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

You are not logged in.

- Topics: Active | Unanswered

**dbpatankar****Member**- From: Roorkee, Uttarakhand, India
- Registered: 2010-05-22
- Posts: 177

Hi all,

Consider following code block....

```
U1 = STAT_NON_LINE(.......
........
........);
U2 = STAT_NON_LINE(.......
........
ETAT_INIT=_F(EVOL_NOLI=U1),
.........);
```

In such a case the result calculated by U2 will be with reference to U1 or initially defined model?

Will U2 consider only the deflected shape of the model obtained after U1 calculation or will it consider stress and strains too along with deflected geometry ?

(Will the strength deterioration after U1 calculation will be taken into account?)

If the results are w.r.t. U1 then how to convert it to absolute?

Thanks in advance

Offline

**tcdonley****Member**- From: Virginia, USA
- Registered: 2010-11-24
- Posts: 94

Hi, dbpatankar,

It is difficult to answer your questions fully unless you fill in the blanks for us.

As I understand it, if your first command calculated a deformed mesh and a field of stress which existed at the end of the calculation, then ETAT_INIT may be used to begin a new calculation on the same area of the mesh, starting with the deformed, stressed state which was passed from the first command. In other words, the first time increment of U2 may start with the mesh in the same state as the final increment of U1. Whether it actually works or not depends on other key words in your STAT_NON_LINE command, load conditions, etc.

If your intent is to use the second command to apply a second load condition to the same part you'll need to be careful that your load curve does not have a discontinuity or sharp change in slope at the point where you switch from U1 to U2, or else U2 will probably not converge. If you extract results from all time steps in U1 and U2 to examine in your post-processor, you can look at how the deformation and stress fields progress through the simulation, and see if they make sense.

If you pass the state of stress and deformation correctly from one calculation to the next, then all result values are absolute. There is no change in reference system unless you create one somehow.

You may wish to have a look at U4.51.03 section 3.6 where usage of ETAT_INIT is discussed in detail.

Good luck!

- Tim Donley

*Last edited by tcdonley (2010-12-09 02:52:59)*

Offline

**dbpatankar****Member**- From: Roorkee, Uttarakhand, India
- Registered: 2010-05-22
- Posts: 177

Really thanks for answering.

tcdonley wrote:

Hi, dbpatankar,

It is difficult to answer your questions fully unless you fill in the blanks for us.

Here I am attaching the whole comm file for you.

Although as you can see it consists of two parts, one for modal analysis and other for non-linear static analysis.

For modal analysis I want to change the MAILLAGE with SDSP. But for the STAT_NON_LINE I am keeping the MAILLAGE same in every loop.

tcdonley wrote:

You may wish to have a look at U4.51.03 section 3.6 where usage of ETAT_INIT is discussed in detail.

I already did but that wasn't enough for me. I had to read the translated version of original doc using google. So I thought translation may not be perfect.

Why I think my calculation is wrong is because the final base_shear(force) Vs top_displacement diagram is showing hardening behaviour which is not correct for RCC.

The curve should show softening.

So I thought that code may not be considering the strength deterioration in each step.

*Last edited by dbpatankar (2010-12-10 01:25:43)*

Offline

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

dbpatankar wrote:

In such a case the result calculated by U2 will be with reference to U1 or initially defined model?

Will U2 consider only the deflected shape of the model obtained after U1 calculation or will it consider stress and strains too along with deflected geometry ?

(Will the strength deterioration after U1 calculation will be taken into account?)If the results are w.r.t. U1 then how to convert it to absolute?

Thanks in advance

To complete the informations given by Tim, I should add the following :

- the results will always be w.r.t. the reference configuration, that is the one given by your mesh (which you input with LIRE_MAILLAGE).

- when using ETAT_INIT=_F(EVOL_NOLI=U1), every field are passed to the new STAT_NON_LINE (displacements, stresses, history variables). To what extent they are used depends as explained by Tim on the settings you gave in STAT_NON_LINE. For example if you make a calculation with a "small perturbations hypothesis" (COMP_INCR=_F(DEFORMATION='PETIT')), the deformed geometry is not taken into account : initial and final configurations are considered the same and therefore everything (stiffness matrix, stresses, etc ...) is computed w.r.t. the initial one.

TdS

Offline