import deformed model (stress and strain)

[lokado]

hello evrybody,
i'm new user to abaqus and i want know ,how i can recover model in explicit with stress and stress in abaqus and use it in another analysis
thanks

 

[burningDiesel]

*import
see user manual: 9.2 Importing and transferring results

 

[lokado]

thank you sdebock
i see that,but i didn't understand how to import the assemblie with stress...,if you can explain me how to apply that..i I will be grateful...
thank you in advance

 

[burningDiesel]

Importing the material state

You can specify whether or not the associated material state should be imported. If you choose to import the material state, the following are imported:

stresses;

equivalent plastic strains;

back stresses for the kinematic hardening models;

user-defined state variables;

damage-related state variables for the concrete damaged plasticity model;

damage-related state-variables for traction-separation response with cohesive elements;

damage-related state variables for ductile metals;

damage-related state variables for fiber-reinforced composites;

maximum deviatoric strain energy density during deformation history for Mullins effect;

internal strains and stresses for viscoelastic material models; and

connector state variables such as plastic strains, frictional slip, and damage state.

Thus, the state is imported correctly for further analysis only for the following:

linear elasticity,

Mises plasticity (including the kinematic hardening models),

extended Drucker-Prager plasticity,

crushable foam plasticity,

Mohr-Coulomb plasticity,

critical state (clay) plasticity,

cast iron plasticity,

concrete damaged plasticity,

hyperelasticity (including Mullins effect),

hyperfoam,

viscoelasticity,

traction-separation response with damage for cohesive elements,

damage for ductile metals,

damage for fiber-reinforced composites,

connector behavior, and

materials defined in user subroutines UMAT and VUMAT.

For all other material models only stresses will be imported. No other state variables will be imported.

If the material behavior is defined in a user subroutine, you must ensure that the UMAT and VUMAT are consistent.

If connector elements are imported, the state can be imported provided that the configuration is not updated.
Input File Usage: Use the following option to specify that the material state should be imported:


*IMPORT, STATE=YES

Use the following option to specify that the material state should not be imported:

*IMPORT, STATE=NO

For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition.

Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Abaqus/CAE always imports the material state. If you want to import only the deformed mesh, you can import an orphan mesh from a selected step and increment of an output database; see “What kinds of files can be imported and exported from Abaqus/CAE?,” Section 10.1.1 of the Abaqus/CAE User's Manual.

 

[lokado]

thank you very much

 

[Mohamedsayed]

I have question, what is the difference between importing results and then using them in anther analysis and restart analysis

 

[burningDiesel]

restart analysis restarts your analysis from a certain step.
import analysis imports your analysis from a certain step.
The main difference is that in *import, you can define additional parts/surfaces/elementsets/...