Hello forum
i would appreciate if someone would have some time to look at the models attached in the ZIP-file. I am a bit confused. I tried to calculate two models. The Füll_ST_mod is the initial case. Füll_ST_mod2 has additional material to reduce y-deflection.
Unfortunately the second Model shows higher displacment ??
I used bonded contact. Are ther any Ideas?
Thanks
Comments
Many Thank's
today I observed some interesting behaviour. (using CCX)
I had build a model consisting of some individual parts with diferent materials. Most of then are coupled by bonded contact. between 2 there is a real contact.
The model was meshed without showing bad elements (after some modification) and could be solved showingg reasonable results. So far so good.
In the next step I put 2 more parts (simple cylinders of different material). Meshing was done for each of the two. The two are interconected by a bonded contact and these both then are connected to the previor existing sturcture with bonded contact.
When I solve the 2. case I get a bunch of errormessages telling about e.g.
*ERROR in e_c3d: nonpositive jacobian determinant in element 97 ...
I am very confused, because all of these errors are related in the part already generated in the 1. step. No remeshing was done for them.
Does anyony can give a exlanation for that. How can I proceed without recreating the whole model...?
Thanks in advance
PS: When I take the last model after aborting "Solve" and delete the additional parts of step 2 - no remeshing - the model is solved again. But the elemets indicated as bad are still there untouched ?????
that I thought also, but I used 0.7 mm with the TIE command and the "problem elements" are min. 20 mm and max. 120 mm away from the last fitted bonded contacts. (?)
I will try to do a complet remeshing with the current parameters
but still wondering about the bad elements when using bonded contact
thank you for your help. I have send you the model and some information about it.
I hope you got the mail and you could download the file
I don't want to bosther you, please let me only know if you received the model data by mail?
Thanks
Now I got your replies by mail.
Why it happens is still not clear to me, but you gave some valuable guidance how I could proceed.
I had also tried some thin with *TIE to Elastic and could run the modle.
Only it was difficult for me to really understand what are the differences in using it and how they affect the result
Regards
The tube is pressed into shape by an upper and a lower tool.
I modeled a non-linear material behavior for the pipe. Unfortunately, I was only able to solve the pressing phase from round into the desired shape after I reduced the Joung's modulus and the yield stress.
*SOLID SECTION,ELSET=rohr,MATERIAL=cublech
*MATERIAL,NAME=cublech
*ELASTIC
10e9,0.3
*PLASTIC
150e6,0
160e6,0.01
170e6,0.1
200e6,0.91
The tool movement is made by displacement constraints.
t/s y/mm +- for upper and lower tool
0 0
0.5 2.5
1 5
1.1 4.9
1.3 4.6
2 1
Now I wanted to see the condition when the tools are moved apart again. So the plastically deformed state on the pipe. Unfortunately I couldn't, because the solver did not solve and model "exploded"!
Does anyone have sugegstions how to get such calculations running stable.
Regards and thanks
It sometimes helps to turn off automatic time stepping and use a small time step.
Also, make sure the pipe is fully constrained, perhaps at its other end, so that when the contacts let go, it's won't experience rigid body motion.
1. Set the pipe elastic modulus and yield stress to the desired values. Set the tool to be elastic with elastic modulus ~2X that of the pipe. This usually makes the contact work better than more mismatched moduli. Adjust the tool stiffness as needed. It is usually easier to get things to converge with softer moduli; once you get things working you step up the moduli to real values (sounds like you know this).
2. Agree with Victor - use manual time stepping. Auto time stepping often leads to too large a step when contact first happens. Plan ~50 time steps for the closure - maybe more. Get that working well before you try unloading. Make sure there is not excessive interpenetration of the tool into the pipe at the final step. If there is, increase the penalty factor on the contact. Excessive interpenetration will often make the unloading crash.
3. Your graphics suggest to me that the contact search algorithm failed, but it may just be an unconverged state. Be sure your displacement increment over one time step is not more than about 20% of the smallest element linear dimension. This can be small, but it will save you a lot of headache in return for more computing time.
4. Once you add unloading, first try a small unloading step - maybe plan 25 time steps to unload from peak deformation to a small gap. You might need more to get things working.
Hope this helps.
-Robert
Take a look at this example.
Try running this model with increasing mesh density in the notch and you will see how density affects the result.