I am modelling a pressure loaded 3D shell model. I believe that I have a decent mesh, but I get different Equivalent Mises stresses when I use second order element regardless of using triangles or quadrilaterals to build the mesh.
Any comments, general guidelines, or options to obtain more accurate results?
Help is much appreciated!
Thanks!
If you are using CalculiX shell elements, try using the Pardiso solver. It gives more consistent results for shells. And then you have to make a mesh convergence study to determine the appropriate mesh size.
Many thanks Matej,
I am using the Pardiso Solver.
I will record the results with the mesh convergence analysis.
The main issue is that using single quads or second order triangles or second order quads gives higher Mises stresses than using first order triangles.
Is it related to the way Calculix converts shells to solids when solving?
Different shell elements are expanded to different solids:
- I order tria —> I order wedge
- I order quad —> I order hex with incompatible modes
- II order tria —> II order wedge
- II order quad —> II order hex
This is assuming shells with full integration.
But element selection can be quite tricky and depends on a given problem. Not only first and second order elements perform very differently but there are also differences between tria and quad (or tetra and hexa) elements. Especially when it comes to stiffness but also stress field representation. That’s why, in addition to mesh converge studies, element type comparisons are important when solving new problems, especially in a new software.
first order wedge element is not recommended for use in mechanical analysis, it’s known not working well.
In fact, there are nice tips regarding element selection in the CalculiX User’s Manual (at the end of each solid element type description). For example: Six-node wedge element (C3D6 and F3D6)
C3D6 still can be used by fine mesh as documented, but seems not for S3 due to currently limitation in one layer trough thickness. Below my example, target value is about +830MPa and -520MPa
(192 elm.)
(768 elm)
(3072 elm.)
(12288 elm.)
(49152 elm.)
1 Like
CalculiX with US3 element shown better results.
** Sections ++++++++++++++++++++++++++++++++++++++++++++++++
**
*USER ELEMENT,TYPE=US3,NODES=3,INTEGRATION POINTS=3,MAXDOF=6
*USER SECTION,ELSET=Shell_part-1,MATERIAL=S235,CONSTANTS=1
1.0
**
** Field outputs +++++++++++++++++++++++++++++++++++++++++++
**
*Node file
RF, U
*El file
SNEG,SMID,SPOS
**
