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

You are not logged in.

- Topics: Active | Unanswered

**Johannes_ACKVA****Member**- From: Ingenieurbüro für Mechanik, DE
- Registered: 2009-11-04
- Posts: 763
- Website

Bonjour,

does anybody know about a way how to calculate the 2 principal stresses on a surface of a solid?

Assuming that no pressure acts on the solid it is ensured that 2 (of the 3 principal stresses) are in the tangent plane of the 3D-solid. In some standards, for example the german FKM-Richtlinie those 2 tangent principal stresses are needed for stress evaluation. I looked to CALC_CHAMP, but it seems none of the options does that

thank you for your any help

Regards

Johannes_ACKVA

_________________________________________________________

CODE-ASTER-courses at Ingenieurbüro für Mechanik, Germany

*** CODE-ASTER INTRODUCTION

14 - 18 Oct 2019

*** CODE-ASTER DYNAMIC ANALYSIS

21 - 22 Nov 2019

Ingenieurbüro für Mechanik

D 91717 Wassertrüdingen / Germany

www.code-aster.de Training & Support for NASTRAN and CODE-ASTER

Offline

**Volker****Member**- From: Chemnitz
- Registered: 2016-05-23
- Posts: 92

Bonjour Johannes,

which part of FKM Guideline do you mean ??

Do you mean for example calculation of G_Sigma and G_Tau according equation no. 4.3.17 ??

Kind regards Volkere

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,974

hello Johannes

if you do a CALC_CHAMP on some group you are to have in the result

'VMIS',

'PRIN_1','PRIN_2','PRIN_3', the principal stress values (modulus of the vector)

'VECT_1_X','VECT_1_Y','VECT_1_Z',

'VECT_2_X','VECT_2_Y','VECT_2_Z',

'VECT_3_X','VECT_3_Y','VECT_3_Z',

the component along X, Y, Z global of each principal stress

after that anything is possible with some post processing in code_aster or Gmsh

the real difficulty is to eliminate the one perpendicular to the plane of the element

i have been struggling at that for quite a while and never found a good solution

however beware that principal directions and principal stress may be meaningless once we do averaging at nodes in SIEQ_ELNO, SIEQ_NOEU

code-aster.org/forum2/viewtopic.php?id=16737

it may be strictly true only with ELGA field

and as far as i know in 3D modeling the Gauss point are not on the face of the elements

i cannot at the time being give a more valuable information

but this task is on my list for 2D elements

the attached screen shot shows SIEQ_NOEU as a vector on a shell model

jean pierre aubry

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**paster****Member**- Registered: 2009-08-14
- Posts: 73

Hello

Maybe you can try to put skin elements around your model. Of course thin thickness, low Young modulus, same nodes .

after that this is Aster "cooking" (only 2 principal stresses by node, element…): I'm not a Code_Aster's specialist (may be Jean Pierre?). This method is quite general and simple

Good luck

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,974

Maybe you can try to put skin elements around your model. Of course thin thickness, low Young modulus, same nodes .

i do think this is not necessary maybe giving wrong results by polluting the model

as post processing on a group of surface elements defined on the skin does the job

at least this is my experience

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**Volker****Member**- From: Chemnitz
- Registered: 2016-05-23
- Posts: 92

Hi All,

here a sketch with my interpretation of the local stresses according the FKM Guideline:

How can we calculate the stress gradient with Code_Aster??

Kind regards Volker

PS

jeanpierreaubry wrote:

i do think this is not necessary maybe giving wrong results by polluting the model..

I total agree with you ,

but I got also the same advice from a commercial support-team to introduce skin elements ;-)

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,974

Volker wrote:

but I got also the same advice from a commercial support-team to introduce skin elements ;-)

probably because their code cannot handle stress on face boundary

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**paster****Member**- Registered: 2009-08-14
- Posts: 73

Re Hello

Open your eyes. Commercial codes are not the devil! This method is not exect of course but better than any kind of extrapolation.

There is no pollution if you take care to the stiffness (lower than possible by thickness) of the skin membrane elements (same dof's like volume elements). Ex: QUA8 on HEX20, TRI3 on TET4.... (for 3D analysis)

Sincerely

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,974

paster wrote:

Re Hello

Open your eyes. Commercial codes are not the devil! This method is not exect of course but better than any kind of extrapolation.

this is not the question

code_aster does what is wanted without this !

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**Johannes_ACKVA****Member**- From: Ingenieurbüro für Mechanik, DE
- Registered: 2009-11-04
- Posts: 763
- Website

@paster,

skin elements for stress evaluation: with some FE-codes this is the suitable method, for example Nastran. Nastran has pure membran elements which have only the translational DOFs, so those as skin elements do not augment the number of DOFs. But Code-Aster's 2D-structural elements have all the rotational DOFs in addition. When making them very thin, there can be numerical problems with the rot DOFs.

@Volker

at the moment I haven't thoroughly studied the FKM-Guideline, I m preparing only the first steps.

For the derivative of stresses something like this (very rough) is perhaps suitable:

CALC_CHAMP( SIGM_NOEU, SIEQ_NOEU)

MACR_LIGN_COUPE to get the evolution of stresses through the thickness of a solid and put it in a table. You can collect components of SIGM_* of of SIEQ_*. Which means that you can collect also the principal stresses

RECU_FONCTION to make a function: Stress(ThicknCoor) or Principal(ThicknCoor)

CALC_FONCTION ( DERIVE..) to make the derivative of the function

When treating with princ stresses I see the problem that the directions of the principal stresses change with the abszissa, do you know a solution to that?

Regards

Johannes_ACKVA

_________________________________________________________

CODE-ASTER-courses at Ingenieurbüro für Mechanik, Germany

*** CODE-ASTER INTRODUCTION

14 - 18 Oct 2019

*** CODE-ASTER DYNAMIC ANALYSIS

21 - 22 Nov 2019

Ingenieurbüro für Mechanik

D 91717 Wassertrüdingen / Germany

www.code-aster.de Training & Support for NASTRAN and CODE-ASTER

Offline

**paster****Member**- Registered: 2009-08-14
- Posts: 73

Hello

One more I'm not a code aster guru but, elements like MEMBTR3, MEMBQU4... are not good for your application (they have 3 translational dof's). I don't know what meshing tool you use but even with Gibi, it's very easy to extract the envelop of a 3D model

After that end for me

Offline

**AsterO'dactyle****Administrator**- Registered: 2007-11-29
- Posts: 449

Hello,

Try SIRO_ELEM in CALC_CHAMP

Code_Asterの開発者

Offline

**Johannes_ACKVA****Member**- From: Ingenieurbüro für Mechanik, DE
- Registered: 2009-11-04
- Posts: 763
- Website

AsterO'dactyle wrote:

Try SIRO_ELEM in CALC_CHAMP

that's it ! Many thanks, AsterO'dactyle !

Regards

Johannes_ACKVA

_________________________________________________________

CODE-ASTER-courses at Ingenieurbüro für Mechanik, Germany

*** CODE-ASTER INTRODUCTION

14 - 18 Oct 2019

*** CODE-ASTER DYNAMIC ANALYSIS

21 - 22 Nov 2019

Ingenieurbüro für Mechanik

D 91717 Wassertrüdingen / Germany

www.code-aster.de Training & Support for NASTRAN and CODE-ASTER

Offline