Hi,

Assuming you are using Salome, just partitioning your geom,
mesh it as one whole (this makes fully conformal mesh on all internal faces of the partitioned geometry),
then use the Duplicate Nodes or/and Elements from the menu Modification->Transformation.
Either the 1st or the 4th option could work, but require different preparation (grouping) and post treatment (re-merging of some nodes).

This process will result fully identical element shapes and node location on the both sides of your interface, but with duplicated nodes! The rest of your mesh is fully merged.

BR.
dezsit

Dear Anirudh,

Your question of course absolutely valid, and can be defined such behavior in aster.
A similar one is shown by Johannes Ackva (code-aster/dot/de), using the DIS_CONTACT material "behavior".

In the attached small example I used grounded springs (POI1). We need two of them connected parallel, one for the tension, one for the compression. The key is that the local csys (REPERE='LOCAL") should be opposite (ORIENTATION in AFFE_CARA_ELEM).
In this example we have stiffness equal to 1(force/displacement) in tension and 10 in compression. You can check it with xmgrace (res.func) or numerically (res.tab).

The line spring (SEG2) works similarly.

I would not say it will work in all cases, but in this simple one it provides the expected result. Tweeking with the parameters (eg. JEU in DEFI_MATERIAU) and combining other springs, very different characteristics can be achieved.

Regards,
dezsit

Hi,

at this moment, if you create group by DEFI_GROUP, asterStudy does not recognize it, since it will be available during run time only. (I guess it could be handled, maybe in the future releases).
So you should put manually the new names at the bottom of the group selection widget (Manual selection) to use it.

Best regards,
dezsit

Hi,

you can manage it with one file, just put all your resulting fields (DKT,3D,...) into one IMPR_RESU.

Then in paraVis, open the resulting med twice (or more, depending on the study), and select your 3D fields on one of the result file, than the 2D fields on the other result file.
See the attached picture,
here you can see mech.rmed file opened twice (it is one file from one IMPR_RESU),
on the first file I selected the 3D results: reslin_SIEQ_NOEU from ComSup2 in the selection window on the left bottom,
then on the second file I selected the DKT results, here the TOP____SIEQ_NOEU 8which contains the equivalent stresses on the top side of my shell),
Then visualized both together (VMIS filed on both) with adjusting the scales.

You can do that for any kind of combination (eg with beams or what ever), just sometimes a good visualization requires more tweeking in paraVis.

Best regards,
dezsit

Hi,

Warp by Vector can do that, but you need a real vector with 3 elements!
In case of beams you have 6 in the DEPL filed: 3 translation 3 rotation, so you should produce a real vector from that.
You have two options to do that
1) the easy way: when you open your med file and select your filed (e.g. depl of course) , you have to tick the checkbox "Generate vectors"  (just below the field selection window). This will generate a new DEPL field (DEPL_Vector or something) what will contain the 3 necessary directional displacements, and can be used by Warp filter

2) the manual way: use the calculator filter, then apply the following expression: ihat*DX + jhat*DY + khat*DZ (DX,DY,DZ is the scalars of your DEPL filed),
this will produce a new vector field with 3 components under the name you provides in the Calculator filter (by default it is Result).

Note: you should use one of the option in any case where the DEPL field contains more than 3 directional displacement, so e.g. in case of shells, or if you use contacts.

Best regards,
dezsit

Hello,

I think the problem is, that you extracted the "extrema" of the displacement DZ with this:

table2 = POST_RELEVE_T(ACTION=_F(OPERATION=('EXTREMA', ),
                                   INTITULE='DZ',
                                   RESULTAT=linel,
                                   NOM_CHAM='DEPL',
                                   PRECISION=1.E-06,
                                   CRITERE='RELATIF',
                                   FORMAT_C='MODULE',),
                         INFO=1,)

This produce not only one DZ value (as necessary for OpenTurns) but four, and actually not simply 'DZ':
#
#--------------------------------------------------------------------------------
##ASTER 14.04.00 CONCEPT table2 CALCULE LE 18/06/2020 A 16:57:37 DE TYPE         
#TABLE_SDASTER                                                                   
INTITULE         RESU     NOM_CHAM         NUME_ORDRE   INST         EXTREMA  NOEUD    CMP      VALE       
DZ               result   DEPL                        1  0.00000E+00 MAX      N98      DZ        6.39285E-02
DZ               result   DEPL                        1  0.00000E+00 MIN      N134     DY       -1.00000E+00
DZ               result   DEPL                        1  0.00000E+00 MAXI_ABS N134     DY        1.00000E+00
DZ               result   DEPL                        1  0.00000E+00 MINI_ABS N52      DX        0.00000E+00

So, that is way a warning reported in the message file:
   ! Parametre absent de la table : DZ.   

So you should try this:

#all dz value extracted from the node group 'Group_1' or whatever into the table
table2 = POST_RELEVE_T(
  ACTION=_F(
    GROUP_NO=('Group_1', ),
    INTITULE='DZ',
    NOM_CHAM='DEPL',
    NOM_CMP=('DZ', ),
    OPERATION=('EXTRACTION', ),
    RESULTAT=result
  )
)

#then it is filtered (only maximum absolute -> MAXI_ABS) during the numpy table creation, so you have only one value at the end.
IMPR_TABLE(
  FILTRE=_F(
    CRIT_COMP='MAXI_ABS',
    NOM_PARA='DZ'
  ),
  FORMAT='NUMPY',
  NOM_PARA=('DZ', ),
  TABLE=table2,
  UNITE=8
)

I did not tried with OpenTurns, but it eliminates the warning, so should work.

Best regards,
dezsit

Just to note:

It does not worked to me either, if I try with SalomeMeca2019 (same error as yours)
but the salome shell method works with the native Salome platform (eg. 9.4) and also with older version of salome meca (eg. 2018). Interesting.

The problem is, if you start the paraview in your way, the MEDloader plugin won't be loaded.
In case of salome shell way, you get a standalone paraview with the capability to handle MED files.

Regards,

Up!

Hi, could somebody from the developers comment that we can expect an updated version with OpenTurns?

Thank you and
Best regards,
dezsit

Hello,

Generally, hex outperforms tetra in mechanics (better mesh convergence with less elements), especially if bending involved. But in some cases hex suffers from various problems (volumetric locking, hourglassing, etc, depending on the numerics behind a specific hex formalism (reduced integration, full integration but linear element, etc.), and how a specific fea package handles this kind of problems (eg. assumed strain as in case of aster) ), you should check the element reference manual of a software package, and do verifications! But sometimes the geometry does not allow to make good hex mesh (or simply the job not worth to spend too much time with mesh preparation) so tetra can be used, but only quadratic for mechanics, and again do verification and mesh convergence study.

Code_aster fatigue case: as I mentioned the fea part of fatigue is "simple" mechanics (statics, dynamics), not aster specific. We do the fatigue evaluation separately, independently from the fea package, so I cant provide an aster specific fatigue evaluation (knowing that aster has in-built fatigue evaluation tool, but we have not used it yet).

BR
dezsit

Hi,

I am not sure python can handle environment variables (from shell) in this way (I suppose the dump.py thrown the exception of your try/except condition), it is more complicated I think, you cannot pass variable from shell to python script in this way especially because the dump.py is executed by salome session and not by the shell. But to be honest I never tried it. If you follow my example I gave you in an other post, the param dict file can handle this simply (as it is already done in the 144 line of salomeScript.py).

BR
dezsit

Hi,

you have to create 0D elements (POI in aster) on the nodes, where you want to apply mass element, then use DISCRETE element modelisation on these 0D elements. (more keywords: AFFE_MODELE->DIS_T, AFFE_CARA_ELEM->DISCRETE->M_T_D_N)

Check Jean Pierre Aubry's excellent book: framabook.org/beginning-with-code_aster/, eg. you will find an example on the 31.page.

BR
dezsit

Hello,

hex mesh: yes, for example. You can produce with this a fully structured hex mesh, but will be hard to make the connecting regions properly partitioned and to provide equal mesh seeding on the opposite edges of a block. Really a lot of work.
The solution, what I proposed on my sketch, is giving you more freedom, you can use sweeping techniques (Extrude3D in salome) which not necessarily produce structured mesh, and not necessarily produces full hex mesh (it can, but sometimes some wedges will be also generated), but it definitely will produce tetra free mesh. And with less work, and giving more freedom to change the local mesh density.

FKM: yes, that is what the referenced paper about. You can check it also here for example: vdmashop.de/Research--FKM-/

BR,
dezsit