Field variable for non-linear material

[Mohamedsayed]

Hello everyone

I know how to change the material properties at specified time step from Mat-1 to Mat-2 if both of them are elastic. I can use the field variable to perform that task
*Elastic, depe=1
E1,Neo1, , 1
E2, Neo2, ,2
** E1 and Neo1 will be assigned for the first Material, while E2 and Neo2 will be assigned to the second material

But how can i change the material properties if Mat-1 is elastic-plastic but Mat-2 is elastic?
I use Mohr-coloumb plasticity to define the non-linearity of the first material.

Since i am using field variable to change the material properties, so there should be field variable-1 associated with the non-linearity of material-1, no problem with that. but my problem is for field variable-2 which is associated with the non-linearity of material-2 !!. AS i mentioned before material-2 is elastic so there is no plasticity. I guess i should omit the field variable-2 assocaited with the non-linearity of Material-2, right?

 

[akabarten]

Hi,

Please try as follow:

** material 1 (elastic-plastic)
*MATERIAL, NAME=MAT-1
*ELASTIC
**   E,   v, temp,  FV1
 200.0, 0.3,     ,  0.0
 210.0, 0.3,     ,  1.0
*PLASTIC, DEPENDENCIES=1
** stress, strain, temp, FV1
      0.3,    0.0,     , 0.0
      0.4,    0.5,     , 0.0
**
      0.4,    0.0,     , 1.0
      0.5,    0.5,     , 1.0
**
** material 1 (elastic)
*MATERIAL, NAME=MAT-2
*ELASTIC
**   E,   v, temp, FV1, FV2
 200.0, 0.3,     ,    , 0.0
 210.0, 0.3,     ,    , 1.0
**

Now you can control both material independent, FV1 for elastic-plastic and FV2 for elastic material.

Regards,
Bartosz

 

[Mohamedsayed]

Thank you Bartosz for your answer, I guess i was not clear in my post, and you miss understand me. I do not have two materials, I have one material, the initial behavior of that material is elastic-plastic. at certain step during the analysis i want to change that property (elastic-plastic) to another property which is elastic. so again it is one material
I guess it should be like that, but please correct me if i am wrong.

*Material, name=Mat-1
*Elastic, dependencies=1
** E, v, temp, FV1
200.0, 0.3, , 0.0
210.0, 0.3, , 1.0
*PLASTIC, DEPENDENCIES=1
** stress, strain, temp, FV1
0.3, 0.0, , 0.0
0.4, 0.5, , 0.0

**Then i will use the *field, variable option to change the material properties at the second step.
*step
*Field, variable=1
setname, 1

by this way the the material will behave initially as elastic-plastic, then it will behave as elastic; because there is only elastic properties associated with the field variable FV1. please correct me if i am wrong.

Thanks

 

[akabarten]

Hi,

You are right I did not get what you want to do.
Now I see, you have one material and you want to change properties from elastic-plastic to elastic.

I think your approach will not work as you expect. Abaqus need to use some FV for *PLASTIC keyword.
Usually if you define FV value you not defined Abaqus is using constant extrapolation outside not defined range.
So in your case it will be FV=0.0 since it is only used value in your definition.

I would try to go in that direction:

** material 1 (elastic-plastic)
**
** FV=0.0 -> elastic-plastic
** FV=1.0 -> elastic
*MATERIAL, NAME=MAT-1
*ELASTIC
**   E,   v, temp,  FV1
 200.0, 0.3,     ,  0.0
 210.0, 0.3,     ,  1.0
*PLASTIC, DEPENDENCIES=1
** stress, strain, temp, FV1
      0.3,    0.0,     , 0.0
      0.4,    0.5,     , 0.0
** use very high yield value to be alwyas in elastic part
  1.0e+28,    0.0,     , 1.0
  1.1e+28,    0.5,     , 1.0
**

However I think it can work wrong, when you get plastic strains for some
elements material will get extreme stress values after switching from FV=0.0 to FV=1.0
Field variable are used to change material properties and you want to change material law used during simulation.

Best,
Bartosz