Atom topic feed | site map | contact | login | Powered by FluxBB | réalisation artaban

You are not logged in.

- Topics: Active | Unanswered

**oltreuomo****Member**- Registered: 2016-09-05
- Posts: 19

Hi,

Could someone give me some guidance on the proper way to retrieve thermally-induced stresses/strains of a structure in a free (mechanically unconstrained) state? I am simply trying to analyze a thick composite cylinder, modeled using solid elements with orthotropic properties.

I first perform a linear thermal analysis to apply the temperature distribution that I want. Then, to retrieve the thermally-induced stresses, I assign a reference temperature using AFFE_MATERIAU/VALE_REF and perform a linear static analysis using MECA_STATIQUE. The issue that I am having is that I am unable to come up with a set of boundary conditions for MECA_STATIQUE which allows the cylinder to change size freely with temperature (and not build stresses due to imposed displacement constraints), and also not fail due to encountering a singular matrix.

Does anyone have any advice for doing this? Thanks in advance.

Offline

**stephaneberger****Member**- From: Strasbourg (France)
- Registered: 2012-10-15
- Posts: 68

Hi,

To run static calculation you must avoid any rigid body motion.

In your case, you have to lock your model, at least one node.

stephane

Offline

**tianyikillua****Member**- From: Paris
- Registered: 2017-11-06
- Posts: 17

Hi,

I have exactly the same problem (thermal stresses induced by temperature dilataion on an unconstrained structure).

I end up by solving the mechanical problem via an iterative solver (GCPC in Code_Aster). This will give you a solution including a rigid body motion. Then I performed a least squares analysis in ParaView to remove this rigid body motion in order that the displacement field is orthogonal to rigid body motions.

Offline

**RenatoLi****Member**- Registered: 2018-01-04
- Posts: 1

Same problem here, but unfortunately what Tiany suggested didn't work for me. Any other ideas would be much appreciated.

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,120
- Website

many structure, particularly revolution one, can be given a set of boundary conditions that will not induce any mechanical stress

it would be a good idea to post a sketch o better the mesh to give an advice

Offline

**tianyikillua****Member**- From: Paris
- Registered: 2017-11-06
- Posts: 17

RenatoLi wrote:

Same problem here, but unfortunately what Tiany suggested didn't work for me. Any other ideas would be much appreciated.

Hi, in which sense that the method doesn't work for you? You do not want to conduct an additional post processing step or you think the solution is not physically meaningful?

Offline

**will.logie****Member**- From: Canberra
- Registered: 2017-09-23
- Posts: 7

I've performed a similar analysis in another software (foam-extend) where I used a mixed boundary condition for axial (longitudinal) displacement to achieve a generalised plane strain state (zero axial force); the displacement tensor is zero-gradient everywhere except for the axial direction (e.g. ZZ), whereby I used Hooke's law to determine the plane displacement required for the state of zero axial force (e.g. using LaTeX notation, with $w$ as axial displacement, E is Young's modulus and A is patch area, $w=\frac{\int_A\sigma_{zz}\mathrm{d}Az}{EA}$). I have also seen this BC called "fixed displacement zero shear" I think.

It would interest me too to learn how generalised plane strain might be handled in Code_Aster. Attached is an image describing (a) simple plane strain and (b) generalised plane strain using an example from Timoshenko (case 135, p412, 1951); outside temperature 100degC, inside temperature 0degC, outer radius 0.7m, inner radius 0.5m - original mesh shown inside and deformed mesh x 1000 outside.

*Last edited by will.logie (2018-01-31 00:52:32)*

Solar Thermal Group

Research School of Engineering

Australian National University

http://stg.anu.edu.au/

Offline

**will.logie****Member**- From: Canberra
- Registered: 2017-09-23
- Posts: 7

Assuming ends of tube are called *front* and *back* the following achieves a state of generalised plane-strain:

```
## DEFINE MECHANICAL BOUNDARY CONDITIONS [U4.44.01]
meLoad1=AFFE_CHAR_MECA(
MODELE=meModel,
DDL_IMPO= _F(
GROUP_MA=('back',),
DZ=0,
),
FORCE_NODALE=_F(
GROUP_NO=('front',),
FZ=0.0,
),
LIAISON_UNIF=_F(
GROUP_MA=('front',),
DDL='DZ',),
);
```

Cheers,

Will.

*Last edited by will.logie (2018-03-17 14:27:54)*

Solar Thermal Group

Research School of Engineering

Australian National University

http://stg.anu.edu.au/

Offline