Accessing Abaqus Materials

Utility Routine Interface

     dimension stress(*),ddsdde(ntens,*),stran(*),dstran(*),
    *	defGrad(3,3),predef(npredf),dpredef(npredf),coords(3)
     ...

     call material_lib_mech(materiallib,stress,ddsdde,stran,dstran,
    *       npt,dvdv0,dvmat,dfgrd,predef,dpredef,npredf,celent,coords)
     ...

Variables to Be Provided to the Utility Routine

materiallib: Variable containing information about the Abaqus material. This variable is passed into user subroutine UELMAT.
stran: Strain at the beginning of the increment.
dstran: Strain increment.
npt: Integration point number.
dvdv0: Ratio of the current volume to the reference volume at the integration point.
dvmat: Volume at the integration point.
dfgrd: Array containing the deformation gradient at the end of the increment.
predef: Array of interpolated values of predefined field variables at the integration point at the start of the increment.
dpredef: Array of increments of predefined field variables.
npredf: Number of predefined field variables, including temperature.
celent: Characteristic element length.
coords: An array containing the coordinates of this point. These are the current coordinates if geometric nonlinearities are accounted for during the step (see Defining an Analysis); otherwise, the array contains the original coordinates of the point.

Variables Returned from the Utility Routine

stress: Stress tensor at the end of the increment.
ddsdde: Jacobian matrix of the constitutive model, $\partial Δ σ / \partial Δ ε$ , where $Δ σ$ are the stress increments and $Δ ε$ are the strain increments. ddsdde(i,j) defines the change in the ith stress component at the end of the time increment caused by an infinitesimal perturbation of the jth component of the strain increment array.