Negative volume error in RADIOSS
Hello All,
I am new to use RADIOSS.
I do not know how to define property card for in RADIOSS for 4 node tetra elements and 8 node hex elements. I have defined ISOLID as 12 and I _tetra as 1 for hex and tetra elements respectively. Remaining fields were not defined.
I have used RBODY elements to connect the parts. When I give run, It is showing error with the message,
MESSAGE ID : 169
** STOP : ZERO OR NEGATIVE VOLUME
FOR 4 NODES TETRAHEDRON ID=121736, INTEGRATION POINT=1
I do not know how to solve this issue. Is there any options/ method to remove this error?
Answers
-
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 try the run with this option.
0 -
Hi, I've got the same problem. I'm simulating an dynami impact test with a PP-polymer. I'm getting the same error message for a tetra element due to exzessive compression.
For the material I'm using the PLAS_TAB card with Pressure vs. yield factor function. The maximum failure strain is 180% for tension. There is no failure strain for compression.
Property:
SOLID
Isolid=25
Icrpe=1
Itetra=1
I tried the option Ismstr=2 plus the following input
/DT/NODA/CST
0.9 0.0009
/DT/BRICK/CST
1.0 0.00088 --> even with a relativ high timestep I get the same error message at exactly the same time:ANIMATION FILE: ********************************************************A012 WRITTEN
6600 5.515 0.7132E-03 INTER 1 1.1% 59.17 143.9 2.196 4.212 0.1993E-01MESSAGE ID : 169
** STOP : ZERO OR NEGATIVE VOLUME
FOR 4 NODES TETRAHEDRON ID=6580602, INTEGRATION POINT=4So I don't see any effect on the solution when I'm using Ismstr=2 !?
How can I solve the problem?
0 -
Hi Eduard,
Please recheck the interface Id 1 defined in the model and also ensure there are no penetrations in the model. By using Ismstr=2 the solid elements will switch to small strain. Please share the model file through the secure dropbox so that we can check the model and suggest the solution.
0 -
Hi George,
apparently in HW 14 the option Ismstr=2 is only avaliable for hexa-elements. I tried to increase the Pressure vs. yield factor function and to reduce the failure strain to 80% but it was unsuccessfull too. There are no penetrations in the interface. I will upload one of the versions.
0 -
Hi Eduard,
Relieved the file. We will check this and will update you very soon.
0 -
Hi Eduard,
Ismstr=2 option is available with tetra elements, with HW 14 version also. Keep Itetra=0 and run with Ismstr=2 option,which is compatible.
The modified files has been sent to you.
0 -
Hi George,
the model I’ve send to you is simplified. That’s why there are no interfaces. But so far my questions have been answered.Thankyou very much for your quick support
0 -
Altair Forum User said:
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 try the run with this option.
Hi George,
I have the same problem and tried what you described above, but it didn't help. Can you have a look at my model and try to help me find the problem? Thanks in advance!
Edited to add most recent versions, still the same problem.
0
Altair Employee