I’m testing a simple 3d cantilever model.
The analytical results are max displacement 22.57um and max VM stress 10.7MPa.
With PrePoMax I tried different mesh refinements obtaining the results below.
The u_max value is quite stable but a bit higher, the VM stress value increases as the mesh size decreases.
I tried also with GetDP and I got the same instability of the max stress.
How can I get more stable values?
That’s how stress concentrations work in FEA. You should run mesh convergence studies until the maximum stress doesn’t increase significantly anymore. Unless you encounter a stress singularity where the stress doesn’t stop increasing. Fixed constraint doesn’t accurately represent the real-life problem. There are several articles on this topic but those can be particularly interesting in this case:
When comparing with analytical solutions do not forget many times Poisson Ratio effect is not taken into consideration on those formulas.
Looking at your Stress distribution, you are probably considering Poisson and the fixed support is inducing peak stresses as Calc_em explained.
If you want to compare with the closed form look for BC that deliver stress profiles like this, with a well-defined neutral fiber down to the base and nearly non discontinuity with the sides.
There are no actual periodic BCs in PrePoMax (and defining them in CalculiX input file is possible but not easy) but you don’t need such advanced BCs. You can just use symmetry in the form of translation being block in the normal direction.
With suitable models, anlalytic results can also be recalculated in FEM.
I therefore used the “SAE keyhole benchmark” and recalculated it with Calculix in FreeCAD. And then the stress results also come closer as the mesh becomes finer.
In FreeCAD we get a maximum stress in X direction of 34.1 MPa and a maximum P1 stress of 34.3 MPa. And that is very close to the estimated analytical results of 33.6 MPa.
That is an excellent validation example to work with. I used it recently to get a better understanding of ccx + the new stress linearization tool in Mecway.
Agreement was excellent.
Do you mean symmetry on the clamped surface? u_x = 0?
or uz=0 on the beam sides? In this case, It would be a plane strain condition that is not correct I think.
Slab should be able to freely slide in the yz supporting plane so Poisson has minimum effect on that area. Poisson should be zero as you want to compare with the ideal analitycal solution.
your solution works if the mesh is structured and the edges coincide with the position you need.
For tetra mesh, I have to draw additional support lines and nodes, right?
Can you suggest any reference books that deal with basic/advanced structural problems to check with FEA?
Singular stresses can occur on different occasions. Mainly on fixed (rigid) supports, sharp internal corners, and under concentrated forces. The reason for their appearance is idealization in the modeling approach.
For fixed supports, the alternative is a spring support. You can use fixed support to evaluate displacements and then replace the fixed support with soft spring support to evaluate stresses. Of course, this approach is limited to linear analysis.
NAFEMS Finite Element Benchmarks is the right way to go.
Different FE software’s rely on them to test their solvers. That means you can go to those software webpages to find them and avoid paying for the Nafems original.
Google this “esrd Benchmarks-Guide-Standard-NAFEMS” or “NX Nastran 11 Verification Manual” for example. They are based on Nafems.
DNV Standards are excellent too. Clear, well explained and typically have some examples to test your understanding at the end.
In fact, using their examples as validation is part of DNV’s methodology. “calibration of analysis methodology”
That makes all your work of validation a training but also a tool to “calibrate” your skills, methodology, solver performance,….
Abaqus itself has a lot of examples. Google “Abaqus Verification Manual”
It has the advantage that you can download the inp to see how they finally do it. From my point of view the problems are not so well stated and can be difficult to set up your model in exactly the same way. Also because Abaqus has additional features and elements .
Don’t get obsessed with accuracy. If you get below 3%-4% agreement move on to the next. At the beginning it can be very frustrating. You need time and can be very tricky to go down below 1% on those validations.
Abaqus has Benchmarks Manual and Example Problems Manual too, they can be better than Verification Manual which is focused on simple tests (often single-element tests) to verify various analysis features like material models and element types. And here’s a newer version of the Abaqus documentation (more recent ones require DS account): http://130.149.89.49:2080/v2016/index.html
