import operation errors - problem with shell elements

  • Kees Wouters
  • Kees Wouters's Avatar Topic Author
  • Offline
  • Moderator
  • Moderator
More
11 years 4 months ago #2682 by Kees Wouters
dear CAELinuxers,

Lately I am trying to model shell elements (coque) where I largely followed the tutorial by Paul Carrico. I think the modelling in Salome and running the analysis in Code Aster goes well.

I have problems importing the results into Salome. I must say the commands for calculating the results are far from clear to me. This is what I do after solving the system matrices:

[code:1]..
meshinit=LIRE_MAILLAGE(FORMAT='MED',
INFO=2,);

meshmod=CREA_MAILLAGE(MAILLAGE=meshinit,
MODI_MAILLE=(_F(TOUT='OUI',
OPTION='QUAD8_9',),
_F(TOUT='OUI',
OPTION='TRIA6_7',),),);
...
load1=.....

result=MECA_STATIQUE(MODELE=model,
CHAM_MATER=material,
CARA_ELEM=shellch,
EXCIT=_F(CHARGE=Load1,),);

result=CALC_ELEM(reuse =result,
MODELE=model,
CHAM_MATER=material,
RESULTAT=result,
OPTION=('SIGM_ELNO_DEPL','EQUI_ELNO_SIGM',),
EXCIT=_F(CHARGE=Load1,),);

result=CALC_NO(reuse =result,
RESULTAT=result,
OPTION=('SIGM_NOEU_DEPL','EQUI_NOEU_SIGM',),);

IMPR_RESU(FORMAT='MED',
UNITE=80,
RESU=_F(MAILLAGE=meshmod,
RESULTAT=result,
NOM_CHAM=('SIGM_NOEU_DEPL','EQUI_NOEU_SIGM','DEPL',),),);

FIN();[/code:1]

When I import the resulting mesh file into Salome post-processing I get the following error message:
Import operation has finished with errors
/../../../shell.resu.med
error in the file.

I get a warning of Code Aster regarding the central node of the shell element during running:
on traite les TRIA7 QUAD9 HEXA27 en oubliant le noeud centre !
! et les SEG4 en oubliant les 2 noeuds centraux.


I have uploaded the mesh, comm and mess file.
I anybody could shed some light on this problem I would be much obliged.

[edit: removed the comm and mesh files.]


Kind regards - kees<br /><br />Post edited by: Kees Wouters, at: 2009/03/17 21:34

Interest: structural mechanics, solar energy (picture at 'my location' shows too little pv panels)

--
kind regards - kees
Attachments:

Please Log in or Create an account to join the conversation.

More
11 years 4 months ago #2687 by johannes ackva
Replied by johannes ackva on topic import operation errors - problem with shell elements
Hi Kees
looking onto Your .mess file, I see the following:

Your mesh in Salome is one with QUAD8-elements, named &quot;meshinit&quot; in .comm. You created a new mesh with QUAD9-elements. You calculated this new mesh. This means that nodal results exist at all the 9 nodes of each QUAD9-element of the new mesh. Then You write all nodal results in a results-file in .MED-format for beeing read by Salome. So there is a discrepancy: Salome doesn't know 9 nodes per element, but only 8 nodes. That is the reason for the ALARM message.

Normally, one should - after CALC_ELEM and CALC_NO - re-project the results, calculated for the latter mesh, onto the original mesh (which is the one contained in Salome). This is done with command PROJ_CHAMP.
Look onto the Template /opt/helpers/Templates/LinStatics3DQuad.comm contained in CAELinux.

Apart from the ALARM-message, You don't write clearly, if You get (and can visualize) results in Salome or not. I am interested to know it, and if yes, are they the same as You get following the way outlined above (PROJ_CHAMP)?

Moreover, I don't see any parameter (SUP or INF) in Your CALC_ELEM determining if You calculate top or bottom stress of Your elements. I have never used COQUE_3D-elements. Do they have several nodal stress locations (top, bottom, center) or at which location do You get the nodal stress?

Regards, Johannes Ackva

Please Log in or Create an account to join the conversation.

  • Kees Wouters
  • Kees Wouters's Avatar Topic Author
  • Offline
  • Moderator
  • Moderator
More
11 years 4 months ago #2691 by Kees Wouters
Beste Johannes

Your mesh in Salome is one with QUAD8-elements, named &quot;meshinit&quot; in .comm. You created a new mesh with QUAD9-elements. You calculated this new mesh. This means that nodal results exist at all the 9 nodes of each QUAD9-element of the new mesh. Then You write all nodal results in a results-file in .MED-format for beeing read by Salome. So there is a discrepancy: Salome doesn't know 9 nodes per element, but only 8 nodes. That is the reason for the ALARM message.

Normally, one should - after CALC_ELEM and CALC_NO - re-project the results, calculated for the latter mesh, onto the original mesh (which is the one contained in Salome). This is done with command PROJ_CHAMP.
Look onto the Template /opt/helpers/Templates/LinStatics3DQuad.comm contained in CAELinux.


I will have a look at &quot;LinStatics3DQuad.comm&quot;. At the moment I cannot find it, maybe because I didnot do a standard install. Salome has been installed in /home/..../salome/... and I cannot find the file here. Maybe I am looking at the wrong place.
I try to have a look at the PROJ_CHAMP command and implement it anyway.

Apart from the ALARM-message, You don't write clearly, if You get (and can visualize) results in Salome or not. I am interested to know it, and if yes, are they the same as You get following the way outlined above (PROJ_CHAMP)?

After the error message at importing the result file nothing happens in Salome. The results are not displayed and unfortunately I won't be able to compare them with the PROJ_CHAMP results.

Moreover, I don't see any parameter (SUP or INF) in Your CALC_ELEM determining if You calculate top or bottom stress of Your elements. I have never used COQUE_3D-elements. Do they have several nodal stress locations (top, bottom, center) or at which location do You get the nodal stress?

In the tutorial three .comm files have been provided for calculating the three layers: central and outside layers (feuilleut moyen, -superieure and - inferieure). Again, I am not sure whether you have to calculate these three cases for obtaining the seperate results. I will re-read the tutorial again.

kind regards - kees<br /><br />Post edited by: Kees Wouters, at: 2009/03/15 19:36

Interest: structural mechanics, solar energy (picture at 'my location' shows too little pv panels)

--
kind regards - kees

Please Log in or Create an account to join the conversation.

  • Kees Wouters
  • Kees Wouters's Avatar Topic Author
  • Offline
  • Moderator
  • Moderator
More
11 years 4 months ago #2700 by Kees Wouters
Good day to you all.

Now I can read the results into Salome using the PROJ_CHAMP command. So part of the question has been solved.
The following code has been used to project the various fields from the 'shell-elements' back to 'Salome-elements':

[code:1]
result=CALC_ELEM(reuse =result,
MODELE=modmod,
CHAM_MATER=material,
RESULTAT=result,
OPTION=('SIGM_ELNO_DEPL','EQUI_ELNO_SIGM',),
EXCIT=_F(CHARGE=Load1,),);

result=CALC_NO(reuse =result,
RESULTAT=result,
OPTION=('SIGM_NOEU_DEPL','EQUI_NOEU_SIGM',),);

salomres=PROJ_CHAMP(RESULTAT=result,
MODELE_1=modmod,
MODELE_2=modinit,);

IMPR_RESU(FORMAT='MED',
UNITE=81,
RESU=_F(MAILLAGE=meshinit,
RESULTAT=salomres,
NOM_CHAM=('SIGM_NOEU_DEPL','EQUI_NOEU_SIGM','DEPL',),),);
[/code:1]

The important part -for me- was the new file creation (unite 81) that can be done by ASTK. A part of the resulting *.export file by adding the appropriate files at ASTK:
F mail kees@localhost:/home/kees/catv/shell12.med D 20
F comm kees@localhost:/home/kees/catv/shell12.comm D 1
F resu kees@localhost:/home/kees/catv/shell12.resu.med R 8
F mess kees@localhost:/home/kees/catv/shell12.mess R 6
F erre kees@localhost:/home/kees/catv/shell12.erre R 9
R base kees@localhost:/home/kees/catv/shell12.base R 0
F mmed kees@localhost:/home/kees/catv/res12.med R 81

And then you can import the res12.med file into Salome. The displacements look fine. Regarding the stresses I still have to look what and where they are exactly defined.
So Johannes, I still need to do some further work. And thank you for guiding me to
* the PROJ_CHAMP command and
* the new file creation in ASTK in the ''Recover deformed mesh'' post. BTW: should I be using UNITE 21 for med files?

I will include the *.comm and *.med files and remove the faulty ones.

kind regards - kees

Attachment shell12.gz not found

<br /><br />Post edited by: Kees Wouters, at: 2009/03/18 14:57

Interest: structural mechanics, solar energy (picture at 'my location' shows too little pv panels)

--
kind regards - kees
Attachments:

Please Log in or Create an account to join the conversation.

  • Kees Wouters
  • Kees Wouters's Avatar Topic Author
  • Offline
  • Moderator
  • Moderator
More
11 years 4 months ago #2729 by Kees Wouters
Dear all

just following my own post, I have run some simulations to test my comm file and the accuracy of dynamics of the coque_3d elements.
A rectangular steel plate with dimensions 1.0*0.7*0.001 m3 has been simulated. All four boundaries of the plate are hinged.
Comparing the first five analytic (Fth) to the numerical (Fnum) results [Hz] and percentual differences gives the following table:

[code:1]
shape Fth Fnum dif %
1*1 7.429 7.425 -0.054
1*2 14.757 14.751 -0.041
2*1 22.389 22.381 -0.036
1*3 26.974 26.963 -0.041
2*2 29.715 29.702 -0.044
[/code:1]

Analytical results according to G.B. Warburton, the vibration of rectangular plates, 1954.

If someone would like to have a glance at the files, pls feel free.

Attachment shell33.gz not found

<br /><br />Post edited by: Kees Wouters, at: 2009/03/26 18:23

Interest: structural mechanics, solar energy (picture at 'my location' shows too little pv panels)

--
kind regards - kees
Attachments:

Please Log in or Create an account to join the conversation.

More
11 years 4 months ago #2734 by Claus
thank you for posting the files - I hope that encourages others to do the same :)

Code_Aster release : STA11.4 on OpenSUSE 12.3 64 bits - EDF/Intel version

Please Log in or Create an account to join the conversation.

Moderators: catux
Time to create page: 0.120 seconds
Powered by Kunena Forum