Spatially dependent material properies

[MojtabaFarrokh]

Hi
Is there any way in Mfront to define a material whose properties depend on the coordinates X,Y,Z?
FEM packages such as abaqus and calculix pass the integration point coordinates in the user-defined subroutine UMAT as an input parameter.

[thelfer]

Dear @MojtabaFarrokh,

Spatial coordinates are currently not accessible in MFront' behaviours for at least two reasons:

• behaviours which explicitly depends on spatial coordinates are not physical (the behaviour must be invariant by change of coordinates). For the same reason, the time is not available (but the time increment is).
• the spatial coordiantes are not available in most solvers.

In Abaqus, you can use external state variables to solve this issue. In calculix, i don't know.

Regards,

Thomas

[thelfer]

To be complete, there is another solution: modify the UMAT source code generated by mfront and compute the quantity you need in the modified UMAT and pass those quantities as external state variables. If such solution is fine for you, I can show you how to do it.

[MojtabaFarrokh]

Dear @thelfer,
Thank you for your replies.
The material that I am going to simulate has properties that depend on coordinates in the reference configuration.
I already thought of your suggestion. However, I do not know how I can implement it.

I have already implemented such behavior in Abaqus UMAT using Fortran coding. Is there any way to have the Fortran code generated by mfront?

[thelfer]

You may want to read the MFront documentation about the Abaqus interface to understand how it works: https://thelfer.github.io/tfel/web/abaqus.html. The main idea is that we provide an umat.cpp file which loads shared libraries generated by MFront .

The idea is to declare in the MFront source files, material properties or external state variables. Material properties corresponds to the PROPS array of the umat, external state variables to the arrays PRED and DPRED.

Let us consider this simple example:

@DSL IsotropicPlasticMisesFlow;
@Behaviour Plasticity;

@MaterialProperty stress H;
@MaterialProperty stress s0;

@FlowRule {
  f = seq - H * p - s0;
  df_dseq = 1;
  df_dp = -H;
}

This behaviour declares four properties, as indicated by mfront-query:

- H
- s0
- YoungModulus (young): the Young's modulus of an isotropic material
- PoissonRatio (ν): the Poisson ratio of an isotropic material

This means that you can modify on the fly the first entry of the array PROPS using a function of the coordinates to compute the hardening slope H. There are then two solutions to do this:

• modify the sources generated by MFront for the behaviour that you want to use. In this case, calling mfront --interface=abaqus Plasticity.mfront generates a file named umatPlasticity.cxx. After modifying this file, you can compile the library using mfront --obuild.
• modify the generic file umat.cpp that is passed to Abaqus (and compiled by Abaqus)

The first solution is cleaner, but more complex. The second is maybe more straigthforward.

[MojtabaFarrokh]

Thank you for your reply. I got your point.
I think the first solution is better. However, I want to make sure of the procedure. Let's have a very basic example: a linear elastic material whose properties such as Young modulus and Poisson's ratio depend on the spatial coordinates. For example, E=f(X,Y,Z) and v=g(X,Y,Z). The mathematical forms of the function f and g are known and have some parameters (material constants) that must be defined and passed to the routine by the user. Could you please give me some hints about how I can implement it?

[thelfer]

@MojtabaFarrokh Let consider the following example: abaqus.zip

The tar contains two files: Plasticity.mfront and abaqusplasicity.mtest

1. generate the sources:

   mfront --interface=abaqus Plasticity.mfront

2. Open src/abaqusPlasticity.cxx with you favorite editor (emacs, vi, vscode, ....)

   tfel-editor src/abaqusPlasticity.cxx &

3. Look at the PLASTICITY_3D and modify it as follows:

   double myPROPS[4] = {3e9, 200e6, PROPS[2], PROPS[3]};
   Plasticity_base_3D(STRESS,STATEV,DDSDDE,SSE,SPD,SCD,RPL,DDSDDT,DRPLDE,DRPLDT,
   STRAN,DSTRAN,TIME,DTIME,TEMP,DTEMP,PREDEF,DPRED,CMNAME,
   NDI,NSHR,NTENS,NSTATV,myPROPS,NPROPS,COORDS,DROT,PNEWDT,
   CELENT,DFGRD0,DFGRD1,NOEL,NPT,LAYER,KSPT,KSTEP,KINC,size);
   

4. Compile your shared library:

   mfront --obuild

5. Run the MTest example:

   mtest plasticity.mtest

   You will notice that the values in the MTest files are ignored and replaced by the values given in the abaqusPlasticity.cxx file, except for the Young's modulus and the Poisson's ratio

   Young's modulus: 1.5e+11
   Poisson's ratio: 0.3
   Yield strength: 2e+08
   Hardening slope: 3e+09
   iteration 3 : 1.80603e-19 5.13539e-08 (0.01 -0.00469935 -0.00469935 0 0 0)
   convergence, after 3 iterations, order 20.8243
   

You can now modify the example to define the myPROPS array using functions of the spatial coordinates.

The cumbersome part is that you have to modify the function for all supported hypotheses..

[MojtabaFarrokh]

Thank you very much.
I will try it.