Jump to content
Sign in to follow this  
konrad_cure

High Energy Error

Recommended Posts

Hello,

 

for my Formula Student Team I am trying to simulate the deformation of the Anti Intrusion Plate. To replicate the real test I've tried to implement the Honeycomb Impact Attenuator Tutorial(https://altairuniversity.com/wp-content/uploads/2016/11/Crash_Box_1.pdf). I've attached the file. When I try to run the simulation the Energy Errror starts at 0% and then rockets up to 99.9%. Then the Simulation stops.

 

ROOT: SteelDummy  RESTART: 0001
 NUMBER OF HMPP PROCESSES     4
 02/12/2019
 NC=       0 T= 0.0000E+00 DT= 2.1400E-04 ERR=  0.0% DM/M= 1.7748E-05
     ANIMATION FILE: SteelDummyA001 WRITTEN
 NC=     100 T= 2.1400E-02 DT= 2.1400E-04 ERR= -0.0% DM/M= 1.7748E-05
 ELAPSED TIME=         54.23 s  REMAINING TIME=     126646.67 s
 NC=     200 T= 3.5753E-02 DT= 1.2229E-04 ERR= -0.0% DM/M= 1.7748E-05
 ELAPSED TIME=         54.82 s  REMAINING TIME=      76607.94 s
 NC=     300 T= 4.7072E-02 DT= 1.0479E-04 ERR= -0.0% DM/M= 1.7748E-05
 ELAPSED TIME=         55.35 s  REMAINING TIME=      58738.95 s
 NC=     400 T= 5.6878E-02 DT= 9.1867E-05 ERR= -0.0% DM/M= 1.7748E-05
 ELAPSED TIME=         55.87 s  REMAINING TIME=      49054.49 s
MESSAGE ID :        259
 ** WARNING ZERO OR NEGATIVE VOLUME : 3D-ELEMENT ID : 700
   ELEMENT IS SWITCHED TO SMALL STRAIN OPTION
MESSAGE ID :        259
 ** WARNING ZERO OR NEGATIVE VOLUME : 3D-ELEMENT ID : 1940
   ELEMENT IS SWITCHED TO SMALL STRAIN OPTION
MESSAGE ID :        259
 ** WARNING ZERO OR NEGATIVE VOLUME : 3D-ELEMENT ID : 3120
   ELEMENT IS SWITCHED TO SMALL STRAIN OPTION
MESSAGE ID :        259
 ** WARNING ZERO OR NEGATIVE VOLUME : 3D-ELEMENT ID : 4080
   ELEMENT IS SWITCHED TO SMALL STRAIN OPTION
 NC=     500 T= 6.2841E-02 DT= 1.1098E-13 ERR= 99.9% DM/M= 1.7748E-05
 ELAPSED TIME=         56.40 s  REMAINING TIME=      44815.82 s
 NC=     600 T= 6.2841E-02 DT= 1.1098E-13 ERR= 99.9% DM/M= 1.7748E-05
 ELAPSED TIME=         56.93 s  REMAINING TIME=      45237.79 s
 NC=     700 T= 6.2841E-02 DT= 1.1098E-13 ERR= 99.9% DM/M= 1.7748E-05
 ELAPSED TIME=         57.43 s  REMAINING TIME=      45635.91 s
 NC=     800 T= 6.2841E-02 DT= 1.1098E-13 ERR= 99.9% DM/M= 1.7748E-05
 ELAPSED TIME=         57.99 s  REMAINING TIME=      46084.90 s
 NC=     900 T= 6.2841E-02 DT= 1.1099E-13 ERR= 99.9% DM/M= 1.7748E-05
 ELAPSED TIME=         58.58 s  REMAINING TIME=      46552.16 s
MESSAGE ID :        205
 ** RUN KILLED : ENERGY ERROR LIMIT REACHED
 NC=    1000 T= 6.2841E-02 DT= 5.1022E-18 ERR= 99.9% DM/M= 1.7748E-05
 ELAPSED TIME=         59.22 s  REMAINING TIME=      47060.74 s
     ANIMATION FILE: SteelDummyA002 WRITTEN

 

 

Thanks upfront,

 

Konrad

SteelDummy.hm

Share this post


Link to post
Share on other sites

Hi,

 

"ZERO OR NEGATIVE VOLUME" warning happens when solid elements are very deformed and their characteristic length goes to 0. For large strain formulation, the time step of an element is reduced when the element is compressed. Solid elements assigned with a relatively compliant material can be deformed so severely that its nodes go through the opposite side and even cause a negative volume. 

 

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. /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.


This honeycomb component can not absorb all of the initial kinetic energy. You should define failure criteria to avoid zero or negative volume and obtain more realistic results. 

 

The master-slave definitions were swapped in the type 7 contact- the master should be stiffer, coarser meshed component. Contact parameters were modified to the recommended. There were initial penetrations so the impactor plate was moved.

SteelDummy_edit.hm

konrad_cure likes this

Share this post


Link to post
Share on other sites

I have reviewed your model again because the deformation just did not look right. You forgot to define the material orientation of the honeycomb property (by default if no orientation is provided it takes element orientation). Also, as per the tutorial, the wrong shear yield stress function was assigned. The honeycomb component can now absorb all of the initial kinetic energy.

SteelDummy_edit2.hm

konrad_cure likes this

Share this post


Link to post
Share on other sites

Glad to help. 

 

Looks like the material orientation step is missing in the tutorial. 

 

Sharing issues on the forum is a great way to catch problems that could happen even to experienced users. That is why feeback (even if negative) is important.

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

Sign in to follow this  

×
×
  • Create New...