your answer to my question is great, as always! In fact I was already thinking about the possibility to neglect the shear stresses because the dimension of my geometry is 10^5 times 10^5 times 10^1, i.e. indeed it is very thin compared to the other dimensions.

I thank you for pointing out the FORTRAN file that I have to modify in order to use ELAS_HYPER on shells. I will try that with my model and hope the best.

Thanks again and please be sure that I'll give feedback concerning this topic.

Ralf

[EDIT] The changes that you suggested work also in my case. Starting from this I will implement another nonlinear material and use it within the shell formulation. Thanks to the Code_Aster developers for the excellent documentation that explains how to implement a new material.

]]>In fact it might be possible to use hyperelasticity in COQUE_3D with a few minor modifications as well as some drawbacks. The main reasons (software speaking) why ELAS_HYPER is not available are :

- it cannot be used in COMP_ELAS because it is not implemented at all. Only linear elasticity is.

- it cannot be used in COMP_INCR because the shear stresses are treated linearly in plates/shells in Code_Aster (e.g. non-linear shear theory is not implemented). That means that one requires a Shear modulus which is obtained from Young Modulus and Poisson ratio to compute SIXZ and SIYZ components of the stress tensor (SIXZ=G*kappa*GammaXZ). Since ELAS_HYPER does not provide them, the code stops.

Therefore 2 solutions may enable to use ELAS_HYPER with COQUE_3D :

- renounce to large strains so that the shear modulus G=2*(C01+C10). But large strains are usually expected with hyperlasticity

- neglect shear stresses or use a shell where thickness is small compared to dimensions. In this case shear stresses may be ignored and ELAS_HYPER should be used with COQUE_3D.

The first solution seems to work (at least I'm able to run a test case) but more testing should be made and as already said by AsterO'dactyle finite deformations is what matters for hyperelasticity.

If one wants to trick with that, the subroutine to modify is vdpnlr.f :

```
232 IF (PHENOM.EQ.'ELAS') THEN
233 NBV = 2
234 NOMRES(1) = 'E'
235 NOMRES(2) = 'NU'
236 ELSE
237 CALL U2MESS('F','ELEMENTS_42')
238 END IF
734 IF (PHENOM.EQ.'ELAS') THEN
735 NBV = 2
736 NOMRES(1) = 'E'
737 NOMRES(2) = 'NU'
738 ELSE
739 CALL U2MESS('F','ELEMENTS_42')
740 END IF
```

The code that makes Aster stops.

` 745 CISAIL = VALRES(1)/ (1.D0+VALRES(2))`

The value of the shear modulus G (2*G more precisely here).

TdS

]]>Many thanks to both of you, you successfully eliminated my confusion

@Johannes Ackva: You advised me to have a look at chapter 7 and indeed - don't know why - I didn't read the section 7.2 carefully enough. From this section it is clear that only elastic material is applicable.

The fact that there "isn't any finite deformation formalism in the plates/shells in Code_Aster" (AsterO'dactyle) is quite a heavy limitation to my work. Do you know why this limitation exists? I only ask because I want to check how to proceed in the best way. Is it very complicated to integrate finite deformations for shells into the code in general or is it just not in the scope of the developers of Code_Aster because this case (maybe) is not that important for their applications?

Have a nice day,

Ralf

The two:

- it's very complicated to integrate finite deformations for shells

- it's not in the scope of the developers of Code_Aster because this case is not that important for their applications

@Johannes Ackva: You advised me to have a look at chapter 7 and indeed - don't know why - I didn't read the section 7.2 carefully enough. From this section it is clear that only elastic material is applicable.

The fact that there "isn't any finite deformation formalism in the plates/shells in Code_Aster" (AsterO'dactyle) is quite a heavy limitation to my work. Do you know why this limitation exists? I only ask because I want to check how to proceed in the best way. Is it very complicated to integrate finite deformations for shells into the code in general or is it just not in the scope of the developers of Code_Aster because this case (maybe) is not that important for their applications?

Have a nice day,

Ralf

]]>Mon message !!!!!!]]>

There isn't any finite deformation formalism in the plates/shells in Code_Aster

GROT_GDEP is posslble for large rotation/translation but small deformation

The same name of "GROT_GDEP" has been choosen for ELAS_HYPER but GROT_GDEP for ELAS_HYPER is for finite deformation.

That's quite confuzing.

Johannes Ackva

______________________________________________________________________

Ingenieurbüro für Mechanik

Dr.-Ing. Johannes Ackva

Markgrafenstr. 21

D 91717 Wassertrüdingen

*** Next Intro Course to Salome and Code-Aster: 26th to 30th of September in Göteburg ***

*** informations at Tel 0049 9832 708152

*** registration at www.simdi.se/web/guest/code-aster-training

I think what You want is not possible. Look to Dok U4.51.11:

4.3.1.2 'ELAS_HYPER'

Relation de comportement hyper-élastique incrémentale : elle permet de prendre en compte des

déplacements et contraintes initiaux donnés sous le mot clé ETAT_INIT. Les données nécessaires du

champ matériau sont fournies dans l'opérateur DEFI_MATERIAU [U4.43.01], sous le mot clé

ELAS_HYPER. Cette relation n'est supportée qu'en grandes déplacements, rotations et grandes

déformations (DEFORMATION='GROT_GDEP') cf.[R5.03.23].

Modélisations supportées: 3D, D_PLAN, C_PLAN

Nombre de variables internes : 1

Signification : V1 : vide donc vaut toujours zéro

Exemple : voir test SSNV187.

I must admit that I have not yet studied the doc R3.07.04 and ..05 which You nominate, so I cannot resolve the contradiction which You speak about.

Johannes Ackva

______________________________________________________________________

Ingenieurbüro für Mechanik

Dr.-Ing. Johannes Ackva

Markgrafenstr. 21

D 91717 Wassertrüdingen

*** Next Intro Course to Salome and Code-Aster: 26th to 30th of September in Göteburg ***

*** informations at Tel 0049 9832 708152

*** registration at www.simdi.se/web/guest/code-aster-training

I am a little bit confused concerning this topic and need some help. In the introduction of the document R3.07.04 "Eléments finis de coques volumiques" I read: "Aucune restriction n'est faite sur le type de comportement en contraintes planes.". Of course in this document the model is restricted to small displacements and small deformations and for this case hyperelastic material is reasonably not applicable.

But there is another document that describes the capabilites concerning geometrical nonlinearities of shell elements: R3.07.05. As I understood after the lecture of these 2 documents and the documents concerning C_PLAN, ELAS_HYPER and COQUE_3D it should be possible to apply hyper-elastic material (ELAS_HYPER) for large displacements, large rotations and large deformations (GROT_GDEP) to the model COQUE_3D. Nevertheless if I try to run a problem with two shells being in contact, where one of the shells is linear elastic and the other is hyperelastic, I get the exception (please find the mess file attached):

```
!----------------------------------!
! <EXCEPTION> <ELEMENTS_42> !
! !
! comportement matériau non admis !
!----------------------------------!
```

Now I think that I understood something wrong or that I did not read the documents carefully enough. Is it not possible to use hyper-elastic material for shells?

Thanks a lot for your replies,

Ralf

]]>