbance will cause the transition to the wavy-shape.

I thougth that, in general, tetra-meshing is better to capture local complex phenomena, for example in turbulet flow in CFX. So, I did not expect that hexa-mesh would work better in these "local buckling" phenomena.

1. Am I right? Should the hexa-mesh result be considered as the "right solution"?

2. Why does the tetra-mesh generate a symmetric deformation? What should we do to avoid this unrealstic result?

The hexa-mesh obtained a 15% greater von Misses tension, and a 34% greater maximum deformation. These are significant discrepancies.

Guillermo

I used solid elements

Victor

The number one rule in FEA is that it's wrong until you estimate the size of the error. The basic reliable way to that is with a mesh convergence study. Here, you only have a single element in the thickness direction which is probably not enough for the tet mesh.

Tet is generally worse than hex but they're both just as good with enough mesh refinement.

I think the symmetric shape is qualitatively correct here because a symmetric structure with symmetric loading should always produce a symmetric deformation in linear static analysis. It won't find buckling. I don't know what caused that wavy shape but I'll look into it...

... It turns out the hex mesh has a slightly irregular shape while the tet mesh is much more uniform. See the attached picture using Node coordinates in cylindrical mode. After I reset the inside and outside surfaces to constant radius (select the surface, then change to Select nodes mode, then right click one of them, set Cylindrical (Z axis), and enter the radius), the hex mesh also had a symmetric deformed shape. So it does look like it's very sensitive to imperfections. In real life, however, that might not be the case since stress stiffening would probably stabilize it. That too is something not modeled in a linear analysis, but is in non-linear analysis.

Guillermo

Thank you, Victor.

I know that buckling can appear when a cylindrical shell is subjected to external pressure. There is much literature on this topic (Rathinam et al. 2015, Teng et al. 2006, for instance). Although I do not find papers on buckling caused by internal pressure, I thougth that this really happens because of fixing the planar faces. The freedom that the wall has for expanding out is not uniform due to the fixed faces, which can cause buckling. I believe that the non-symmetries (or unbalances) in the mesh and in the solver algorithms could induce the buckling.

So, I have no clear that:
— This is buckling
— Why does it appear in linear static
— Why does only hex-mesh (with imperfections) capture it

I am trying to carry out a buckling analisys. From the information provided in the manual of Mecway, I am not sure it that is possible: cylinder wall with both end faces fixed, subjected to internal pressure.

Victor

Yes, you can use imperfections to cause buckling in FEA, but with nonlinear analysis, not with linear.

Perhaps you're looking for wrinkling like this?

- No, this isn't buckling because linear static analysis can't do that. Displacements are proportional to forces (linear) which isn't true for buckling.
- I was surprised at this too. Maybe the thin wall makes it more sensitive to imperfections.
- A tet mesh with the same imperfections also captures it. See attached picture. I used Mesh tools -> Automesh 3D to convert the structured hex mesh to an unstructured tet mesh.

I tried nonlinear analysis (simply change the analysis type to Nonlinear Static 3D) and the wavey shape is still there. However, at a higher pressure (20 MPa), it evens out and becomes more uniform.

Two ways to find buckling:
A ) Linear buckling analysis (Buckling 3D). This is a quick way to start but can't capture all types of buckling. I don't think it would work in this case and it didn't when I tried it.
B ) Nonlinear analysis with Quasi-static turned on, some time steps, and the load ramped. Also give it an initial imperfection such as this shape, an extra force, or use the deformed shape from linear buckling analysis (Mesh tools -> Transfer displacements from solution). Preferably use the CCX solver for nonlinear. This is the most capable way to do it and I expect it would find any buckling or wrinkling if it exists.

Guillermo

I have the impression that that wrinkling corresponds to Internal pressure + Axial compression.

Anyway, your last answer clarifies better the problem to me. Thanks