Atom topic feed | site map | contact | login | Protection des données personnelles | Powered by FluxBB | réalisation artaban

You are not logged in.

- Topics: Active | Unanswered

Pages: **1**

**toltec****Member**- Registered: 2009-01-04
- Posts: 94

Hello,

I'm trying to get output from a COQUE_3D, STAT_NON_LINE (elastic-plastic) analysis:

1) equivalent plastic strain (at nodes and integration points) for Salome display

2) equivalent plastic strain at the integration points (& section integration points, using Abaqus terminology) for printing to .resu

I have no problem getting the Mises stresses, but am battling with PEEQ. Any pointers would be appreciated!

Gary

Ubuntu 12.04

Intel(R) Core(TM)2 Quad CPU Q9400 @ 2.66GHz

Offline

**toltec****Member**- Registered: 2009-01-04
- Posts: 94

Hi All,

I put a lot of effort into searching the documentation (thank you google translate!) but don't seem to be able to find how to extract the equivalent plastic strain at COQUE_3D integration points for a non-linear analyses. At times CALC_ELEM TYPE_OPTION looked promising but alas no...

Am I waisting my time or is my quest possible?

Regards

Gary

*Last edited by toltec (2011-03-02 21:55:21)*

Ubuntu 12.04

Intel(R) Core(TM)2 Quad CPU Q9400 @ 2.66GHz

Offline

**pierre_j****Member**- Registered: 2010-01-19
- Posts: 773

Hi Toltec,

In my understanding of integration point management in shell section, you should:

1) In AFFE_CARA_ELEM define your number of integration points using the option COQUE_NCOU (**COU**che in french is layer in english).

What is not clear in my mind is which integration method is used for element section integration?

In other solvers, it has usually an impact on number of layers you can define... Something like (example for 3 layers):

```
CARA=AFFE_CARA_ELEM(MODELE=MODEL,
COQUE=_F(GROUP_MA='plaque',
EPAIS=1.022,
ANGL_REP=(0.,0.,),
COQUE_NCOU=3,),);
```

2) Then, for "adequate" post-processing, you should define one CALC_ELEM per integration point (or layer in Aster terminology), something like (example for 3 integration points):

```
PLY1=CALC_ELEM(RESULTAT=RESU,
REPE_COQUE=_F(NUME_COUCHE=1,
NIVE_COUCHE='MOY',),
OPTION=('SIEF_ELNO_ELGA','EPSI_ELNO_DEPL',),);
PLY2=CALC_ELEM(RESULTAT=RESU,
REPE_COQUE=_F(NUME_COUCHE=2,
NIVE_COUCHE='MOY',),
OPTION=('SIEF_ELNO_ELGA','EPSI_ELNO_DEPL',),);
PLY3=CALC_ELEM(RESULTAT=RESU,
REPE_COQUE=_F(NUME_COUCHE=3,
NIVE_COUCHE='MOY',),
OPTION=('SIEF_ELNO_ELGA','EPSI_ELNO_DEPL',),);
IMPR_RESU(FORMAT='MED',
RESU=(_F(RESULTAT=PLY1,),
_F(RESULTAT=PLY2,),
_F(RESULTAT=PLY3,),
_F(RESULTAT=RESU,),),);
```

For a "possible" understanding (not validated by someone from EDF team) of the NIVE_COUCHE option in CALC_ELEM, we exchanged with Todd in this post a meaningful picture.

If someone from EDF team happens to read this post, I will be glad to give you all the rights required for this picture be included in the documentation of CALC_ELEM :-).

Toltec, hope this helps you.

Have a good day!

Bests,

Pierre

*Last edited by pierre_j (2011-03-03 08:26:33)*

Offline

**toltec****Member**- Registered: 2009-01-04
- Posts: 94

Hello Pierre,

Thank you very much for your useful post. I'll go through it carefully as it seems my understanding of Aster's COQUE_3D intergration and section points (to use Abaqus terminology) is not yet where it should be.

My original question still stands... is it possible to calculate and write the integration point *equivalent plastic strain* (and Mises stress for that matter) to text and .med files? I want to do this to ensure that mises stresses and equivalent plastic strains are consistent with the plastic strain curve implied in the material model. This must be done at integration points where material calculations are done as extrapolated nodal values will be misleading.

I'm beginning to think that this may not be possible.

Regards

Gary

*Last edited by toltec (2011-03-03 20:30:54)*

Ubuntu 12.04

Intel(R) Core(TM)2 Quad CPU Q9400 @ 2.66GHz

Offline

**Thomas DE SOZA****Guru**- From: EDF
- Registered: 2007-11-23
- Posts: 3,066

pierre_j wrote:

What is not clear in my mind is which integration method is used for element section integration?

In other solvers, it has usually an impact on number of layers you can define... Something like (example for 3 layers):

The integration in the layers is explained in :

- for DKT : [R3.07.03] Eléments de plaque DKT, DST, DKQ, DSQ et Q4g, page 42, §4.7

- for COQUE_3D : [R3.07.04] Éléments finis de coques volumiques , page 26, §4.8

Regarding the question of getting the results at the integration point, CALC_ELEM and POST_RELEVE_T should solve it.

TdS

Offline

**pierre_j****Member**- Registered: 2010-01-19
- Posts: 773

toltec wrote:

My original question still stands... is it possible to calculate and write the integration point *equivalent plastic strain* (and Mises stress for that matter) to text and .med files? I want to do this to ensure that mises stresses and equivalent plastic strains are consistent with the plastic strain curve implied in the material model. This must be done at integration points where material calculations are done as extrapolated nodal values will be misleading.

Well actually, and in my understanding, I thought I answered your question: the commands I pasted should exactly do this.

Now, I also understand that you may fear that a CALC_ELEM re-interpolate even if it is not needed, right?

Well, this, I am unable to answer.

Bests,

Pierre

PS: Thomas, thanks for your answer.

Could you also please comment the picture: does it reflect a correct understanding of "NIVE_COUCHE" option of "CALC_ELEM" command or not?

*Last edited by pierre_j (2011-03-04 14:01:10)*

Offline

**Thomas DE SOZA****Guru**- From: EDF
- Registered: 2007-11-23
- Posts: 3,066

pierre_j wrote:

PS: Thomas, thanks for your answer.

Could you also please comment the picture: does it reflect a correct understanding of "NIVE_COUCHE" option of "CALC_ELEM" command or not?

Yes. The 3-point integration per layer (COQUE_NCOU layers in the thickness in Code_Aster) is a simple Simpson's integration rule.

As explained in the manual, this choice has been made to enable the computation of the stress on the top and bottom of a plate **without extrapolation**. This means that when one uses CALC_ELEM and NUME_COUCHE/NIVE_COUCHE the stresses are the exact ones output by the constitutive law.

TdS

Offline

**toltec****Member**- Registered: 2009-01-04
- Posts: 94

Hi Thomas, Pierre,

Many thanks for your input. As I understand it then, using EQUI_NOEU_SIGM (for example) with CALC_ELEM and NUME_COUCHE/NIVE_COUCHE will give correct stresses, even though results are at nodes. In abaqus extrapolation from Gauss integration points to the nodes would've introduced error.

I'll play around with a model and dig deeper into the manuals.

Regards

Gary

Ubuntu 12.04

Intel(R) Core(TM)2 Quad CPU Q9400 @ 2.66GHz

Offline

**Thomas DE SOZA****Guru**- From: EDF
- Registered: 2007-11-23
- Posts: 3,066

toltec wrote:

Many thanks for your input. As I understand it then, using EQUI_NOEU_SIGM (for example) with CALC_ELEM and NUME_COUCHE/NIVE_COUCHE will give correct stresses, even though results are at nodes. In abaqus extrapolation from Gauss integration points to the nodes would've introduced error.

I was not clear enough. CALC_ELEM with NUME_COUCHE/NIVE_COUCHE will give exact results for fields given at the gauss points (*_ELGA fields). For plates, the interesting point to note is that when using NUME_COUCHE=n and NIVE_COUCHE='SUP' you'll get exact results for the gauss points located on the top of plate.

As in all FEM software however, fields expressed at the nodes on whatever layer (*_ELNO or *_NOEU) will be extrapolated and therefore may lose their meaning (for example a cumulative plastic strain may become negative).

TdS

Offline

Pages: **1**