Product: Abaqus/Standard
Warning: This feature is intended for advanced users only. Its use in all but the simplest test examples will require considerable coding by the user/developer. “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide, should be read before proceeding.
User subroutine UELMAT:
will be called for each element that is of a general user-defined element type (i.e., not defined by a linear stiffness or mass matrix read either directly or from results file data) each time element calculations are required;
(or subroutines called by user subroutine UELMAT) must perform all of the calculations for the element, appropriate to the current activity in the analysis;
can access some of the Abaqus materials through utility routines MATERIAL_LIB_MECH and MATERIAL_LIB_HT;
is available for a subset of the procedures supported for user subroutine UEL (see “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide); and
is available for plane stress and three-dimensional element types in a stress/displacement analysis and for two-dimensional and three-dimensional element types in a heat transfer analysis (see “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide).
SUBROUTINE UELMAT(RHS,AMATRX,SVARS,ENERGY,NDOFEL,NRHS,NSVARS,
1 PROPS,NPROPS,COORDS,MCRD,NNODE,U,DU,V,A,JTYPE,TIME,DTIME,
2 KSTEP,KINC,JELEM,PARAMS,NDLOAD,JDLTYP,ADLMAG,PREDEF,NPREDF,
3 LFLAGS,MLVARX,DDLMAG,MDLOAD,PNEWDT,JPROPS,NJPROP,PERIOD,
4 MATERIALLIB)
C
INCLUDE 'ABA_PARAM.INC'
C
DIMENSION RHS(MLVARX,*),AMATRX(NDOFEL,NDOFEL),PROPS(*),
1 SVARS(*),ENERGY(8),COORDS(MCRD,NNODE),U(NDOFEL),
2 DU(MLVARX,*),V(NDOFEL),A(NDOFEL),TIME(2),PARAMS(*),
3 JDLTYP(MDLOAD,*),ADLMAG(MDLOAD,*),DDLMAG(MDLOAD,*),
4 PREDEF(2,NPREDF,NNODE),LFLAGS(*),JPROPS(*)
user coding to define RHS, AMATRX, SVARS, ENERGY, and PNEWDT
RETURN
ENDThese arrays depend on the value of the LFLAGS array.
RHS
An array containing the contributions of this element to the right-hand-side vectors of the overall system of equations. For most nonlinear analysis procedures, NRHS=1 and RHS should contain the residual vector. The exception is the modified Riks static procedure (“Static stress analysis,” Section 6.2.2 of the Abaqus Analysis User's Guide), for which NRHS=2 and the first column in RHS should contain the residual vector and the second column should contain the increments of external load on the element. RHS(K1,K2) is the entry for the K1th degree of freedom of the element in the K2th right-hand-side vector.
AMATRX
An array containing the contribution of this element to the Jacobian (stiffness) or other matrix of the overall system of equations. The particular matrix required at any time depends on the entries in the LFLAGS array (see below).
All nonzero entries in AMATRX should be defined, even if the matrix is symmetric. If you do not specify that the matrix is unsymmetric when you define the user element, Abaqus/Standard will use the symmetric matrix defined by 
, where 
is the matrix defined as AMATRX in this subroutine. If you specify that the matrix is unsymmetric when you define the user element, Abaqus/Standard will use AMATRX directly.
SVARS
An array containing the values of the solution-dependent state variables associated with this element. The number of such variables is NSVARS (see below). You define the meaning of these variables.
For general nonlinear steps this array is passed into UELMAT containing the values of these variables at the start of the current increment. They should be updated to be the values at the end of the increment, unless the procedure during which UELMAT is being called does not require such an update; this requirement depends on the entries in the LFLAGS array (see below). For linear perturbation steps this array is passed into UELMAT containing the values of these variables in the base state. They should be returned containing perturbation values if you wish to output such quantities.
When KINC is equal to zero, the call to UELMAT is made for zero increment output (see “Output,” Section 4.1.1 of the Abaqus Analysis User's Guide). In this case the values returned will be used only for output purposes and are not updated permanently.
ENERGY
For general nonlinear steps array ENERGY contains the values of the energy quantities associated with the element. The values in this array when UELMAT is called are the element energy quantities at the start of the current increment. They should be updated to the values at the end of the current increment. For linear perturbation steps the array is passed into UELMAT containing the energy in the base state. They should be returned containing perturbation values if you wish to output such quantities. The entries in the array are as follows:
| ENERGY(1) | Kinetic energy. |
| ENERGY(2) | Elastic strain energy. |
| ENERGY(3) | Creep dissipation. |
| ENERGY(4) | Plastic dissipation. |
| ENERGY(5) | Viscous dissipation. |
| ENERGY(6) | “Artificial strain energy” associated with such effects as artificial stiffness introduced to control hourglassing or other singular modes in the element. |
| ENERGY(7) | Electrostatic energy. |
| ENERGY(8) | Incremental work done by loads applied within the user element. |
When KINC is equal to zero, the call to UELMAT is made for zero increment output (see “Output,” Section 4.1.1 of the Abaqus Analysis User's Guide). In this case the energy values returned will be used only for output purposes and are not updated permanently.
PNEWDT
Ratio of suggested new time increment to the time increment currently being used (DTIME, see below). This variable allows you to provide input to the automatic time incrementation algorithms in Abaqus/Standard (if automatic time incrementation is chosen). It is useful only during equilibrium iterations with the normal time incrementation, as indicated by LFLAGS(3)=1. During a severe discontinuity iteration (such as contact changes), PNEWDT is ignored unless CONVERT SDI=YES is specified for this step. The usage of PNEWDT is discussed below.
PNEWDT is set to a large value before each call to UELMAT.
If PNEWDT is redefined to be less than 1.0, Abaqus/Standard must abandon the time increment and attempt it again with a smaller time increment. The suggested new time increment provided to the automatic time integration algorithms is PNEWDT × DTIME, where the PNEWDT used is the minimum value for all calls to user subroutines that allow redefinition of PNEWDT for this iteration.
If PNEWDT is given a value that is greater than 1.0 for all calls to user subroutines for this iteration and the increment converges in this iteration, Abaqus/Standard may increase the time increment. The suggested new time increment provided to the automatic time integration algorithms is PNEWDT × DTIME, where the PNEWDT used is the minimum value for all calls to user subroutines for this iteration.
If automatic time incrementation is not selected in the analysis procedure, values of PNEWDT that are greater than 1.0 will be ignored and values of PNEWDT that are less than 1.0 will cause the job to terminate.
PROPS
A floating point array containing the NPROPS real property values defined for use with this element. NPROPS is the user-specified number of real property values. See “Defining the element properties” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide.
JPROPS
An integer array containing the NJPROP integer property values defined for use with this element. NJPROP is the user-specified number of integer property values. See “Defining the element properties” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide.
COORDS
An array containing the original coordinates of the nodes of the element. COORDS(K1,K2) is the K1th coordinate of the K2th node of the element.
U, DU, V, A
Arrays containing the current estimates of the basic solution variables (displacements, rotations, temperatures, depending on the degree of freedom) at the nodes of the element at the end of the current increment. Values are provided as follows:
| U(K1) | Total values of the variables. If this is a linear perturbation step, it is the value in the base state. |
| DU(K1,KRHS) | Incremental values of the variables for the current increment for right-hand-side KRHS. If this is an eigenvalue extraction step, this is the eigenvector magnitude for eigenvector KRHS. For steady-state dynamics KRHS  denotes real components of perturbation displacement and KRHS  denotes imaginary components of perturbation displacement. |
| V(K1) | Time rate of change of the variables (velocities, rates of rotation). Defined for implicit dynamics only (LFLAGS(1)  11 or 12). |
| A(K1) | Accelerations of the variables. Defined for implicit dynamics only (LFLAGS(1) 11 or 12). |
JDLTYP
An array containing the integers used to define distributed load types for the element. Loads of type Un are identified by the integer value n in JDLTYP; loads of type UnNU are identified by the negative integer value 
in JDLTYP. JDLTYP(K1,K2) is the identifier of the K1th distributed load in the K2th load case. For general nonlinear steps K2 is always 1.
ADLMAG
For general nonlinear steps ADLMAG(K1,1) is the total load magnitude of the K1th distributed load at the end of the current increment for distributed loads of type Un. For distributed loads of type UnNU, the load magnitude is defined in UELMAT; therefore, the corresponding entries in ADLMAG are zero. For linear perturbation steps ADLMAG(K1,1) contains the total load magnitude of the K1th distributed load of type Un applied in the base state. Base state loading of type UnNU must be dealt with inside UELMAT. ADLMAG(K1,2), ADLMAG(K1,3), etc. are currently not used.
DDLMAG
For general nonlinear steps DDLMAG contains the increments in the magnitudes of the distributed loads that are currently active on this element for distributed loads of type Un. DDLMAG(K1,1) is the increment of magnitude of the load for the current time increment. The increment of load magnitude is needed to compute the external work contribution. For distributed loads of type UnNU the load magnitude is defined in UELMAT; therefore, the corresponding entries in DDLMAG are zero. For linear perturbation steps DDLMAG(K1,K2) contains the perturbation in the magnitudes of the distributed loads that are currently active on this element for distributed loads of type Un. K1 denotes the K1th perturbation load active on the element. K2 is always 1, except for steady-state dynamics, where K2=1 for real loads and K2=2 for imaginary loads. Perturbation loads of type UnNU must be dealt with inside UELMAT.
PREDEF
An array containing the values of predefined field variables, such as temperature in an uncoupled stress/displacement analysis, at the nodes of the element (“Predefined fields,” Section 34.6.1 of the Abaqus Analysis User's Guide).
The first index of the array, K1, is either 1 or 2, with 1 indicating the value of the field variable at the end of the increment and 2 indicating the increment in the field variable. The second index, K2, indicates the variable: the temperature corresponds to index 1, and the predefined field variables correspond to indices 2 and above. In cases where temperature is not defined, the predefined field variables begin with index 1. The third index, K3, indicates the local node number on the element.
| PREDEF(K1,1,K3) | Temperature. |
| PREDEF(K1,2,K3) | First predefined field variable. |
| PREDEF(K1,3,K3) | Second predefined field variable. |
| Etc. | Any other predefined field variable. |
| PREDEF(K1,K2,K3) | Total or incremental value of the K2th predefined field variable at the K3th node of the element. |
| PREDEF(1,K2,K3) | Values of the variables at the end of the current increment. |
| PREDEF(2,K2,K3) | Incremental values corresponding to the current time increment. |
PARAMS
An array containing the parameters associated with the solution procedure. The entries in this array depend on the solution procedure currently being used when UELMAT is called, as indicated by the entries in the LFLAGS array (see below).
For implicit dynamics (LFLAGS(1) = 11 or 12) PARAMS contains the integration operator values, as:
LFLAGS
An array containing the flags that define the current solution procedure and requirements for element calculations. Detailed requirements for the various Abaqus/Standard procedures are defined earlier in this section.
| LFLAGS(1) | Defines the procedure type. See “Results file output format,” Section 5.1.2 of the Abaqus Analysis User's Guide, for the key used for each procedure. |
| LFLAGS(2)=0 | Small-displacement analysis. |
| LFLAGS(2)=1 | Large-displacement analysis (nonlinear geometric effects included in the step; see “General and linear perturbation procedures,” Section 6.1.3 of the Abaqus Analysis User's Guide). |
| LFLAGS(3)=1 | Normal implicit time incrementation procedure. User subroutine UELMAT must define the residual vector in RHS and the Jacobian matrix in AMATRX. |
| LFLAGS(3)=2 | Define the current stiffness matrix (AMATRX  ) only. |
| LFLAGS(3)=3 | Define the current damping matrix (AMATRX  ) only. |
| LFLAGS(3)=4 | Define the current mass matrix (AMATRX  ) only. Abaqus/Standard always requests an initial mass matrix at the start of the analysis. |
| LFLAGS(3)=5 | Define the current residual or load vector (RHS  ) only. |
| LFLAGS(3)=6 | Define the current mass matrix and the residual vector for the initial acceleration calculation (or the calculation of accelerations after impact). |
| LFLAGS(3)=100 | Define perturbation quantities for output. |
| LFLAGS(4)=0 | The step is a general step. |
| LFLAGS(4)=1 | The step is a linear perturbation step. |
| LFLAGS(5)=0 | The current approximations to  , etc. were based on Newton corrections. |
| LFLAGS(5)=1 | The current approximations were found by extrapolation from the previous increment. |
TIME(1)
Current value of step time or frequency.
TIME(2)
Current value of total time.
DTIME
Time increment.
PERIOD
Time period of the current step.
NDOFEL
Number of degrees of freedom in the element.
MLVARX
Dimensioning parameter used when several displacement or right-hand-side vectors are used.
NRHS
Number of load vectors. NRHS is 1 in most nonlinear problems: it is 2 for the modified Riks static procedure (“Static stress analysis,” Section 6.2.2 of the Abaqus Analysis User's Guide), and it is greater than 1 in some linear analysis procedures and during substructure generation.
NSVARS
User-defined number of solution-dependent state variables associated with the element (“Defining the number of solution-dependent variables that must be stored within the element” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide).
NPROPS
User-defined number of real property values associated with the element (“Defining the element properties” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide).
NJPROP
User-defined number of integer property values associated with the element (“Defining the element properties” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide).
MCRD
MCRD is defined as the maximum of the user-defined maximum number of coordinates needed at any node point (“Defining the maximum number of coordinates needed at any nodal point” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide) and the value of the largest active degree of freedom of the user element that is less than or equal to 3. For example, if you specify that the maximum number of coordinates is 1 and the active degrees of freedom of the user element are 2, 3, and 6, MCRD will be 3. If you specify that the maximum number of coordinates is 2 and the active degrees of freedom of the user element are 11 and 12, MCRD will be 2.
NNODE
User-defined number of nodes on the element (“Defining the number of nodes associated with the element” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide).
JTYPE
Integer defining the element type. This is the user-defined integer value n in element type Un (“Assigning an element type key to a user-defined element” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide).
KSTEP
Current step number.
KINC
Current increment number.
JELEM
User-assigned element number.
NDLOAD
Identification number of the distributed load or flux currently active on this element.
MDLOAD
Total number of distributed loads and/or fluxes defined on this element.
NPREDF
Number of predefined field variables, including temperature. For user elements Abaqus/Standard uses one value for each field variable per node.
MATERIALLIB
A variable that must be passed to the utility routines performing material point computations.
The solution variables (displacement, velocity, etc.) are arranged on a node/degree of freedom basis. The degrees of freedom of the first node are first, followed by the degrees of freedom of the second node, etc.
The values of 
(and, in direct-integration dynamic steps, 
and 
) enter user subroutine UELMAT as their latest approximations at the end of the time increment; that is, at time 
.
The values of 
enter the subroutine as their values at the beginning of the time increment; that is, at time t. It is your responsibility to define suitable time integration schemes to update . To ensure accurate, stable integration of internal state variables, you can control the time incrementation via PNEWDT.
The values of 
enter the subroutine as the values of the total load magnitude for the 
th distributed load at the end of the increment. Increments in the load magnitudes are also available.
In the following descriptions of the user element's requirements, it will be assumed that LFLAGS(3)=1 unless otherwise stated.
.
Automatic convergence checks are applied to the force residuals corresponding to degrees of freedom 1–7.
You must define AMATRX 
and RHS 
and update the state variables, .
Automatic convergence checks are applied to the force residuals corresponding to degrees of freedom 1–7.
LFLAGS(3)=1: Normal time increment. Either the Hilber-Hughes-Taylor or the backward Euler time integration scheme will be used. With 
set to zero for the backward Euler, both schemes imply
and 
; that is, the highest time derivative of in 
and 
is 
, so that 
as an internal state vector. If half-increment residual calculations are required, you must also store 
as an internal state vector, where 
indicates the time at the beginning of the previous increment. For 
, 
and is not needed. You must define AMATRX 
where 
and 
. RHS must also be defined and the state variables, , updated. Although the value of given in the dynamic step definition is passed into UELMAT, the value of can vary from element to element. For example, can be set to zero for some elements in the model where numerical dissipation is not desired.LFLAGS(3)=5: Half-increment residual (
) calculation. Abaqus/Standard will adjust the time increment so that 
(where 
is specified in the dynamic step definition). The half-increment residual is defined as
indicates the time at the beginning of the previous increment ( is a parameter of the Hilber-Hughes-Taylor time integration operator and will be set to zero if the backward Euler time integration operator is used). You must define RHS 
. To evaluate and 
, you must calculate 
. These half-increment values will not be saved. DTIME will still contain 
(not 
). The values contained in U, V, A, and DU are half-increment values.LFLAGS(3)=4: Velocity jump calculation. Abaqus/Standard solves 
for 
, so you must define AMATRX
.
LFLAGS(3)=6: Initial acceleration calculation. Abaqus/Standard solves 
for 
, so you must define AMATRX and RHS
.
The requirements are identical to those of static analysis, except that the automatic convergence checks are applied to the heat flux residuals corresponding to degrees of freedom 11, 12, …
Automatic convergence checks are applied to the heat flux residuals corresponding to degrees of freedom 11, 12, …
The backward difference scheme is always used for time integration; that is, Abaqus/Standard assumes that 
, where 
and so 
always. For degrees of freedom 11, 12, …, 
will be compared against the user-prescribed maximum allowable nodal temperature change in an increment, 
, for controlling the time integration accuracy.
You need to define AMATRX 
, where 
is the heat capacity matrix and RHS , and must update the state variables, .
“General and linear perturbation procedures,” Section 6.1.3 of the Abaqus Analysis User's Guide, describes the linear perturbation capabilities in Abaqus/Standard. Here, base state values of variables will be denoted by , , etc. Perturbation values will be denoted by 
, 
, etc.
Abaqus/Standard will not call user subroutine UELMAT for the following procedures: eigenvalue buckling prediction, response spectrum, transient modal dynamic, steady-state dynamic (modal and direct), and random response.
Abaqus/Standard will solve 
for 
, where 
is the base state stiffness matrix and the perturbation load vector, 
, is a linear function of the perturbation loads, 
; that is, 
.
LFLAGS(3)=1: You must define AMATRX 
and RHS 
.
LFLAGS(3)=100: You must compute perturbations of the internal variables, 
, and define RHS 
for output purposes.
Both a structural and a heat transfer user element have been created to demonstrate the usage of subroutine UELMAT. These user-defined elements are applied in a number of analyses. The following excerpt illustrates how the linearly elastic isotropic material available in Abaqus can be accessed from user subroutine UELMAT:
... *USER ELEMENT, TYPE=U1, NODES=4, COORDINATES=2, VAR=16, INTEGRATION=4, TENSOR=PSTRAIN 1,2 *ELEMENT, TYPE=U1, ELSET=SOLID 1, 1,2,3,4 ... *UEL PROPERTY, ELSET=SOLID, MATERIAL=MAT ... *MATERIAL, NAME=MAT *ELASTIC 7.00E+010, 0.33The user element defined above is a 4-node, fully integrated plane strain element, similar to the Abaqus CPE4 element.
The next excerpt shows the listing of the user subroutine. Inside the subroutine, a loop over the integration points is performed. For each integration point the utility routine MATERIAL_LIB_MECH is called, which returns stress and Jacobian at the integration point. These quantities are used to compute the right-hand-side vector and the element Jacobian.
.
for 
and 
, where 
is the base state stiffness matrix and 
is the base state mass matrix.c***********************************************************
subroutine uelmat(rhs,amatrx,svars,energy,ndofel,nrhs,
1 nsvars,props,nprops,coords,mcrd,nnode,u,du,
2 v,a,jtype,time,dtime,kstep,kinc,jelem,params,
3 ndload,jdltyp,adlmag,predef,npredf,lflags,mlvarx,
4 ddlmag,mdload,pnewdt,jprops,njpro,period,
5 materiallib)
c
include 'aba_param.inc'
C
dimension rhs(mlvarx,*), amatrx(ndofel, ndofel), props(*),
1 svars(*), energy(*), coords(mcrd, nnode), u(ndofel),
2 du(mlvarx,*), v(ndofel), a(ndofel), time(2), params(*),
3 jdltyp(mdload,*), adlmag(mdload,*), ddlmag(mdload,*),
4 predef(2, npredf, nnode), lflags(*), jprops(*)
parameter (zero=0.d0, dmone=-1.0d0, one=1.d0, four=4.0d0,
1 fourth=0.25d0,gaussCoord=0.577350269d0)
parameter (ndim=2, ndof=2, nshr=1,nnodemax=4,
1 ntens=4, ninpt=4, nsvint=4)
c
c ndim ... number of spatial dimensions
c ndof ... number of degrees of freedom per node
c nshr ... number of shear stress component
c ntens ... total number of stress tensor components
c (=ndi+nshr)
c ninpt ... number of integration points
c nsvint... number of state variables per integration pt
c (strain)
c
dimension stiff(ndof*nnodemax,ndof*nnodemax),
1 force(ndof*nnodemax), shape(nnodemax), dshape(ndim,nnodemax),
2 xjac(ndim,ndim),xjaci(ndim,ndim), bmat(nnodemax*ndim),
3 statevLocal(nsvint),stress(ntens), ddsdde(ntens, ntens),
4 stran(ntens), dstran(ntens), wght(ninpt)
c
dimension predef_loc(npredf),dpredef_loc(npredf),
1 defGrad(3,3),utmp(3),xdu(3),stiff_p(3,3),force_p(3)
dimension coord24(2,4),coords_ip(3)
data coord24 /dmone, dmone,
2 one, dmone,
3 one, one,
4 dmone, one/
c
data wght /one, one, one, one/
c
c*************************************************************
c
c U1 = first-order, plane strain, full integration
c
c State variables: each integration point has nsvint SDVs
c
c isvinc=(npt-1)*nsvint ... integration point counter
c statev(1+isvinc ) ... strain
c
c*************************************************************
if (lflags(3).eq.4) then
do i=1, ndofel
do j=1, ndofel
amatrx(i,j) = zero
end do
amatrx(i,i) = one
end do
goto 999
end if
c
c PRELIMINARIES
c
pnewdtLocal = pnewdt
if(jtype .ne. 1) then
write(7,*)'Incorrect element type'
call xit
endif
if(nsvars .lt. ninpt*nsvint) then
write(7,*)'Increase the number of SDVs to', ninpt*nsvint
call xit
endif
thickness = 0.1d0
c
c INITIALIZE RHS AND LHS
c
do k1=1, ndof*nnode
rhs(k1, 1)= zero
do k2=1, ndof*nnode
amatrx(k1, k2)= zero
end do
end do
c
c LOOP OVER INTEGRATION POINTS
c
do kintk = 1, ninpt
c
c EVALUATE SHAPE FUNCTIONS AND THEIR DERIVATIVES
c
c determine (g,h)
c
g = coord24(1,kintk)*gaussCoord
h = coord24(2,kintk)*gaussCoord
c
c shape functions
shape(1) = (one - g)*(one - h)/four;
shape(2) = (one + g)*(one - h)/four;
shape(3) = (one + g)*(one + h)/four;
shape(4) = (one - g)*(one + h)/four;
c
c derivative d(Ni)/d(g)
dshape(1,1) = -(one - h)/four;
dshape(1,2) = (one - h)/four;
dshape(1,3) = (one + h)/four;
dshape(1,4) = -(one + h)/four;
c
c derivative d(Ni)/d(h)
dshape(2,1) = -(one - g)/four;
dshape(2,2) = -(one + g)/four;
dshape(2,3) = (one + g)/four;
dshape(2,4) = (one - g)/four;
c
c compute coordinates at the integration point
c
do k1=1, 3
coords_ip(k1) = zero
end do
do k1=1,nnode
do k2=1,mcrd
coords_ip(k2)=coords_ip(k2)+shape(k1)*coords(k2,k1)
end do
end do
c
c INTERPOLATE FIELD VARIABLES
c
if(npredf.gt.0) then
do k1=1,npredf
predef_loc(k1) = zero
dpredef_loc(k1) = zero
do k2=1,nnode
predef_loc(k1) =
& predef_loc(k1)+
& (predef(1,k1,k2)-predef(2,k1,k2))*shape(k2)
dpredef_loc(k1) =
& dpredef_loc(k1)+predef(2,k1,k2)*shape(k2)
end do
end do
end if
c
c FORM B-MATRIX
c
djac = one
c
do i = 1, ndim
do j = 1, ndim
xjac(i,j) = zero
xjaci(i,j) = zero
end do
end do
c
do inod= 1, nnode
do idim = 1, ndim
do jdim = 1, ndim
xjac(jdim,idim) = xjac(jdim,idim) +
1 dshape(jdim,inod)*coords(idim,inod)
end do
end do
end do
djac = xjac(1,1)*xjac(2,2) - xjac(1,2)*xjac(2,1)
if (djac .gt. zero) then
! jacobian is positive - o.k.
xjaci(1,1) = xjac(2,2)/djac
xjaci(2,2) = xjac(1,1)/djac
xjaci(1,2) = -xjac(1,2)/djac
xjaci(2,1) = -xjac(2,1)/djac
else
! negative or zero jacobian
write(7,*)'WARNING: element',jelem,'has neg.
1 Jacobian'
pnewdt = fourth
endif
if (pnewdt .lt. pnewdtLocal) pnewdtLocal = pnewdt
c
do i = 1, nnode*ndim
bmat(i) = zero
end do
do inod = 1, nnode
do ider = 1, ndim
do idim = 1, ndim
irow = idim + (inod - 1)*ndim
bmat(irow) = bmat(irow) +
1 xjaci(idim,ider)*dshape(ider,inod)
end do
end do
end do
c
c CALCULATE INCREMENTAL STRAINS
c
do i = 1, ntens
dstran(i) = zero
end do
!
! set deformation gradient to Identity matrix
do k1=1,3
do k2=1,3
defGrad(k1,k2) = zero
end do
defGrad(k1,k1) = one
end do
c
c COMPUTE INCREMENTAL STRAINS
c
do nodi = 1, nnode
incr_row = (nodi - 1)*ndof
do i = 1, ndof
xdu(i)= du(i + incr_row,1)
utmp(i) = u(i + incr_row)
end do
dNidx = bmat(1 + (nodi-1)*ndim)
dNidy = bmat(2 + (nodi-1)*ndim)
dstran(1) = dstran(1) + dNidx*xdu(1)
dstran(2) = dstran(2) + dNidy*xdu(2)
dstran(4) = dstran(4) +
1 dNidy*xdu(1) +
2 dNidx*xdu(2)
c deformation gradient
defGrad(1,1) = defGrad(1,1) + dNidx*utmp(1)
defGrad(1,2) = defGrad(1,2) + dNidy*utmp(1)
defGrad(2,1) = defGrad(2,1) + dNidx*utmp(2)
defGrad(2,2) = defGrad(2,2) + dNidy*utmp(2)
end do
c
c CALL CONSTITUTIVE ROUTINE
c
isvinc= (kintk-1)*nsvint ! integration point increment
c
c prepare arrays for entry into material routines
c
do i = 1, nsvint
statevLocal(i)=svars(i+isvinc)
end do
c
c state variables
c
!DEC$ NOVECTOR
do k1=1,ntens
stran(k1) = statevLocal(k1)
stress(k1) = zero
end do
c
do i=1, ntens
!DEC$ NOVECTOR
do j=1, ntens
ddsdde(i,j) = zero
end do
ddsdde(i,j) = one
enddo
c
c compute characteristic element length
c
celent = sqrt(djac*dble(ninpt))
dvmat = djac*thickness
c
dvdv0 = one
call material_lib_mech(materiallib,stress,ddsdde,
1 stran,dstran,kintk,dvdv0,dvmat,defGrad,
2 predef_loc,dpredef_loc,npredf,celent,coords_ip)
c
do k1=1,ntens
statevLocal(k1) = stran(k1) + dstran(k1)
end do
c
isvinc= (kintk-1)*nsvint ! integration point increment
c
c update element state variables
c
do i = 1, nsvint
svars(i+isvinc)=statevLocal(i)
end do
c
c form stiffness matrix and internal force vector
c
dNjdx = zero
dNjdy = zero
do i = 1, ndof*nnode
force(i) = zero
do j = 1, ndof*nnode
stiff(j,i) = zero
end do
end do
dvol= wght(kintk)*djac
do nodj = 1, nnode
incr_col = (nodj - 1)*ndof
dNjdx = bmat(1+(nodj-1)*ndim)
dNjdy = bmat(2+(nodj-1)*ndim)
force_p(1) = dNjdx*stress(1) + dNjdy*stress(4)
force_p(2) = dNjdy*stress(2) + dNjdx*stress(4)
do jdof = 1, ndof
jcol = jdof + incr_col
force(jcol) = force(jcol) +
& force_p(jdof)*dvol
end do
do nodi = 1, nnode
incr_row = (nodi -1)*ndof
dNidx = bmat(1+(nodi-1)*ndim)
dNidy = bmat(2+(nodi-1)*ndim)
stiff_p(1,1) = dNidx*ddsdde(1,1)*dNjdx
& + dNidy*ddsdde(4,4)*dNjdy
& + dNidx*ddsdde(1,4)*dNjdy
& + dNidy*ddsdde(4,1)*dNjdx
stiff_p(1,2) = dNidx*ddsdde(1,2)*dNjdy
& + dNidy*ddsdde(4,4)*dNjdx
& + dNidx*ddsdde(1,4)*dNjdx
& + dNidy*ddsdde(4,2)*dNjdy
stiff_p(2,1) = dNidy*ddsdde(2,1)*dNjdx
& + dNidx*ddsdde(4,4)*dNjdy
& + dNidy*ddsdde(2,4)*dNjdy
& + dNidx*ddsdde(4,1)*dNjdx
stiff_p(2,2) = dNidy*ddsdde(2,2)*dNjdy
& + dNidx*ddsdde(4,4)*dNjdx
& + dNidy*ddsdde(2,4)*dNjdx
& + dNidx*ddsdde(4,2)*dNjdy
do jdof = 1, ndof
icol = jdof + incr_col
do idof = 1, ndof
irow = idof + incr_row
stiff(irow,icol) = stiff(irow,icol) +
& stiff_p(idof,jdof)*dvol
end do
end do
end do
end do
c
c assemble rhs and lhs
c
do k1=1, ndof*nnode
rhs(k1, 1) = rhs(k1, 1) - force(k1)
do k2=1, ndof*nnode
amatrx(k1, k2) = amatrx(k1, k2) + stiff(k1,k2)
end do
end do
end do ! end loop on material integration points
pnewdt = pnewdtLocal
c
999 continue
c
return
end