Product: Abaqus/Standard
Utility routine MATERIAL_LIB_MECH returns the stress and the material Jacobian at the element material point.
The routine can be called only from Abaqus/Standard user subroutine UELMAT.
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)
...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,” Section 6.1.2 of the Abaqus Analysis User's Guide); otherwise, the array contains the original coordinates of the point.
stress
Stress tensor at the end of the increment.
ddsdde
Jacobian matrix of the constitutive model, 
, where 
are the stress increments and 
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.