Negative Volume
Altair EmployeeHey,
after creating my model and run the simulation i realized that i made i scaling mistake and i rescaled it with Hypermesh and now my model is 1000 times smaller. If i run the simulation now i got an error with NEGATIVE OR ZERO VOLUME. I already tried to switch properties - because i have a soft material in my model - and after this now i have a new error and RADIOSS find a initial penetration.
Now I am a little bit confused. I hope you can help me. I uploaded my model, just in case.
Best and thanks, Max.
Answers
-
Hi Max,
We will have a workaround in your model and will update you the same.
0 -
Thank you very much!
Best,
Max
0 -
Hi Max,
This NEGATIVE VOLUME error happens when solid elements are very deformed and their characteristic length goes to 0. For large strain formulation the time step of an element goes to 0 when the element is compressed.
In RADIOSS Starter input file (Runname_0000.rad), use Ismstr =2 in the solid property and in RADIOSS Engine file (Runname_0001.rad) use the option/DT/BRICK/CST which will set the time step value tmin at which the solid elements will switch to small strain.This means that the solid elements using Ismstr =2 will use large strain formulation while their time step remains greater than tmin, and will then switch to small strain formulation.
(/DT/BRICK/CST option is used to control the time step of the analysis. The time step becomes constant after reaching Tmin specified by the user )
Please check with the model attached along.
0 -
Thank.
Did you change something? But now i load my old control cards and now the estimations need just 7000sec instead of 27000.
Thank you a lot.
Best, Max
0 -
Hi Max,
I just cleared the penetrations in the model and only some slight changes.The model and other parameters remains the same. Penetrations can result in time step drop, and since it is cleared now it can be one reason for the reduction in estimation time.
0 -
Thank you very much it worked very well.
Can you explain me how did you clear the penetrations with which tool?
Best Max
0 -
Hi Max,
In HyperMesh, in Tool menu>Penetration option is available to check for penetrations. There are various options available for fixing.
<?xml version="1.0" encoding="UTF-8"?>
In HyperCrash, go to LoadCase>Contact Interface and select the contact in the model and click on check penetrations. A depenetrate auto option is available which will automatically fix the penetrations.
<?xml version="1.0" encoding="UTF-8"?>
0 -
Hey,
thank you very much. The thing is i used this tool already before and before i checked the penetration i used the faces tool to equivalence the faces. Who knows.
Thank you very much for your help.
Best
Max
0
