Large contact problem

Hello all,

This time it is a bit of a marathon post - so bear with me...

I am currently trying to model in which 35 parts (yikes!) are to be joined together in a structure. All components are copies of three different original geometries (translated and/or rotated).

Using Salomé, I tried to combine the parts using a boolean operation, but the resulting mesh was far too large. Instead I have now meshed the three original parts separately, copied them and and joined them in a compound of meshes (just over 1e6 volumes in all ~ 86MB ). The compound structure looks something like:

Compound:
--Groups of faces:
----Group 1
----Group 2
----Group 3
----Group 4
----Group 5
----Group 6
--Groups of volumes:
----Group 1
----Group 2
----Group 3

The contacting faces have been made into groups and the different meshes have been put into groups of volumes.

To summarize the problem, I have done a quick schematic as can be seen below.



As seen, each contact between meshes is repeated several times.

I am trying to figure out the following before venturing forth:

My approach has been to merge the groups of faces that belong to the "same" contact (all group 1 faces for instance). My hope is that this merged group can be used as slave for all contacts of that type, and that this can be coupled to merged group functioning as master. In that case I would only need to call that contact once.

Is this a valid approach or do i need to model each contact separately? (I sure hope not )

BTW: I am completely new in using contacting meshes; is it a necessity to use a non-linear analysis?

Thank you in advance for your input!

Best regards,

Jakob

Post edited by: Jakob Andersen, at: 2010/01/11 19:45

Post edited by: Jakob Andersen, at: 2010/01/11 21:14<br /><br />Post edited by: Jakob Andersen, at: 2010/01/11 21:14

1) yes, You need nonlinearity

2) Grouping: I m not shure if I understand well what You explain. Principally, for each pair of contacting bodies, You need one master and one slave group (of face elements). But things can be treated very flexibly: For example You could even make the skin elements of both blue volumes and of all 5 green volumes be one (and the only) master group. And make the skin elements of all red volumes one other group which is the slave group. So You would have only one master and one slave group. But does this make sense? For postprocessing it will be more convenient to make several pairs of groups: it enables You much easier to calculate the contact force between a couple of bodies. And it enables You to adjust numerical parameters, contact methods and so on for the several contact pairs individually.

Regards, Johannes Ackva

______________________________________________________________________
Ingenieurbüro für Mechanik 708152
Dr.-Ing. Johannes Ackva
Markgrafenstr. 21
D 91717 Wassertrüdingen

www.code-aster.de
Training &amp; Support for NASTRAN and CODE-ASTER<br /><br />Post edited by: johannes ackva, at: 2010/01/12 01:04

Hello Johannes,

Thank you for your reply. Maybe the question was a bit unclear, but it was definitely answered!

Indeed, it would be nice to have each contact described, but if I have counted correctly, the 35 components have 81 pairings in all. I will definitely look into a more detailed model at a later point, but for now, the simplified version will do - my focus is on the behaviour of the entire structure.

...and also; I have to keep it simple, as I am in no way a seasoned code_aster user.

Best regards,

Jakob

81 is no problem, because it is very simple to generate code like this:

Contact=AFFE_CHAR_MECA(MODELE=FEMLin,
CONTACT=(
_F(GROUP_MA_MAIT='C1_MAS',
GROUP_MA_ESCL='C1_SLA',),
_F(GROUP_MA_MAIT='C2_MAS',
GROUP_MA_ESCL='C2_SLA',),
_F(GROUP_MA_MAIT='C3_MAS',
GROUP_MA_ESCL='C3_SLA',),

and so on, 81 times

You can also do it creating several contact definitions, which enables You to activate or deactivate contacts, including or excluding them in the solver-command:

Cont_1=AFFE_CHAR_MECA(MODELE=FEMLin,
CONTACT=(
_F(GROUP_MA_MAIT='C1_MAS',
GROUP_MA_ESCL='C1_SLA',),
_F(GROUP_MA_MAIT='C2_MAS',
GROUP_MA_ESCL='C2_SLA',),

and so on

Cont_2=AFFE_CHAR_MECA(MODELE=FEMLin,
CONTACT=(
_F(GROUP_MA_MAIT='C3_MAS',
GROUP_MA_ESCL='C3_SLA',),
_F(GROUP_MA_MAIT='C4_MAS',
GROUP_MA_ESCL='C4_SLA',),

and so on


Creating lots of groups can be cumbersome. So You must do it in an intelligent way. When You make Compound meshes in Salo there are several ways how the groups of the input meshes are treated for the output Compound mesh. Your should have a close look to the options.

There is also DEFI_GROUP in Code-Aster to define groups during the run. It has geometrical criteria, Boolean criteria and so on which merits a deep look

Regards, Johannes Ackva

______________________________________________________________________
Ingenieurbüro für Mechanik 708152
Dr.-Ing. Johannes Ackva
Markgrafenstr. 21
D 91717 Wassertrüdingen

www.code-aster.de
Training &amp; Support for NASTRAN and CODE-ASTER<br /><br />Post edited by: johannes ackva, at: 2010/01/12 11:13

Hi again,

I have tried to implement a simple version using one single contact for all part interfaces - this would enable me to borrow most of the .comm file written by Claus Andersen ( www.caelinux.org/wiki/index.php/Contrib:Claws/Code_Aster ).

My mesh (a rotor for a wind turbine) essentially looks like this:

rotor
--Groups of faces
----master
----slave
----b1
--Groups of volumes
----tri_nth
----tri
----prof
----prof120
----prof240
----cutprt
----rectend

Collectively, the groups of volumes account for the entire mesh.

To this .comm file I have added rotation and gravity following the instructions Kees Wouters gave me in another post a few days ago.

Most of the syntax seems to be in order, but I get an error message (see attached .mess and .erre files):

End of .mess file:

[code:1]JDC.py : ERREUR A L'EXECUTION - INTERRUPTION
&gt;&gt; JDC.py : DEBUT RAPPORT
CR d'execution de JDC en MIXTE
!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
! &lt;S&gt; Exception utilisateur levee mais pas interceptee. !
! Les bases sont fermees. !
! error : &lt;EXCEPTION LEVEE&gt; DVP_1 !
!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
fin CR d'execution de JDC en MIXTE

&gt;&gt; JDC.py : FIN RAPPORT
EXECUTION_CODE_ASTER_EXIT_10545=1

&lt;F&gt;_ABNORMAL_ABORT exit code = 1[/code:1]

from .erre file:

[code:1]!

---

!
! &lt;E&gt; &lt;CALCULEL2_73&gt; !
! !
! !
! on n'a pas pu extraire toutes les cmps voulues du champ associé au paramètre: PMATERC !
! - option: CHAR_MECA_PESA_R !
! - type_element: MECA_TETRA10 ) !
! !
! !
! !
! Cette erreur sera suivie d'une erreur fatale. !
!

---

!


!

---

!
! &lt;F&gt; &lt;DVP_1&gt; !
! !
! !
! Erreur de programmation : condition non respectée. !
! !
! !
! !
! Cette erreur est fatale. Le code s'arrete. !
! Il y a probablement une erreur dans la programmation. !
! Veuillez contacter votre assistance technique. !
!

---

!

&lt;S&gt; ERREUR UTILISATEUR RECUPEREE PAR LE SUPERVISEUR
&lt;I&gt; &lt;FIN&gt; FERMETURE DE LA BASE &quot;GLOBALE&quot; EFFECTUEE.
&lt;I&gt; &lt;FIN&gt; ARRET NORMAL DANS &quot;FIN&quot; PAR APPEL A &quot;JEFINI&quot;.
&lt;I&gt; FERMETURE DES BASES EFFECTUEE

&lt;F&gt;_ABNORMAL_ABORT exit code = 1[/code:1]

I have tried to look for a similar error message here, in the Code_aster forum and by googling. I have yet to find a solution...

Any ideas on what's happening?

Thanks again

Jakob Andersen

I suppose You didn't include all 3D elements of Your 3D Modele in the material assignment (AFFE_MATERIAU). Johannes Ackva