How to apply elasto-plastic material property in first step and elastic property in the second step? 1

[hiall12]

Hi,
I have an axi-spymmetric model. I want to apply elasto-plastic material properties in the first step and elastic material property in the second step. Is there a way to do it?
What I did is, while defining the material properties, I have given the plastic properties only at 20 degrees and elastic properties in all other temperatures ranging from 20 degree, 50 degree, and so on upto 550 degree. I have pre-defined the model to 20 degree in the initial step and it propagated to the first step. I have modified the temperature to 50 degree in the second step. I am expecting that it will take the available plastic properties in the initial and first step and elastic properties in the second step as the plastic properties are not defined at 50 degree. Is my logic correct? Will abaqus behave as per this logic?
Kindly suggest.

Thanks in advance.

 

[FEA way]

Abaqus will extend the material properties beyond the specified temperature range - it will keep them constant so it will be perfect plasticity above those 20 degrees.

Another way would be to use the import functionality. This case is even mentioned in the documentation chapter "Transferring Results from One Abaqus/Standard Analysis to Another":

It may sometimes be possible to simplify the material definition. For example, if a Mises plasticity model was used in the first Abaqus/Standard analysis and no further plastic yielding is expected in a subsequent Abaqus/Standard analysis, a linear elastic material can be used for the Abaqus/Standard analysis. However, if further nonlinear material behavior is expected, no changes to the existing material definitions should be made. The history of the state variables will not be maintained if the material models are not the same in both the original analysis and the import analysis.

 

[hiall12]

Thank you FEA way.
Will import functionality allow changing the material property from elasto-plastic to elastic?
In my case, I want to use elasto-plastic in the first step to allow forming.
In the next step, I want to give pressure and displacement to the formed component giving elastic properties.

 

[FEA way]

That’s what this part of the above quote refers to.

For example, if a Mises plasticity model was used in the first Abaqus/Standard analysis and no further plastic yielding is expected in a subsequent Abaqus/Standard analysis, a linear elastic material can be used for the Abaqus/Standard analysis.

Plasticity in the first analysis and linear elasticity in the second (import) analysis.

 

[hiall12]

Hi FEA way,
I have tried to import the first step that was elastoplastic, to the current abaqus file using pre-defined field in loads. Now when I am trying to change the material property to elastic, it says "One or more instances of the current part are associated with an Initial State Predefined Field. The geometry or mesh of such parts cannot be modified. Suppress or delete the Initial State Predefined Field to remove this restriction."

So it is not allowing to make any changes in the material properties.

It would really be helpful if you can please outline the steps to be followed.
Thank you.

 

[FEA way]

The import functionality is typically used by copying the original model and applying an initial state field in the copied model or by importing the part’s deformed mesh from odb and then also applying an initial state field.