UHYPEL

User subroutine to define a hypoelastic stress-strain relation.

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, $ν$ ;
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); and
ignores any data specified outside the user subroutine for the associated hypoelastic material definition.

This page discusses:

Special Considerations for Various Element Types
User Subroutine Interface
Variables to Be Defined
Variables Passed in for Information

Special Considerations for Various Element Types

There are several special considerations that need to be noted.

Beams and Shells That Calculate Transverse Shear Energy

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 material transverse shear modulus (see Defining the Elastic Transverse Shear Modulus) or the element's transverse shear stiffness (see Shell Section Behavior).

Elements with Hourglassing Modes

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.

User Subroutine Interface

      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
      END

Variables to Be Defined

E: Young's modulus.
GNU: Poisson's ratio.

Variables Passed in for Information

STRAIN: Array containing the total (elastic) strains, $(ε) .$
NDI: Number of direct strain components at this point.
NSHR: Number of shear strain components at this point.
EINV1: $I_{1} = trace (ε)$ , the first strain invariant.
EINV2: $I_{2} = 1 / 2 (ε : ε - I_{1}^{2})$ , the second strain invariant.
EINV3: $I_{3} = det (ε)$ , 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); 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.