Contrib:KeesWouters/nlgeom

nlgeom1

   *  » Code_Aster usage
   *  » Non linear geometry on Code-Aster

Non linear geometry on Code-Aster

Hello, is possible activate non linear geometry on Code-Aster solver? There is a command (for example in ABAQUS there is NLGEOM=YES and the sw update stifness matrix step by step) to doing it? To activete it needed use some particular 3D element?

Regards Jacopo

AlexD

Re: Non linear geometry on Code-Aster

NLGEOM in abaqus is unabled when dealing with hight strains and high displacements / rotations.

You can do it as well in Aster using the GREEN or (depending on the behaviour law ... ) SIMO_MIEHE for the strains tensors.

Thomas DE SOZA ==> In Code_Aster, geometrically (exact) non-linear analysis has to be enabled by hand depending on the type of finite element :

• with isoparametric elements (D_PLAN,C_PLAN and 3D) you can use DEFORMATION='GREEN' to enable large displacements (including large rotations). Note that constitutive law is still written with a small strain hypothesis. Any constitutive law available under COMP_INCR can be used. Under COMP_ELAS, you can use ELAS_VMIS_* and ELAS_HYPER (non-linear elasticity and hyperelasticity).

• with 3D shell elements (COQUE_3D), the same is enabled when selecting GREEN_GR (with constitutive law ELAS under COMP_ELAS, that is only linear elasticity can be used when dealing with large displacements/rotations).

• with beam element POU_D_T_GD, you must use GREEN_GR (with constitutive law ELAS_POUTRE_GR under COMP_ELAS, that is only linear elasticity can be used).

• with bar element CABLE, you must use GREEN (with constitutive law CABLE under COMP_ELAS, that is only linear elasticity can be used).

==> In addition to that, Code_Aster provides imprecise approaches to take into account large displacements/rotations :

• for most of the finite elements one can use PETIT_REAC which updates the geometry at each iteration before computing the stiffness matrix, depending on the element it can be really hard to reach convergence (really slow).
• for POU_D_TGM element (a multi-fiber beam element), one can use DEFORMATION='REAC_GEOM' to help converge when large displacements and large rotations occur.

==> Lastly, the most complete kinematic and constitutive behavior in Code_Aster is through the use of DEFORMATION='SIMO_MIEHE' (for isoparametric elements) which computes accurately the transformation gradient.

TdS

AlexD

""Note that constitutive law is still written with a small strain hypothesis. Any constitutive law available under COMP_INCR can be used.""

Don't you can use comp_elas as well ? In this case (for hyperelasticity for example) the stress tensor will be calculated regarding to the problem initial configuration and high strains can be considered through the Green Lagrange strain tensor. Well it remembers me one post .... http://www.code-aster.org/forum2/viewto … 09&p=2

Thomas DE SOZA Hi,

You're right, I modified my post to reflect your remarks.

TdS Jacopo

Thx Paul Thomas and Alex for help, now I asking you about a little summary about COMP_INCR and COMP_ELAS definition, I not sure to understand so well the differences. The COMP_ELAS to calculate the strain take as reference situation the indeformed shape (initial condition)? The COMP_INCR to calculate the starin take as reference the reactualizated geometry step by step? When is better use one instead other one? Other things, If I understand yuo said me that with 3D eleemnt you can use Green formulation to have a correct behaviuor for large rotation and large displacement.On the guideline I read that the green formulation give correct behaviour for big rotation but small displacement, it is true? To have correct behaviour for big roation and big displacement the best formulation appare Simo_miehe.

Regards Jacopo

Thomas DE SOZA

   Jacopo wrote:

   On the guideline I read that the green formulation give correct behaviour for big rotation but small displacement, it is true?
   To have correct behaviour for big roation and big displacement the best formulation appare Simo_miehe.
   Jacopo

Which guidelines are you talking about ?

'GREEN' (meaning the strain tensor is Green-Lagrange) correctly models large displacements and large rotations but with the hypothesis of small strains (see in french R5.03.22).

Remember :

small displacements implies small strains (which is often summed up as small perturbations) however small strains does not imply small displacements

TdS

Jacopo

Thomas, you have rigth as soon as possible I send you where I read what I said you on previous post (probabbly I made a mistake...), about what you said me I think that you wont said me something similar the simple example on file attched. On case 2 if I have a big perturbation I heve big strain too, so I must use SIMO_MIEHI formulation.

Jacopo I make a mistake you have rigth I'm refferring to U.4.51.11-B1....You can explene better the differencies between COMP_INCR and COMP_ELAS?

Regards and Thx again Jacopo

Paul CARRICO

May be I'm mistaken but : -COMP_INCR => typically plastic calculation ... plastic calculation are calculated from plastic flow -COMP_ELAS => Contact calculation i.e. elastic material and geometrical non linearity

PC

Thomas DE SOZA COMP_ELAS : linear and non-linear elasticity. History of loading does not impact behavior, stress are related to (strains regarding a reference setup) ==> splitting the load into several parts is theorically not necessary. However the non-linearity is more easily solved when cutting it, that's why "temporal" discretization is also used as in COMP_INCR (where it is mandatory).

COMP_INCR : general constitutive equation (non-linear). History accounts for the constitutive equation. Incremental stresses are related to incremental strains (regarding last equilibrium setup). History is stored through internal variables (at each Gauss points).