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
**
I am enclosing a word file that has the images for the stress analysis of a 3D shell model subjected to internal pressure. The model is a composite of several shells. I made the composite and meshed the composite. The project runs but I believe that I am getting some wrong results just at the intersection line of two shells, as the outer nodes created by Prepomax/Calculix appear to be getting disconnected. Is there a command to impose a Knot condition to prevent this behavior. Comments and suggestions are really appreciated.
- List item
2nd order quad results.zip (602.4 KB)
It would be better to share the images directly here but never mind. Can’t you share the .pmx file too ?
One may expect some spurious effects right at the edge between the shell faces. Knots are described in detail in the CalculiX User’s Manual (section 6.2.14. Eight-node shell element (S8 and S8R), page 105): https://www.dhondt.de/ccx_2.21.pdf
The site has a limit of 8 MB. What can I do to send it to you?
Upload it to some hosting website and paste the link here.
Here you go! Thanks!
Mac-model-4-26-24-half-linear-quad-2nd-order.pmx
Mac-model-4-26-24-half.pmx
Frequency analysis indeed shows some separation on one side:
It might be a matter of how this “Compound” surface part was created in CAD software. Maybe not all the faces were connected properly by a boolean operation due to some inaccuracies, for instance.
I saw that. I corrected the issue. But the issue that worries me is the fact that the outer surface nodes at the junction between the two shells is opening and resulting in incorrect stresses.
The compound was created by loading up the shell sections and suing Prepomax to create the compound. In the meshing parameters I used the “Merge compound Parts : Yes” option.
It looks, based on the images that I sent before that when the shell is converted into a 3D solid element, the nodes in the outer surface are not fused together as one.
I can try and join the surfaces again and rerun it, but the issue remains in the section with the highest stresses at the joint between the two surfaces.
Separation is occurring at the intersection of a cylindrical section and a conical section.
Thanks!
When the angle between elements is greater than 20 degrees, they’re expanded into solids with separate nodes and connected by MPCs. That’s normal and not a problem on its own. You have that angle between the cylinder and cone.
What’s incorrect about the stress? It will be different because it’s not averaged.
1 Like
You can add a fillet to get rid of such “cracks”.
I will try that.
I tried restricting the opening by adding zero rotations at the line joining the two sections but did not help.
Thanks all for your feedback!
Great application Matej!
1 Like
Why would you wan to get rid of them? I’m not convinced there’s any problem here. Stress is high because the crease is a stress concentration. Yea, you could make that more accurate with a fillet that’s the actual bend radius, but if that’s not well known, it’ll just disguise the error.
I meant that now, as you said, the stress at such cracks is not being averaged. That makes a difference compared to the other points, where the stress is averaged. So, we are looking at averaged and unaveraged stresses at the same time. The fillet will, at least, introduce averaging.