ABAQUS User Subroutines Reference Manual  

1.1.27 UHYPEL
User subroutine to define a hypoelastic stress-strain relation.

Product: ABAQUS/Standard  

References

Overview

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 1.1.40); and

  • ignores any data specified outside the user subroutine for the associated hypoelastic material definition.

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 element's transverse shear stiffness. See “Shell section behavior,” Section 23.6.4 of the ABAQUS Analysis User's Manual, and “Choosing a beam element,” Section 23.3.3 of the ABAQUS Analysis User's Manual, for guidelines on choosing this stiffness.

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,” Section 21.1.4 of the ABAQUS Analysis User's Manual.

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,

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 “Procedures: overview,” Section 6.1.1 of the ABAQUS Analysis User's Manual); 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.