Product: Abaqus/Standard
User subroutine UHYPEL:
can be used to define isotropic hypoelastic material behavior, thus requiring the definition of Young's modulus, E, and Poisson's ratio, 
;
is called at all material calculation points of elements for which the material definition contains user-defined hypoelastic behavior;
can be used in conjunction with user subroutine USDFLD to redefine any field variables that are passed in (see “USDFLD,” Section 1.1.53); and
ignores any data specified outside the user subroutine for the associated hypoelastic material definition.
There are several special considerations that need to be noted.
When UHYPEL is used to define the material response of shell or beam elements that calculate transverse shear energy, Abaqus/Standard cannot calculate a default value for the transverse shear stiffness of the element. Hence, you must define the element's transverse shear stiffness. See “Shell section behavior,” Section 29.6.4 of the Abaqus Analysis User's Guide, and “Choosing a beam element,” Section 29.3.3 of the Abaqus Analysis User's Guide, for guidelines on choosing this stiffness.
If this capability is used to describe the material of elements with hourglassing modes, you must define the hourglass stiffness for hourglass control based on the total stiffness approach. The hourglass stiffness is not required for enhanced hourglass control, but you can define a scaling factor for the stiffness associated with the drill degree of freedom (rotation about the surface normal). See “Section controls,” Section 27.1.4 of the Abaqus Analysis User's Guide.
SUBROUTINE UHYPEL(E,GNU,STRAIN,NDI,NSHR,EINV1,EINV2,EINV3,
1 COORDS,NOEL,TEMP,PREDEF,CMNAME)
C
INCLUDE 'ABA_PARAM.INC'
C
CHARACTER*80 CMNAME
C
DIMENSION STRAIN(*),COORDS(3),PREDEF(*)
user coding to define E and GNU
RETURN
ENDSTRAIN
Array containing the total (elastic) strains, 
NDI
Number of direct strain components at this point.
NSHR
Number of shear strain components at this point.
EINV1
, the first strain invariant.
EINV2
, the second strain invariant.
EINV3
, the third strain invariant.
COORDS
An array containing the coordinates of the material point. These are the current coordinates if geometric nonlinearity is 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.
NOEL
Element number.
TEMP
Current temperature at this point.
PREDEF
An array containing current values of the predefined field variables at this point (initial values at the beginning of the analysis and current values during the analysis).
CMNAME
User-specified material name, left justified.