User Subroutine Interface
subroutine ucoupledconstresp(
* stress, dDStress_dDStrain, dDStress_dGradT, dDStress_dGradSol,
* dDStress_dT, dDStress_dSol,
* qHeat, dqHeat_dDStrain, dqHeat_dGradT, dqHeat_dGradSol,
* dqHeat_dT, dqHeat_dSol,
* fluxesSol, dfluxes_dDstrain, dfluxes_dGradT, dfluxes_dGradSol,
* dfluxes_dT, dfluxes_dSol,
* qLoss, dqLoss_dDStrain, dqLoss_dGradT, dqLoss_dGradSol,
* dqLoss_dT, dqLoss_dSol,
* iCoupledAssemble_GradDep, iCoupledAssembleSoltnDep,
* iCoupledAssembleqLoss_GradDep, iCoupledAssembleqLoss_SoltnDep,
* nDim, nTens, nSolutionVar,
* props, nprops, predef, dpredef, npredef,
* statev, statevOld, nstatv,
* temp, dtemp,
* solutionVar, dSolutionVar,
* strain, dStrain, GradT, GradSol,
* coords,
* energy, time, dtime, CMNAME, ndi, nshr,
* celent, dRot, dFgrd0, dFgrd1, noel,
* npt, kstep, lFlags, kinc,
* i_array, niarray, r_array, nrarray, c_array, ncarray)
C
include 'aba_param.inc'
c Include below file to access property and parameter table.
include 'aba_tcs_param.inc'
c Include below file to access universal constants
include 'aba_phcon_param.inc'
c Include below file for parametrized location of various solution variables.
include 'aba_solutionvarloc.inc'
C
dimension strain(ntens),dStrain(ntens),
* stress(ntens),dDStress_dDStrain(ntens,ntens),
* dDStress_dGradT(ntens,ndim), dDStress_dGradSol(ntens,ndim,nsolutionvar),
* dDStress_dT(ntens),dDStress_dSol(ntens,nsolutionvar),
* qHeat(ndim),dqHeat_dDStrain(ndim,ntens),dqHeat_dGradT(ndim,ndim),
* dqHeat_dGradSol(ndim,ndim,nsolutionvar),dqHeat_dT(ndim),
* dqHeat_dSol(ndim,nsolutionvar),
* fluxesSol(ndim,nsolutionvar),dfluxes_dDstrain(ndim,ntens,nsolutionvar),
* dfluxes_dGradT(ndim,ndim,nsolutionvar),
* dfluxes_dGradSol(ndim,ndim,nsolutionvar,nsolutionvar),
* dfluxes_dT(ndim,nsolutionvar),dfluxes_dSol(ndim,nsolutionvar,nsolutionvar),
* dqLoss_dDStrain(ntens),dqLoss_dGradT(ndim),
* dqLoss_dGradSol(ndim,nsolutionvar),dqLoss_dSol(nSolutionVar),
* iCoupledAssemble_GradDep(nAllFieldsMax,nAllFieldsMax),
* iCoupledAssembleSoltnDep(nAllFieldsMax,nAllFieldsMax),
* iCoupledAssembleqLoss_GradDep(nAllFieldsMax), iCoupledAssembleqLoss_SoltnDep(nAllFieldsMax),
* props(nprops), predef(npredef),dpredef(npredef),statev(nstatv),statevOld(nstatv),
* solutionvar(nsolutionvar),dsolutionvar(nsolutionvar),
* gradT(ndim),gradSol(ndim,nSolutionVar),coords(*),
* energy(*),time1(2),drot(3,3),dfgrd0(3,3),dfgrd1(3,3),
* i_array(*),r_array(*), lFlags(*)
character*80 cmname, c_array(NCARRAY)
user coding
return
end
Variables to Be Defined
-
stress
- This array is passed in as the stress tensor at the beginning of the
increment and must be updated in this routine to be the stress tensor at the end of the
increment. If you specified initial stresses (Initial Conditions), this array will
contain the initial stresses at the start of the analysis. The size of this array
depends on the value of ntens as defined below. In
finite-strain problems the stress tensor has already been rotated to account for rigid
body motion. The measure of stress used is “true” (Cauchy) stress.
-
dDStress_dDStrain
- dDStress_dDStrain(I,J) defines the
change in the Ith stress component at the end of the time increment caused by an
infinitesimal perturbation of the Jth component of the strain increment array. Unless
you invoke the unsymmetric equation solution capability for the user-defined material,
Abaqus/Standard will use only the symmetric part of dDStress_dDStrain.
The symmetric part of the matrix is calculated by taking one half the sum of the matrix
and its transpose.
-
dDStress_dGradT
- dDStress_dGradT defines the variation
of the stress components with respect to the gradient of temperature
GradT.
-
dDStress_dGradSol
- dDStress_dGradSol defines the variation
of the stress components with respect to the gradient of the various solution variables
GradSol.
-
dDStress_dT
- dDStress_dT defines the variation of
the stress components with respect to the temperature
Temp.
-
dDStress_dSol
- dDStress_dSol defines the variation of
the stress components with respect to the other physics fields as defined in the
solution variables solutionvar.
-
qHeat
- Total heat flux from different fields.
-
dqHeat_dDStrain
- Variation of qHeat with respect to the
strain increments.
-
dqHeat_dGradT
- Variation of qHeat with respect to the
temperature gradients.
-
dqHeat_dGradSol
- Variation of qHeat with respect to the
gradient of the solution variables.
-
dqHeat_dT
- Variation of qHeat with respect to
temperature.
-
dqHeat_dSol
- Variation of qHeat with respect to the
solution variables.
-
fluxesSol
- Fluxes for the different physics fields defined by the solution
variables solutionvar.
-
dfluxes_dDStrain
- Variation of fluxesSol with respect to
the strain increments.
-
dfluxes_dGradT
- Variation of fluxesSol with respect to
the temperature gradients.
-
dfluxes_dGradSol
- Variation of fluxesSol with respect to
the gradient of the solution variables.
-
dfluxes_dT
- Variation of fluxesSol with respect to
temperature.
-
dfluxes_dSol
- Variation of fluxesSol with respect to
the solution variables.
-
qLoss
- Volumetric heat generation per unit time at the end of the increment,
which can be similar to RPL in UMAT.
-
dqLoss_dDStrain
- Variation of qLoss with respect to the
strain increments.
-
dqLoss_dGradT
- Variation of qLoss with respect to the
temperature gradients.
-
dqLoss_dGradSol
- Variation of qLoss with respect to the
gradient of the solution variables.
-
dqLoss_dT
- Variation of qLoss with respect to
temperature.
-
dqLoss_dSol
- Variation of qLoss with respect to the
solution variables.
-
iCoupledAssemble_GradDep
- An array of integer flags of dimension
(nAllFieldsMax,
nAllFieldsMax) that indicates whether the variation of
fluxesSol with respect to the gradients of the
different fields must be assembled. These gradient-dependent flags are used for
performance to avoid assembling zeros.
If you have gradient-dependent terms to be
assembled, specify a value of 1 in the specific locations for the different fields.
The default is set to 0. The table below illustrates an example of the
assembly flag set for assembling the gradient-dependent terms for the electric
potential flux with respect to the gradient of other fields.
| iCoupledAssemble_GradDep(i_sol_phiS,
i_sol_phiS) |
If set to 1, assemble gradient dependence of electric potential flux with
respect to the gradient of the electric potential field. |
| iCoupledAssemble_GradDep(i_sol_phiS,
i_sol_phiE) |
If set to 1, assemble gradient dependence of electric potential flux with
respect to the gradient of electric potential in the electrolyte. |
| iCoupledAssemble_GradDep(i_sol_phiS,
i_sol_Ce) |
If set to 1, assemble gradient dependence of electric potential flux with
respect to the gradient of ion concentration in the electrolyte. |
| iCoupledAssemble_GradDep(i_sol_phiS,
i_sol_solidC) |
If set to 1, assemble gradient dependence of electric potential flux with
respect to the gradient of species concentration. |
| iCoupledAssemble_GradDep(i_sol_phiS,
i_sol_porP) |
If set to 1, assemble gradient dependence of electric potential flux with
respect to the gradient of pore pressure. |
| iCoupledAssemble_GradDep(i_sol_phiS,
i_sol_temp) |
If set to 1, assemble gradient dependence of electric potential flux with
respect to gradient of temperature. |
| iCoupledAssemble_GradDep(i_sol_phiS,
i_sol_disp) |
If set to 1, assemble gradient dependence of electric potential flux with
respect to the gradient of displacement field. |
-
iCoupledAssembleSoltnDep
-
An array of integer flags of dimension (nAllFieldsMax
and nAllFieldsMax) that indicates whether the variation
of fluxesSol with respect to the solution variables
solutionVar for the different fields must be
assembled.
If you have solution-dependent terms to be assembled, specify a value of 1 in the
specific locations for the different fields. The default is set to 0.
The table below illustrates an example of assembling the solution dependence of ion
concentration flux with respect to the other fields.
| iCoupledAssembleSoltnDep(i_sol_Ce,
i_sol_phiS) |
If set to 1, assemble dependence of ion concentration flux with respect
to electric potential field. |
| iCoupledAssembleSoltnDep(i_sol_Ce,
i_sol_phiE) |
If set to 1, assemble dependence of ion concentration flux with respect
to electric potential in the electrolyte. |
| iCoupledAssembleSoltnDep(i_sol_Ce,
i_sol_Ce) |
If set to 1, assemble dependence of ion concentration flux with respect
to ion concentration in the electrolyte. |
| iCoupledAssembleSoltnDep(i_sol_Ce,
i_sol_solidC) |
If set to 1, assemble dependence of ion concentration flux with respect
to species concentration. |
| iCoupledAssembleSoltnDep(i_sol_Ce,
i_sol_porP) |
If set to 1, assemble dependence of ion concentration flux with respect
to pore pressure. |
| iCoupledAssembleSoltnDep(i_sol_Ce,
i_sol_Temp) |
If set to 1, assemble dependence of ion concentration flux with respect
to temperature. |
| iCoupledAssembleSoltnDep(i_sol_Ce,
i_sol_Disp) |
If set to 1, assemble dependence of ion concentration flux with respect
to displacement field. |
-
iCoupledAssembleqLoss_GradDep
- An array of integer flags of dimension
(nAllFieldsMax) that indicates whether the variation of
qloss with respect to the gradients of the different
fields must be assembled.
If you have gradient-dependent terms to be assembled,
specify a value of 1 in the specific locations for the different fields. The default
is set to 0.
| iCoupledAssembleqLoss_GradDep(i_sol_phiS) |
If set to 1, assemble dependence of heat loss with respect to the
gradient in electric potential field. |
| iCoupledAssembleqLoss_GradDep(i_sol_phiE) |
If set to 1, assemble dependence of heat loss with respect to the
gradient in electric potential in the electrolyte. |
| iCoupledAssembleqLoss_GradDep(i_sol_Ce) |
If set to 1, assemble dependence of heat loss with respect to gradient in
ion concentration in the electrolyte. |
| iCoupledAssembleqLoss_GradDep(i_sol_solidC) |
If set to 1, assemble dependence of heat loss with respect to the
gradient in species concentration. |
| iCoupledAssembleqLoss_GradDep(i_sol_porP) |
If set to 1, assemble dependence of heat loss with respect to the
gradient in pore pressure. |
| iCoupledAssembleqLoss_GradDep(i_sol_Temp) |
If set to 1, assemble dependence of heat loss with respect to the
gradient in temperature. |
| iCoupledAssembleqLoss_GradDep(i_sol_Disp) |
If set to 1, assemble dependence of heat loss with respect to the
gradient in displacement field. |
-
iCoupledAssembleqLoss_SoltnDep
- An array of integer flags of dimension
(nAllFieldsMax) that indicates whether the variation of
qloss with respect to the solution variables of the
different fields must be assembled.
If you have solution-dependent terms to be
assembled, specify a value of 1 in the specific locations for the different fields.
The default is set to 0.
| iCoupledAssembleqLoss_SoltnDep(i_sol_phiS) |
If set to 1, assemble dependence of heat loss with respect to electric
potential field. |
| iCoupledAssembleqLoss_SoltnDep(i_sol_phiE) |
If set to 1, assemble dependence of heat loss with respect to electric
potential in the electrolyte. |
| iCoupledAssembleqLoss_SoltnDep(i_sol_Ce) |
If set to 1, assemble dependence of heat loss with respect to ion
concentration in the electrolyte. |
| iCoupledAssembleqLoss_SoltnDep(i_sol_solidC) |
If set to 1, assemble dependence of heat loss with respect to species
concentration. |
| iCoupledAssembleqLoss_SoltnDep(i_sol_porP) |
If set to 1, assemble dependence of heat loss with respect to pore
pressure. |
| iCoupledAssembleqLoss_SoltnDep(i_sol_Temp) |
If set to 1, assemble dependence of heat loss with respect to
temperature. |
| iCoupledAssembleqLoss_SoltnDep(i_sol_Disp) |
If set to 1, assemble dependence of heat loss with respect to
displacement field. |
Variables That Can Be Updated
-
statev
-
Current value of the solution-dependent variables.
Variables Passed in for Information
-
ndim
-
Number of spatial dimensions.
-
ntens
-
Size of the stress or strain component array.
-
nsolutionVar
-
Number of solution variables.
-
props
-
User-specified array of material constants associated with this user material.
-
nprops
-
User-defined number of material constants associated with this user material.
-
predef
-
Array of interpolated values of predefined field variables at this point at the start
of the increment, based on the values read in at the nodes.
-
dpredef
-
Array of increments of predefined field variables.
-
npredef
-
Number of predefined field variables.
-
statevold
-
Array containing the user-defined solution-dependent state variables at the end of
the previous increment.
-
nstatev
-
Number of solution-dependent state variables that are associated with this material
type (defined as described in Allocating Space for Solution-Dependent State Variables).
-
Temp
-
Current temperature.
-
dTemp
-
Incremental temperature.
-
solutionVar
-
Current value of the solution variables.
| solutionVar(i_sol_phiS) |
Current value of the electric potential. |
| solutionVar(i_sol_phiE) |
Current value of the electric potential in the electrolyte. |
| solutionVar(i_sol_Ce) |
Current value of the ionic concentration in the electrolyte. |
| solutionVar(i_sol_solidC) |
Current value of the species concentration. |
| solutionVar(i_sol_porP) |
Current value of the pore pressure. |
-
dsolutionVar
-
Incremental value of the solution variables.
| dsolutionVar(i_sol_phiS) |
Incremental value of the electric potential. |
| dsolutionVar(i_sol_phiE) |
Incremental value of the electric potential in the electrolyte. |
| dsolutionVar(i_sol_Ce) |
Incremental value of the ionic concentration in the electrolyte. |
| dsolutionVar(i_sol_solidC) |
Incremental value of the species concentration. |
| dsolutionVar(i_sol_porP) |
Incremental value of the pore pressure. |
-
strain
-
An array containing the total strains at the beginning of the increment. If thermal
expansion is included in the same material definition, the strains passed into UCOUPLEDCONSTRESP are the
mechanical strains only (that is, the thermal strains computed based on the thermal
expansion coefficient have been subtracted from the total strains). These strains are
available for output as the “elastic” strains.
In finite-strain problems the strain components have been rotated to account for
rigid body motion in the increment before UCOUPLEDCONSTRESP is called
and are approximations to logarithmic strain.
-
dStrain
-
Array of strain increments. If thermal expansion is included in the same material
definition, these are the mechanical strain increments (the total strain increments
minus the thermal strain increments).
-
gradT
-
Current values of the spatial gradients of temperature.
-
gradSol
-
Current values of the spatial gradients of solution variables (see
solutionVar).
-
coords
-
An array containing the current coordinates of this integration point. These are the
current coordinates if geometric nonlinearity is accounted for during the step;
otherwise, the array contains the original coordinates of the point.
-
time(1)
-
Current value of step time.
-
time(2)
-
Current value of total time.
-
dtime
-
Time increment.
-
cmName
-
User-defined material name, left justified. Some internal material models are given
names starting with the “ABQ_” character string. To
avoid conflict, you should not use “ABQ_” as the
leading string for CMNAME.
-
ndi
-
Number of direct stress components at this point.
-
nshr
-
Number of engineering shear stress components at this point.
-
celent
-
Characteristic element length, which is a typical length of a line across an element
for a first-order element.
-
dRot
-
Rotation increment matrix. This matrix represents the increment of rigid body
rotation of the basis system in which the components of stress and 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 UCOUPLEDCONSTRESP 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 (when a local orientation is used).
-
dFgrd0
-
Array containing the deformation gradient at the beginning of the increment. If a
local orientation is defined at the material point, the deformation gradient
components are expressed in the local coordinate system defined by the orientation at
the beginning of the increment. For more information about the availability of the
deformation gradient for various element types, see Deformation Gradient.
-
dFgrd1
-
Array containing the deformation gradient at the end of the increment. If a local
orientation is defined at the material point, the deformation gradient components are
expressed in the local coordinate system defined by the orientation. This array is set
to the identity matrix if nonlinear geometric effects are not included in the step
definition associated with this increment. For more information about the availability
of the deformation gradient for various element types, see Deformation Gradient.
-
noel
-
User-assigned element number.
-
npt
-
Integration point number.
-
kstep
-
Current step number.
-
lFlags
-
An array containing the flags that define the current solution procedure and analysis
type.
| lFlags(1)
|
Defines the procedure type. See Results File 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 Perturbation Procedures.
|
-
kinc
-
Current increment number.
-
i_array
-
Not used.
-
niarray
-
Size of array i_array.
-
r_array
-
Not used.
-
nrarray
-
Size of array r_array.
-
c_array
-
Not used.
-
ncarray
-
Size of array c_array.
|