×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Field variable for non-linear material

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?

RE: Field variable for non-linear material

Hi,

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

(OP)
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

RE: Field variable for non-linear material

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:

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

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources