how to solve the ZERO OR NEGATIVE VOLUME problem when using very soft material?
Altair EmployeeHi,
I am trying a simple impact analysis like radioss example 26 ruptured plate ( I am not interested in the rupture, just want to try an impact problem). I am using a soft non linear material M36_PLAS_TAB with a stress strain curve (E=8Mpa,nu=0.42,rho=1.412e-6Mg) and fixing the whole bottom surface. I used the volume tetra mesh to mesh my disk. ( I am using solid elements instead of shells as a basis for a more complex problem I am working on)
The model was working fine with linear elastic materials...
I read a few posts about this problem. There it was suggested to use a really thin linear elastic surface on top.
And to change the element formulation.
Could you please elaborate more in detail the steps to overcome this problem?
Thanks!
Answers
-
We have some FAQ about this error message depending when you get the error message, Is it for the starter? does the error also include an element ID or element description?
When you change the element formulation, card edit the property and then choose ismstr to 2 along with timestep variation as explained in detail in the FAQ below.
Navigation: Altair RADIOSS > RADIOSS Frequently Asked Questions > Elements
I used solid elements and the run stopped before the end time, with the message: 'Zero or Negative Volume'. How do I solve this problem?Navigation: Altair RADIOSS > RADIOSS Frequently Asked Questions > Elements
I used solid elements with Ismstr=2 and /DT/BRICK/CST; but the run stopped with the message: 'Zero or Negative Volume'; is this normal?Navigation: Altair RADIOSS > RADIOSS Frequently Asked Questions > Elements
I used solid elements and several integration points, and the Starter gives the following error message while the element seems to be well-defined: ** ERROR: ZERO OR NEGATIVE 3D SOLID VOLUME, is this normal?0 -
I tried using Isolid=14 and 24 and used Icpre to 2.
But still the error remains..:
MESSAGE ID : 166
** STOP : ZERO OR NEGATIVE VOLUME FOR 3D-ELEMENT ID=18219
ERROR TERMINATION0 -
ow to use the HA8 formulation? I am using block51 format. I don't see Inpts option in the card edit window..
0 -
Arbhaval,
If you are using tetrahedron elements you should perhaps not change the Isolid value,
The Isolid flag is not used with 4- and 10-node tetrahedron elements. For these elements the number of integration points is fixed (1 and 4, respectively).
Read the last FAQ topic -
In the RADIOSS Starter input file (Runname_0000.rad), use Ismstr =2 in the solid property or in the option /DEF_SOLID; in RADIOSS Engine file (Runname_0001.rad) use the option /DT/BRICK/CST0 -
I tried using Icpre=2 with a combination of Ismstr=2, No Isolid; No Ismstr , No Isolid . I also tried Isolid=0,1, But no luck yet.. I am using DT/Brick/CST with 0.6Tscale and 5e-7Tmin
NC= 0 T= 0.0000E+00 DT= 1.2600E-04 ERR= 0.0% DM/M= 0.0000E+00
ANIMATION FILE: similartoes26zsorbothane100kgpvelA001 WRITTEN
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 16954
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 17763
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 11585
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 13442
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 16598
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 16945
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 17318
MESSAGE ID : 166
** STOP : ZERO OR NEGATIVE VOLUME FOR 3D-ELEMENT ID=18218
MESSAGE ID : 166
** STOP : ZERO OR NEGATIVE VOLUME FOR 3D-ELEMENT ID=18702
ERROR TERMINATION
ERROR TERMINATION==== End of solver screen output ====
I also tried using Ismstr=1,Icpre=2,No Isolid and it gave me no errors. But the sphere passed through the disk. I got normal termination with this combination. But I don't know if the results are valid/practical?This was the solver output:
NC= 0 T= 0.0000E+00 DT= 1.2600E-04 ERR= 0.0% DM/M= 0.0000E+00
ANIMATION FILE: similartoes26zsorbothane100kgpvelA001 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA002 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA003 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA004 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA005 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA006 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA007 WRITTEN
RESTART FILES: similartoes26zsorbothane100kgpvel_0001_[0001-0001].rst WRITTEN
NORMAL TERMINATION
TOTAL NUMBER OF CYCLES : 1700 -
I also tried to solve the warnings of 'incompatible kinematic conditions' but couldn't.. I read about it in the help and tried to add one more rigid wall but I am not able to get rid of these warnings.. Please give me some suggestions..
0 -
i,
Remove the constraint in Z direction. In your model a boundary condition and imposed velocity are in same direction. for more information on Kinematic condition please refer to FAQ in Help.
0 -
es, I am trying to analyze the impact of the ball on the foam material.
I tried this impact in 4 models each with different materials. Now I have combined all of these materials (using type 7 interfaces with csurfs and node sets) and want to run the analysis.
I didn't get any errors. But the solver is taking long time to run. I assume this is comparatively a simple analysis. So I might be doing something wrong. Maybe in the engine file definition. Can you please take a look and give any tips? I am sending the model file by dropbox.
Thanks!0 -
Hi,
there are 2D scattered elements in your model, please delete and re-configure the master surface and slave nodes.
0 -
Hi,
Thanks. I am able to get results and animations with a normal termination. But from the animation, it is clear that I am making some mistakes probably in my use of contacts. I read the General Purpose Interface (/INTER/TYPE7) help and think I should follow the Soft Part Against Hard Part technique. I don't know how I should calculate the stiffness values and what flags to use in the contact definition. Can you please advise me?0 -
i,
in TYPE7 card, change the Istiff to 4 and run the analysis. you can also specify a stiffness factor (STFAC)
Istiff 4 takes the minimum stiffness of master and slave.
hope this helps
0 -
Hi,
I am doing drop test analysis, but following error is coming.
MESSAGE ID : 44** ERROR : ABNORMAL END+=============================================================+| Segmentation Violation |+=============================================================+| TRACE BACK : |+=============================================================+| + RADIOSS ENGINE| + SOLUTION PHASE: Processor= 1/ 1| + MAIN LOOP: Cycle= 0| + INTERNAL FORCES+=============================================================+ERROR TERMINATIONcould you please suggest to solve this error.Thank youRegards,Narasimahmurthy0 -
Hi narasimhamurthy,
INDIA support is taking care of your query.
Please note: if you are a commercial customer, you can contact your local support @ http://www.altairhyp...ortProduct.aspx
0 -
Hi,
to model foams use law70 and tetrahedrons (Ismstr4). It is VERY important to extrapolate the compressive stress-strain-curve near the compression point! If you do not so, the elements will inverse at large deformations finally leading to zero negative.
0 -
Hi Prakash - I am getting similar problem -
One which listed in this post -
tried using Icpre=2 with a combination of Ismstr=2, No Isolid; No Ismstr , No Isolid . I also tried Isolid=0,1, But no luck yet.. I am using DT/Brick/CST with 0.6Tscale and 5e-7Tmin
NC= 0 T= 0.0000E+00 DT= 1.2600E-04 ERR= 0.0% DM/M= 0.0000E+00
ANIMATION FILE: similartoes26zsorbothane100kgpvelA001 WRITTEN
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 16954
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 17763
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 11585
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 13442
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 16598
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 16945
-- CONSTANT TIME STEP FOR SOLID ELEMENT NUMBER 17318
MESSAGE ID : 166
** STOP : ZERO OR NEGATIVE VOLUME FOR 3D-ELEMENT ID=18218
MESSAGE ID : 166
** STOP : ZERO OR NEGATIVE VOLUME FOR 3D-ELEMENT ID=18702
ERROR TERMINATION
ERROR TERMINATION==== End of solver screen output ====
I also tried using Ismstr=1,Icpre=2,No Isolid and it gave me no errors. But the sphere passed through the disk. I got normal termination with this combination. But I don't know if the results are valid/practical?This was the solver output:
NC= 0 T= 0.0000E+00 DT= 1.2600E-04 ERR= 0.0% DM/M= 0.0000E+00
ANIMATION FILE: similartoes26zsorbothane100kgpvelA001 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA002 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA003 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA004 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA005 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA006 WRITTEN
ANIMATION FILE: similartoes26zsorbothane100kgpvelA007 WRITTEN
RESTART FILES: similartoes26zsorbothane100kgpvel_0001_[0001-0001].rst WRITTEN
NORMAL TERMINATION
TOTAL NUMBER OF CYCLES : 170I have tried to use Icpre=2 but problem still persists. Can you please let me know how did you solve this problem ?
0 -
Hi,
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 the a higher value of Tmin.
0 -
Hi George -
Thank you for your reply. I have already tried doing that. I changed my Ismstr value to 2 and gave tmin value of 7e-7 in control card CST. I am still getting the error. within first 10 mins of run
0 -
Hi,
Can you share the model file through the secure dropbox link?.
0 -
Hi George - I have shared the model file with you.
0 -
Hi,
The corrected file has been sent to you.
0 -
Hi GeorgeNow I am able to run file but I am not getting any h3d file in the end of run. Plus a error message -pops up when I try to run individual animation file. Am I still missing something ?Thanks0
-
Hi,
This seems to be a bug. I'm able to open the same in HyperWorks 14 and 2017 version.
Which version are you using?.
0 -
Hi - I am using HyperWorks14.0 2017 version. Probably I will try running it again. Can you explain changes/adjustments that made in model ? I know re-defined slave nodes in Self-contact by some other method. Anything other than that ?
0 -
Hi,
I modified only the contact parameters.
The recommended contact parameters for /INTER/TYPE7 are:
Istf=4
Igap=2
Fscale_Gap=0.8
INACTI=6
Gap_min=0.1
Fric = 0.1
Iform=2
Did you try loading .h3d file?.
0 -
Yes I did. It is opening fine in hypermesh. I will try to run it again.
0 -
Hi George - Can please have a look at my file again ? Sorry for troubling you again but I am still getting the error. Can you please check the file let me know if I am still making a error and send me back file in *.hm format.I appreciate your help. Thank you.0
-
Hi,
The modified files has been sent to you.
We always recommend to use the latest HyperWorks version which has the best features.Please go through the post below.
0
