Issues to solvers, multi core, stress parameter
After accomplished the B35 "Ball Coupling" tutorial, I tried another more simple test: a mere beam whose dimensions, material and BCs can be seen in the attached image. The results I've obtained not appear to be correct. Here they are:
No linear analysis, 50 loading steps, 10 spring back steps
Von Mises law:
max Total Displacement @ step 50 = 61MM
max Stress per Element = 690 Mpa
max Total Displacement @ step 50 = 3.24 MM
max Stress per Element = 750 Mpa
max Total Displacement = 3.23 MM
max Stress per Element = 853 Mpa
Analysis through Estructural Element Beam Nº 13
Max Total Displacement = 3.17 MM
The stress difference at the two NLA is coherent with the comments of the tutorial, but the 61 MM deflection for the analysis according von Mises law seems to be rather weird. (I also attach an image of the console for this analysis). What are your opinions?
Thanks a lot.
could you please send us your project folder so we can analyze this problem?
At first sight your load of 1 ton seems pretty high for a cross section of 30 mm x 10 mm. But we will look into this and come up with a solution when we analyzed your project.
P.S. I created a new thread for you so this problem can be easily found by other forum members.
Because its size (135MB), I compressed the folder an uploaded it to the cloud. This is the link:
https://drive.google.com/file/d/0B8BwIN ... sp=sharing
I had a look at your project and can say that the calculation went well and everything was set up ok.
Your problem is that the load is much too high for your structure. Keep in mind that a structural steel like E295 can only bear stresses up to 600-690 N/mm^2 and above that it will fail.
If you calculate your example with our linear solver, the material behaviour is linearly extrapolated and thus a very high stiffness is achieved with high loads. That's why you only get 3.2 mm deformation.
In real life this material would start to deform plastically with stresses around 295 N/mm^2 and with stresses above 600 N/mm^2 it will fail. Your linear calculation shows stresses above 800 N/mm^2, so it is your task to tell if your part will fail because Z88Aurora does not have a failure criterion implemented in its solvers.
Same for geometric nonlinear calculations (Hooke), the material behaviour is still linear and will give you great stiffness at high loads. Stresses are above all limits again.
For your calculation with von Mises (material nonlinear analysis) the solver runs fine, at the first load steps your structre deforms elastically and with higher load amount a plastic deformation comes up. This is when stresses get above 295 N/mm^2. But you still haven't reached your maximum load, so the solver keeps on raising the load amount and your structure flows plastically until it reaches its maximum tensile strength of around 600 N/mm^2. Due to the fact that we don't provide a failure criterion, the solver keeps on running until load application is finished. As already mentioned, in real life your part would have already failed and the deformation of 61 mm would not be reached. If you try to calculate your project with the Wehmann model, the solver will stop and provide an error message because the plastic deformation is too great. With von Mises model it runs fine but the results need to be seen in the real light
If you have further questions, please feel free to ask again - we are always there for our users!
Thanks alot for your comments that explain so well the logic and limits of a NLA solver. In other terms, the "real life" of this FEA tool, that regrettably is not the "real life" of what happens out there in the industry, where every day thousands of #10MM (or more) steel plates are cold bended 90º (or more) without fails, producing parts that will last for life.
I appreciate very much your concern for reality, that is also the mine and, I'm sure, of all the members of this forum. The 10000 N load from my example is just the load needed for a press brake to bend at 90º a # 30 x 10 MM steel plate with a 200 MM die opening. Notably, the 61 MM of deflection that outputs the solver under von Mises law, is very close to the "real life" deflection of this part, that is achieved without any fail.
What really happens (I'm sure you know this) is that due to the change of the mechanical properties under plastic deformation (work hardening / grain dislocation that reduce the continuity of the atomic slipping planes), the effective load application zone migrates along the part following the ductile regions (for that old law that says that the chain is broken by the weakest link), so the max tensile strength is never achieved.
I understand very well that apply this phenomenon is, at least for the moment, beyond the possibilities of FEA. Through your kind explanations it's now clear for me that the actual NLA is a very useful tool for cases where the max tensile strength is not exceeded and permanent deformations are unintended. If I've extended myself in these comments was just for loyalty with "real life".
you are completely right. "Real life" was in fact not correct, I should've said "the expected behaviour in reality according to the chosen material model".
The provided material models are just not suitable for the metalworking process forming. To perform a forming analysis, you would have to use adapted material models and material data.
My explanations were imprecise for clearer understanding for all forum members, which are not all specialists in material science But I'm glad you provided the necessary info for our professional users and made clear what you wanted to achieve and which problems were encountered.
Thank you very much for your answer. Perhaps this change of opinions has been of interest for someone else in the forum.
By the way, I have other questions. I hope you have time to consider them. Te material more applied in the projects I work is the Titanium alloy TiA6V4. See please the attached images and tell me, if it’s possible, if the Flow Curve that I’ve derived from the Strain / Stress curve (quasi static rate) is acceptable. I mean, if I’ve correctly interpreted the guide instructions.
I tested this Flow Curve (NLA / von Mises) and at least the calculation is accomplished, but the last steps require hundred of iterations. Almost reaching the limit. Is it due to some error in the Flow Curve? Or is because in this case the Yield Limit is too close to the Max Tensile Strength?
If the last one is the reason, I ask myself if it has sense to perform NLA with materials like Titanium, that have so plane curves.
Thanks a lot in advance.
- TiA6V4.jpeg (66.52 KiB) 2449 mal betrachtet
- TiA6V4flow.jpeg (77.33 KiB) 2449 mal betrachtet