Density and Elasticity Modulus changes through thickness

[sdata]

Hello Colleagues,
I'm working on modeling a FGM plate in which Density and Elasticity Modulus changes through
thickness of plate by an exponential function. The following USDFLD subroutine is copied from
thread799-295995.
I have some questions to complete this subroutine:
1. How Abaqus will relate field(1) or statev(1) to Elasticity Modulus?
2. If Abaqus reads Elasticity Modulus from subroutine, then what is the point of filling
Elastic material table in property module?
3. In Elastic material table in property module, what does field(1) refer to?
4. If I want to add density change to this subroutine similar to Elasticity change, how
can i elaborate in subroutine for Abaqus to distinguish between Density and Elasticity Modulus?
Any help would be appreciated in advance.

c     first inc. of first step ?
      if (kstep .eq. 1 .and. kinc .eq. 1) then

c       read y-coordinate
        y = coord(2)
c       calculate Young module
        E = 69600.d0 * (1.d0 + y / 2.5d0)
c       define depend state variable (E(y))
        field(1) = E
c       save E value for state dependend variable
        statev(1) = E

c     do it for all others inc. and steps
      else
c       assign initial values calculated in first inc.
        field(1) = statev(1)

      end if

 

[akabarten]

Hi,

How Abaqus will relate field(1) or statev(1) to Elasticity Modulus?

The relation is made by material definition and field variable used with it.
Variable filed(1) in the subroutine is first field variable (FV1) in material definition.

If Abaqus reads Elasticity Modulus from subroutine

Not true, Abaqus does not read elastic module from the subrotutine, Abaqus read value of field variable from subroutine.

then what is the point of filling Elastic material table in property module?

It is because Abaqus has to know what is relation between elastic module and field variable from the subroutine.
The trick here is that elastic module is equal to field variable.

If I want to add density change to this subroutine similar to Elasticity change

Just use two field variable. FV1 can refer to density and FV2 to elastic module.

**
**
*MATERIAL, NAME=myMaterial
*DENSITY, DEPENDENCIES=1
**     ro, temp,    FV1
      0.0,     ,    0.0
   1000.0,     , 1000.0
*ELASTIC, DEPENDENCIES=2, TYPE=ISOTROPIC
**    E,   v, temp, FV1,    FV2
    0.0, 0.3,     ,    ,    0.0
 1000.0, 0.3,     ,    , 1000.0
*DEPVAR
 2
 1, RO, Density
 2,  E, Elastic_module
**

Next the subroutine has to set filed(1) for FV1 (density) and filed(2) for FV2 (elastic modeule):

c     first inc. of first step ?
      if (kstep .eq. 1 .and. kinc .eq. 1) then

c       calculate value of E and ro
        rRo = ... equation to define ...
        rE = ... equation to define ...
c       define depend state variable
        field(1) = rRo
        field(2) = rE
c       set state depended variable
        statev(1) = rRo
        statev(2) = rE

c     do it for all others inc. and steps
      else

c       assign initial values calculated in first inc.
        field(1) = statev(1)
        field(2) = statev(2)

      end if

Regards,
Bartosz

 

[sdata]

Thank you Bartosz for your perfect answer. I've read your other posts and I know you're doing great.
I have another question:
I'm verifying this USDFLD with song's umat in a cracked 3D plate. In .dat file both stress and strain are close together but displacement are different. what does this difference refer to?

 

[sdata]

Also, in my models Elasticity decrease through thickness, and field variables should be arranged
in ascending order. How can i fix this problem?

 

[akabarten]

Hello,

stress and strain are close together but displacement are different. what does this difference refer to?

I do not know.

Elasticity decrease through thickness, and field variables should be arranged in ascending order

I do not see a problem. Field variable is set by the subroutine not by Abaqus material definition.

Regards,
Bartosz