Just to give some background: I’m working on a compression test involving an auxetic structure. I ran the static analysis aiming for a displacement of 15 mm, but the simulation failed with results and stopped around 9–10 mm.
I have a couple of questions:
What does “Failed with Results” actually mean? My assumption is that the model failed before reaching the target displacement—please correct me if I’m wrong.
If I want the analysis to reach 15 mm displacement, what adjustments should I consider making?
Lastly, I haven’t explored explicit dynamic steps yet, and I’m still new to PrePoMax. Any recommendations or guidance on that would be greatly appreciated.
It just means that the analysis failed with some CalculiX error but partial results (for completed increments) are available. It’s a common sign of non-convergence. There can be many reasons but it’s particularly likely if you have contact in your model. However, other nonlinearities (geometric and material) can cause it too. You should check the existing results and look for any issues occurring before it fails to converge.
I for one would be interested to see the model. If confidential, a simplified model would do
Without having any more information than auxetic structure, are these not normally structures which move (parts which change position) to achieve a negative Poison ratio? Just wondering if a large deformation as yours can in general be simulated using a static approach as, by definition, the material is dynamic? … Might be wrong though but certainly interested in this topic!
I am currently working on the Arrowhead auxetic structure. As expected, this pattern exhibits a negative Poisson’s ratio (NPR), but my research is primarily focused on its energy absorption capabilities.
At the moment, I am running static simulations. However, my next step involves transitioning to dynamic simulations. I’m still a bit unsure about the appropriate ‘Step’ settings for dynamic analysis and would appreciate some guidance in that area.
Please find attached a screenshot of the model for your reference.
This appeared on the model, and I wasn’t entirely sure what it meant. I’m wondering if it might be the cause of the error that led to the simulation stopping midway through the calculation.
The displacement is shown as 1,500,000 mm. Clearly something going wrong in this area… and a lot of your other elements of neighbouring cells also seem severely distorted at the tips of your arrows. Have you used any boundary conditions on the sides (any symmetry boundary conditions applied)? Maybe upload your pmx file? There may be someone smarter than myself able to help … but also wondering how the mesh itself was created and how the arrow tip elements are joined? Within your structure, some arrow head elements (top pointy bit) also seem pultruding neighbouring structures. How are these elements joint?
Following your previous suggestion, I updated the model by enabling NLgeom (nonlinear geometry), as appropriate, and assigned additional contact pairs at the necessary surfaces.
I then re-ran the analysis, but it stopped midway again, showing the message “Failed with Results” and leaving me with the screen shown below.
I would use shell elements for that, you have quite coarse tetrahedral mesh with one element through thickness which is not good for bending. Check the linked tutorial.
Contact pairs will be needed only if it deforms so much that the arms touch each other. You could try with smaller prescribed displacement and without contact first.
I’ve treated the model as a solid structure. I’m not entirely sure about the specifics of the boundary conditions you’re referring to, but you can review them directly through the link to the model provided below.
The aim of my research is to compare the FEM results with the experimental compression results obtained in the lab using the same structure. The laboratory testing has already been completed I’m now focused on the FEM simulation. However, setting up the correct conditions has been quite challenging and, so far, has felt like a process of trial and error.
You can access the model via the link below. The goal is to simulate compression up to 15 mm displacement, in order to match the lab test conditions.
Set Recombine algorithm for Extrude mesh to get hex-dominated mesh. You should refine it too (if you don’t want to use shells for now). This should help it converge.
A large scale deformation under tension shows that the lateral distance of nodes on the BC grows . Model wan’t to expand under tension as expected. ¿Are those plates on top and bottom constraining that posibility in some way?
It depends on how they are supposed to be connected in real life. If they are manufactured (e.g. 3D printed or casted) as part of the auxetic structure, you can keep them merged/tied. But if they are components of the test rig and auxetic structure is only placed between them, frictional contact would be a better (but more difficult to converge) option.
The physical model was 3D printed with both plates attached to the auxetic structure as one.
In terms of progress, I have applied a hex-dominated mesh and observed some improvement in convergence. However, the analysis still fails before reaching the desired displacement.
Could this non-convergence be due to the mesh or boundary conditions? Or is it possible that the target displacement is simply too large for the current setup? How about in the Explict Dynamics Set up?
How does it behave before failing to converge ? Is the mesh getting distorted ? Is contact behaving unexpectedly ? Or maybe it reaches plastic plateau ?
Explicit dynamics procedure is rather underdeveloped in CalculiX - it has many issues and limitations and takes a lot of time to solve. I would rather avoid it if not absolutely necessary. Static step should be sufficient in this case, you just need to get the mesh and contact right.
I ran your file @SupharoekS , and the “no convergence” message seems to appear already from the first iteration. Not sure why yet, but there seems something wrong with your set-up from the very start.
The changes made were in the meshing. I reduced the max element size from 3mm to 1mm. (While playing with the mesh, there were sometimes issues with Jacobian’s at the arrow tip suggesting that this may be one of your issues?). I also changed the element type to Frontal-Delaunay-for-Quads and the recombination algorithm to Blossom-Full-Quad.
To get this running, I also turned off all Contact Pairs in an attempt to simplify your model.
But as said, not sure if our model is correct even though it ran without errors now…
One issue you may have, just an opinion and not sure I’m right, is that your element size was too coarse, especially for the arrow tips. I would suggest that you make use of the symmetries for your model (vertical symmetry). If the load introduction parts are just there for introducing loads and you are not interested in their actual behaviour, you may be able to change these too, e.g. single layer of very stiff material? Or remove entirely and apply fixed boundary conditions as needed to the arrow tips? This could then reduce the number of elements used in these beams.
Don’t have the solution but hope this is a starting point for you to get further.
I ran a similar setup using a finer mesh while keeping all the contact pairs intact. The model completed successfully, though it took approximately 9 hours to finish. I’m using an i9 14th Gen processor with 32 threads available, and I configured PrePoMax to utilise up to 25 processors and 128 GB of RAM.
I do have a question regarding the different solvers available in PrePoMax. For this run, I used the default solver. I’m curious to know the differences between the available solvers and whether there might be one that’s better suited for this type of structure than the default option.
