Good afternoon everyone,
I am currently using Prepomax (as I mentioned before it’s an incredible software).
During one of the comparison analyses, I noticed significant discrepancies between the results obtained with Ansys and what is observed in Prepomax.
Specifically, it appears that the contact definition is not functioning correctly. The stress values and their distribution around the holes are incorrect.
I’ve tried various modifications to the contact definition, changed the mesh (type and small size) and experimented with different solvers, but I still obtain the same incorrect values.
The solution is better if I use tie constraints insted of contacts, but that’s not what I want to do in this test.
I haven’t find the solution in old posts.
You have a very different mesh in PrePoMax, with tetrahedral elements using the default size and no refinement. Try to make it more similar to the one used in Ansys or, even better, use the same mesh in both analyses (assuming that Ansys can export the mesh to .inp or some neutral format). Mesh in regions of interested (especially with contact involved) should be really dense.
Is the rest of the setup (e.g. boundary conditions) the same ? I’ve also noticed that in PrePoMax you apply the force only to one half of the hole while in Ansys it’s applied to the entire hole. So that’s yet another difference.
Calculix is not Ansys and Calculix will not be like Ansys. Some contact definition is very different, e.g. Master/Slave should be switched compared to the Ansys contact definition proposals. And you must be sure that your modeling is comparable.
I made a similar contact model from a bicycle chain in PrePoMax and that looks very good.
First you should start with a compound part and select “split compound mesh - yes” to generate coincident nodes between the separate parts. That would reduce the high peak stresses you get because of penetrating elements in combination with the coarse mesh. However, because of the sharp edge-contact and linear material, the results at the edges won’t ever converge i guess.
Good morning everyone,
I thank you for the responses, which I found all very helpful.
First of all, I wanted to explain my situation in more detail:
This analysis does not require high precision. It falls into the category of E.C. checks, and for example, I don’t even look at the peak values around the hole, preferring to verify them manually.
What struck me, besides the unrealistic stress values, is the complete lack of sense in their distribution. Instead of being localized at the contact side between the hole and the screw, the stress distribution is uniform around the hole. It’s easy to see that the results are nonsensical from the comparison image created by Gunnar (the before and after his intervention).
Now, I’ll respond to the various people who helped me:
FEAnalyst: I had already tried a very dense mesh without improvement. The values were very similar, so I preferred to send the file with the larger mesh for your convenience in analysis. Increasing mesh density (assuming the current mesh is not excessively coarse) improves stress value accuracy but doesn’t change the overall distribution, as mentioned earlier. The constraints in both Ansys and Prepomax models are quite similar (but not perfectly identical).
Arnie: Thank you for the additional information, which will undoubtedly enhance the accuracy of the obtained values. Unfortunately, I cannot access the Ansys source file, and I don’t have information about displacements. However, in the specific case at hand, displacements wouldn’t make much sense because the model is highly sensitive in that regard, given that the node acts as a hinge. Small variations in the constraints added for convergence can significantly impact deformation values due to rotations in the bolt contact zone (stress values don’t have this issue).
fatigue.pro: It’s true that Ansys and Calculix are different, but for “simple” analyses (assuming constraints and loads are very similar), the results should be similar (at least in stress distribution and magnitude), even if the mesh is slightly different. The differences between the two models, from my perspective, are “negligible” for the purpose of the work. (PS: I’ve read your articles on fatigue.pro, they’re very interesting. Fatlab is a great software that I plan to try out.)
Gunnar: Thank you. As I suspected, the issue was related in some way to the contact definition. I admit that the “Compound Part” function is quite unfamiliar to me since I don’t use it in my other softwares. Now I finally understand its purpose.
Thanks for the replies, I really appreciated them, and sorry for the long post.
I would say that using a smaller contact stiffness helps in cases where the mesh in contact is not coincident. Non-coincident mesh courses stress concentrations since only a few nodes come into contact - in penetration. This number of nodes can be increased by allowing a greater penetration in contact.
I ran a basic test to compare contact stress results (and fringe plot patterns) between Ansys and PrePoMax. The model is rather simple and just consists of two plates held together with a bolt & nut (simplified). One plate is fixed at the far surface and a force (tension) is applied at the far surface of the other plate. Frictional surface contacts with coefficient of 0.2 were applied to all the contact faces between plates, bolt & nut. Ansys solver used was linear static and in PPM I used non linear Pardiso solver.
In both software I meshed the plates with 2.5mm second order hex elements. In PPM, I had to mesh the bolt & nut with 2.5mm second order tet elements because I did not section it.
You may be interested to see the similarity in results and fringe plots below between Ansys and PPM.
A note however that in using the same laptop where Ansys takes only 48 seconds to solve, PPM takes a 99 minutes !
Some FE solver use compression only element and nodal constraints for contact without large deformation activated, this mean purely iteration by element force detected and it can be faster. However, a solver times discrepancy of single bolt contact analysis from below one minute in Ansys to almost two hours in CalculiX is look strange for me. Maybe it can give insight by starting the same mesh and element, contact surfaces definition also.
Yes, the mesh is clearly not the same but it’s also mentioned that in Ansys it was a linear solver (without Nlgeom, I guess since contact introduces nonlinearity as well) while in PrePoMax it was a nonlinear one.
Maybe it can give insight by starting the same mesh and element, contact surfaces definition also.
@synt Unfortunately Ansys does not export a mesh format that PPM recognizes. However, I can split the simplified ‘bolt & nut’ and mesh it with second order hex mesh and then re-run. I will report back on this and the results soon.
I guess since contact introduces nonlinearity as well)
@FEAnalyst Yes, with frictional contact Ansys switches over to non-linear solver, so the disparity in solve time is really a mystery to me too. Having said this; I am not complaining because one is free and the other costs you a kidney in the subscription every single year !!
If it can export to Abaqus or Nastran format then it should be possible to convert it to CalculiX .inp at least partially readable by PrePoMax (just to import the mesh). I guess there are no universal mesh formats supported for export ?
The model you shared has a hexahedral bolt mesh, and the bolt is split into three parts. Should I merge the bolt parts and use the default mesher to get the model you compared with Ansys? Or do you have it still?
Yeah, I tried that but the weird thing is that if I use the Search Contact Pairs, it does not recognize the Merged Part as individual parts that need to be connected… It only recognizes the plate contacts to each other and the nut & head.
