Warning ID 760
Hello,
I am trying to simulate a deep drawing process of a thermobimetal plate with HyperCrash. The current model is very crude, but will be improved once this Problem is solved.
When trying to solve my model with RADIOSS I Encounter the following error:
************************************************************************
** **
** **
** RADIOSS STARTER 2017.2.1 **
** **
** Non-linear Finite Element Analysis Software **
** from Altair Engineering, Inc. **
** **
** **
** Windows 64 bits, Intel compiler **
** **
** **
** **
** Build tag: 0876086_123352072.1_1020_0049245_10 **
************************************************************************
** COPYRIGHT (C) 1986-2017 Altair Engineering, Inc. **
** All Rights Reserved. Copyright notice does not imply publication. **
** Contains trade secrets of Altair Engineering Inc. **
** Decompilation or disassembly of this software strictly prohibited. **
************************************************************************
.. BLOCK FREE FORMAT
.. STARTER RUNNING ON 1 THREAD
.. CONTROL VARIABLES
.. UNITS SYSTEM
.. FUNCTIONS & TABLES
.. MATERIALS
WARNING ID : 765
** WARNING IN MATERIAL LAW
WARNING ID : 765
** WARNING IN MATERIAL LAW
.. NODES
.. PROPERTIES
.. 3D SOLID ELEMENTS
.. 3D SHELL ELEMENTS
.. 3D TRIANGULAR SHELL ELEMENTS
.. SUBSETS
.. ELEMENT GROUPS
.. PART GROUPS
.. SURFACES
.. NODE GROUP
.. BOUNDARY CONDITIONS
.. IMPOSED VELOCITIES
.. AMS INITIALIZATION
.. DOMAIN DECOMPOSITION
.. ELEMENT GROUPS
.. INTERFACES
.. INTERFACE BUFFER INITIALIZATION
.. RIGID BODIES
.. RETURNS TO DOMAIN DECOMPOSITION FOR OPTIMIZATION
.. AMS INITIALIZATION
.. DOMAIN DECOMPOSITION
.. ELEMENT GROUPS
.. INTERFACES
.. INTERFACE BUFFER INITIALIZATION
.. RIGID BODIES
.. ELEMENT BUFFER INITIALIZATION
** ERROR TRAPPED : REPORT TO LISTING FILE
ERROR ID : 760
==== End of solver screen output ====
==== Job completed ====
I have attached the .rad file I exported from HyperCrash.
I would appreciate any help. Thank you in advance.
Answers
-
Hi,
to find modeling errors and warnings use:
- Hypercrash: quality>modelchecker>run
- Hypermesh: Tools>Model Checker>RadiossBlock
In the model you shared these are the error and remedies:
- components active and passive has more than one element type which is invalid. Shell elements used for solid element creation should be moved into a separate component or deleted. Use display/mask/isolate by element type to identify offending elements
- there are duplicate 2D elements: since those elements were used for solid creation they can be deleted prior to simulation.
- negative or zero volume of solids: is due to the poor element quality at the center created by spinning. The solid is decomposed into sub-volumes associated to each integration point. If the element is badly shaped, one sub-volume could be negative. Check your element quality by check elements (F10)>3D>aspect, jacobian, warpage, tet collapse in Hypermesh or Check elements of tree selection in Hypercrash.
0 -
Thank you very much for your reply. I have improved the model according to your suggestions and I am now able to run the calculation without encountering an error.
However, there doesn't seem to be any calculating being done:
************************************************************************
** **
** **
** RADIOSS STARTER 2017.2.1 **
** **
** Non-linear Finite Element Analysis Software **
** from Altair Engineering, Inc. **
** **
** **
** Windows 64 bits, Intel compiler **
** **
** **
** **
** Build tag: 0876086_123352072.1_1020_0049245_10 **
************************************************************************
** COPYRIGHT (C) 1986-2017 Altair Engineering, Inc. **
** All Rights Reserved. Copyright notice does not imply publication. **
** Contains trade secrets of Altair Engineering Inc. **
** Decompilation or disassembly of this software strictly prohibited. **
************************************************************************.. BLOCK FREE FORMAT
.. STARTER RUNNING ON 1 THREAD
.. CONTROL VARIABLES
.. UNITS SYSTEM
.. FUNCTIONS & TABLES
.. MATERIALS
WARNING ID : 765
** WARNING IN MATERIAL LAW
WARNING ID : 765
** WARNING IN MATERIAL LAW
.. NODES
.. PROPERTIES
.. 3D SOLID ELEMENTS
.. 3D SHELL ELEMENTS
.. SUBSETS
.. ELEMENT GROUPS
.. PART GROUPS
.. SURFACES
.. NODE GROUP
.. BOUNDARY CONDITIONS
.. IMPOSED VELOCITIES
.. AMS INITIALIZATION
.. DOMAIN DECOMPOSITION
.. ELEMENT GROUPS
.. INTERFACES
.. INTERFACE BUFFER INITIALIZATION
.. RIGID BODIES
.. RETURNS TO DOMAIN DECOMPOSITION FOR OPTIMIZATION
.. AMS INITIALIZATION
.. DOMAIN DECOMPOSITION
.. ELEMENT GROUPS
.. INTERFACES
.. INTERFACE BUFFER INITIALIZATION
.. RIGID BODIES
.. ELEMENT BUFFER INITIALIZATION
WARNING ID : 499
** WARNING : INITIAL PENETRATIONS IN INTERFACE
.. GEOMETRY PLOT FILE
.. PARALLEL RESTART FILES GENERATION
TERMINATION WITH WARNING
------------------
0 ERROR(S)
5 WARNING(S)
PLEASE CHECK LISTING FILE FOR FURTHER DETAILS==== End of solver screen output ====
************************************************************************
** **
** **
** RADIOSS ENGINE 2017.2.1 **
** **
** Non-linear Finite Element Analysis Software **
** from Altair Engineering, Inc. **
** **
** **
** Windows 64 bits, Intel compiler **
** **
** **
** **
** Build tag: 0876086_123352072.1_2020_0049245_10 **
************************************************************************
** COPYRIGHT (C) 1986-2017 Altair Engineering, Inc. **
** All Rights Reserved. Copyright notice does not imply publication. **
** Contains trade secrets of Altair Engineering Inc. **
** Decompilation or disassembly of this software strictly prohibited. **
************************************************************************ROOT: Tiefziehen_HC RESTART: 0001
NUMBER OF HMPP PROCESSES 1
28/08/2019
NC= 0 T= 0.0000E+00 DT= 1.2774E-05 ERR= 0.0% DM/M= 0.0000E+00
ANIMATION FILE: Tiefziehen_HCA001 WRITTEN
STATE FILE: Tiefziehen_HC_0001.sta WRITTEN
RESTART FILES: Tiefziehen_HC_0001_[0001-0001].rst WRITTEN** CPU USER TIME **
#PROC CONT.SORT CONT. F ELEMENT KIN.COND. INTEGR. I/O TASK0 ASSEMB. AMS RESOL
1 .9828E+00 .3120E-01 .6037E+01 .1248E+00 .3432E+00 .1872E+00 .6240E-01 .1560E-01 .1995E+02 .2800E+02** CUMULATIVE CPU TIME SUMMARY **
CONTACT SORTING............: .9828E+00 3.51 %
CONTACT FORCES.............: .3120E-01 0.11 %
ELEMENT FORCES.............: .6037E+01 21.56 %
KINEMATIC COND.............: .1248E+00 0.45 %
INTEGRATION................: .3432E+00 1.23 %
ASSEMBLING.................: .1560E-01 0.06 %
AMS........................: .1995E+02 71.26 %
OTHERS (including I/O).....: .5129E+00 1.83 %
TOTAL......................: .2800E+02 100.00 %** MEMORY USAGE STATISTICS **
TOTAL MEMORY USED .........................: 43 MB
MAXIMUM MEMORY PER PROCESSOR...............: 43 MB
MINIMUM MEMORY PER PROCESSOR...............: 43 MB
AVERAGE MEMORY PER PROCESSOR...............: 43 MB** DISK USAGE STATISTICS **
TOTAL DISK SPACE USED .....................: 7133 KB
ANIMATION/TH/OUTP SIZE ....................: 726 KB
RESTART FILE SIZE .........................: 6407 KBELAPSED TIME = 29.86 s
0:00:29NORMAL TERMINATION
TOTAL NUMBER OF CYCLES : 1983==== End of solver screen output ====
==== Job completed ====I suspect, that I have made some Errors in defining the control Cards.
The improved .rad file is attached.
Thank you in advance.
0 -
Hi,
glad to help.
- Check unit consistency: the diameter of the disk is 50 meters and it weighs only 16 grams?
- In Hypermesh use Tools>Engine file assistant to set up basic run and output parameters.
- The Type 21 interface did not work- so type 24 with the same settings as others were used
- Use Isolid=24 in solid property to reduce hourglass
- The loading function of 10 seconds duration is computationally expensive for explicit method. It could be solved more efficiently by applying the load over shorter period of time or with implicit method.
0 -
Thank you again for your reply.
I have made the changes based on your suggestion and the simulation is working now.
During this process however, I have removed all control cards that didn't align with your edited model. These included, among others, all cards that were selected to write state files.
It is my goal to export the solution of this simulation and import it in HyperMesh, because I need the strain that is induced during the deep drawing process to correctly simulate the discs behavior under a temperature load. I was told, that this is best done with state files. What cards would I have to select to do this?
Thank you yet again in advance.
0 -
The procedure to carry over stress and strain state of elements is to create STATE engine cards in the 1. step:
/STATE/BRICK/STRAIN/FULL
/STATE/BRICK/STRES/FULLif there are shells also create additional cards (search Radioss help with keyword: STATE)
/STATE/DT(define start time and frequency to write state files and declare components to be included)
Run the simulation which creates model_name.sta file, which is then imported into the original model. It will overwrite the original mesh with deformed and there should also be Tables entry in the model browser (stress & strain information for each element that can be edited).
Attached are the modified files and also some tips about STATE files.
https://community.altair.com/community?id=community_question&sys_id=af76483a1b2bd0908017dc61ec4bcb1a0 -
Thank you very much. I managed to Import the state file.
Now I am trying to impose a temperature load on the disc which should result in a Change of curvature. However, after running the Simulation no Change is visible at all. I am assuming that I did something wrong with the control Cards again.
Thank you in advance for your help.
0