Field variable for non-linear material
Field variable for non-linear material
(OP)
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?
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?





RE: Field variable for non-linear material
Please try as follow:
CODE
** 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
RE: Field variable for non-linear 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
RE: Field variable for non-linear material
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:
CODE
** 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