Product: Abaqus/Standard
User subroutine UDMGINI:
can be used to specify a user-defined damage initiation criterion;
allows the specification of more than one failure mechanism in an element, with the most severe one governing the actual failure;
can be used in combination with several Abaqus built-in damage evolution models, with each model corresponding to a particular failure mechanism;
will be called at all integration points of elements for which the material definition contains user-defined damage initiation criterion;
can call utility routine GETVRM to access material point data; and
is currently available only for enriched elements.
SUBROUTINE UDMGINI(FINDEX,NFINDEX,FNORMAL,NDI,NSHR,NTENS,PROPS,
1 NPROPS,STATEV,NSTATEV,STRESS,STRAIN,STRAINEE,LXFEM,TIME,
2 DTIME,TEMP,DTEMP,PREDEF,DPRED,NFIELD,COORDS,NOEL,NPT,LAYER,
3 KSPT,KSTEP,KINC,KDIRCYC,KCYCLELCF,TIMECYC,SSE,SPD,SCD,SVD,
4 SMD,JMAC,JMATYP,MATLAYO,LACCFLA,CELENT,DROT,ORI)
C
INCLUDE 'ABA_PARAM.INC'
C
DIMENSION FINDEX(NFINDEX),FNORMAL(NDI,NFINDEX),COORDS(*),
1 STRESS(NTENS),STRAIN(NTENS),STRAINEE(NTENS),PROPS(NPROPS),
2 STATEV(NSTATV),PREDEF(NFIELD),DPRED(NFIELD),TIME(2),JMAC(*),
3 JMATYP(*),DROT(3,3),ORI(3,3)
user coding to define FINDEX, and FNORMAL
RETURN
ENDFINDEX(NFINDEX)
A Vector defining the indices for all the failure mechanisms.
FNORMAL(NDI, NFINDEX)
An Array defining the normal direction to the fracture plane (three dimensions) or line (two dimensions) for each failure mechanism.
STATEV
An array containing the user-defined solution-dependent state variables at this point. This array will be passed in containing the values of these variables at the start of the increment unless the values are updated in user subroutine USDFLD. They can be updated in this subroutine to their values at the end of the increment. You define the size of this array by allocating space for it (see “Allocating space” in “User subroutines: overview,” Section 18.1.1 of the Abaqus Analysis User's Guide, for more information).
SSE,SPD,SCD,SVD,SMD
Specific elastic strain energy, plastic dissipation, “creep” dissipation, viscous, and damage energy, respectively, passed in as the values at the start of the increment and should be updated to the corresponding specific energy values at the end of the increment. They have no effect on the solution, except that they are used for energy output.
NFINDEX
Number of indices for all failure mechanisms.
NDI
Number of direct stress components at this point.
NSHR
Number of engineering shear stress components at this point.
NTENS
Size of the stress or strain component array (NRI + NSHR).
PROPS(NPROPS)
User-specified array of material constants associated with this user-defined failure criterion.
NPROPS
User-defined number of material constants associated with this user-defined failure criterion.
NSTATV
Number of solution-dependent state variables associated with this material (specified when space is allocated for the array; see “Allocating space” in “User subroutines: overview,” Section 18.1.1 of the Abaqus Analysis User's Guide).
STRESS(NTENS)
An Array passed in as the current stress tensor. If a local orientation is used at the same point as user subroutine UDMGINI, the stress components will be in the local orientation; in the case of finite-strain analysis, the basis system in which stress components are stored rotates with the material.
STRAIN(NTENS)
An Array containing the current total strains. If a local orientation is used at the same point as user subroutine UDMGINI, the strain components will be in the local orientation; in the case of finite-strain analysis, the basis system in which strain components are stored rotates with the material.
STRAINEE(NTENS)
An Array containing the current elastic strains. If a local orientation is used at the same point as user subroutine UDMGINI, the elastic strain components will be in the local orientation; in the case of finite-strain analysis, the basis system in which elastic strain components are stored rotates with the material.
LXFEM
An integer flag to indicate an enriched element.
TIME(1)
Value of step time at the beginning of the current increment.
TIME(2)
Value of total time at the beginning of the current increment.
DTIME
Time increment.
TEMP
Temperature at the start of the increment.
DTEMP
Increment of temperature during the time increment.
PREDEF
An array containing the values of all of the user-specified predefined variables at this point at the start of the increment.
DPRED
An array containing the increments of all of the predefined variables during the time increment.
NFIELD
Number of user-specified predefined variables.
COORDS
An array containing the current coordinates of this point.
NOEL
Element number.
NPT
Integration point number.
LAYER
Layer number (for composite shells and layered solids).
KSPT
Section point number within the current layer.
KSTEP
Step number.
KINC
Increment number.
KDIRCYC
Iteration number in a direct cyclic analysis.
KCYCLELCF
Cycle number in a direct cyclic low-cycle fatigue analysis.
TIMECYC
Time period in one loading cycle in a direct cyclic analysis.
JMAC
Variable that must be passed into the GETVRM utility routine to access a material point variable.
JMATYP
Variable that must be passed into the GETVRM utility routine to access a material point variable.
MATLAYO
Variable that must be passed into the GETVRM utility routine to access a material point variable.
LACCFLA
Variable that must be passed into the GETVRM utility routine to access a material point variable.
CELENT
Characteristic element length, which is a typical length of a line across an element for a first-order element; it is half of the same typical length for a second-order element. For beams and trusses it is a characteristic length along the element axis. For membranes and shells it is a characteristic length in the reference surface. For axisymmetric elements it is a characteristic length in the (r, z) plane only. For cohesive elements it is equal to the constitutive thickness.
DROT(3,3)
Rotation increment matrix. This matrix represents the increment of rigid body rotation of the basis system in which the components of stress (STRESS) and strain (STRAIN) are stored. It is provided so that vector- or tensor-valued state variables can be rotated appropriately in this subroutine: stress and strain components are already rotated by this amount before UDMGINI is called. This matrix is passed in as a unit matrix for small-displacement analysis and for large-displacement analysis if the basis system for the material point rotates with the material (as in a shell element or when a local orientation is used).
ORI(3,3)
Material orientation with respect to global basis.
As a simple example of the coding of user subroutine UDMGINI, consider a damage initiation criterion based on two different failure mechanisms: the maximum principal stress and the quadratic traction-interaction.
SUBROUTINE UDMGINI(FINDEX,NFINDEX,FNORMAL,NDI,NSHR,NTENS,PROPS,
1 NPROPS,STATEV,NSTATEV,STRESS,STRAIN,STRAINEE,LXFEM,TIME,
2 DTIME,TEMP,DTEMP,PREDEF,DPRED,NFIELD,COORDS,NOEL,NPT,
3 KLAYER,KSPT,KSTEP,INC,KDIRCYC,KCYCLELCF,TIMECYC,SSE,SPD,
4 SCD,SVD,SMD,JMAC,JMATYP,MATLAYO,LACCFLA,CELENT,DROT,ORI)
C
INCLUDE 'ABA_PARAM.INC'
CC
DIMENSION FINDEX(NFINDEX),FNORMAL(NDI,NFINDEX),COORDS(*),
1 STRESS(NTENS),STRAIN(NTENS),STRAINEE(NTENS),PROPS(NPROPS),
2 STATEV(NSTATEV),PREDEF(NFIELD),DPRED(NFIELD),TIME(2),
3 JMAC(*),JMATYP(*),DROR(3,3),ORI(3,3)
DIMENSION PS(3), AN(3,3), WT(6)
PS(1)=0.0
PS(2)=0.0
PS(3)=0.0
C
C ROTATE THE STRESS TO GLOBAL SYSTEM IF THERE IS ORIENTATION
C
CALL ROTSIG(STRESS,ORI,WT,1,NDI,NSHR)
C
C MAXIMUM PRINCIPAL STRESS CRITERION
C
CALL SPRIND(WT,PS,AN,1,NDI,NSHR)
SIG1 = PS(1)
KMAX=1
DO K1 = 2, NDI
IF(PS(K1).GT.SIG1) THEN
SIG1 = PS(K1)
KMAX = K1
END IF
END DO
FINDEX(1) = SIG1/PROPS(1)
DO K1=1, NDI
FNORMAL(K1,1) = AN(KMAX,K1)
END DO
C
C QUADRATIC TRACTION-INTERACTION CRITERION
c
FINDEX(2)=(STRESS(1)/PROPS(2))**2.0+(STRESS(NDI+1)/
$ PROPS(3))**2.0+(STRESS(NDI+2)/PROPS(4))**2.0
C
FINDEX(2)=sqrt(FINDEX(2))
C
DO K1=1, NDI
FNORMAL(K1,2)=ORI(K1,1)
END DO
RETURN
END