Explicit Solution Dependence
Since this routine provides access to material point quantities only at the start of the
increment, the material properties for a given increment are not influenced by the results
obtained during the increment. Hence, the accuracy of the results depends on the size of the
time increment. However, in most situations this is not a concern for explicit dynamic
analysis because the stable time increment is usually sufficiently small to ensure good
accuracy.
Defining Field Variables
Before user subroutine VUSDFLD is called, the values of the
field variables at the material point are calculated by interpolation from the values
defined at the nodes. Any changes to the field variables in the user subroutine are local to
the material point: the nodal field variables retain the values defined as initial
conditions or predefined field variables or the values defined in user subroutine VUFIELD. The values of the field
variables defined in this routine are used to calculate values of material properties that
are defined to depend on field variables and are passed into other user subroutines that are
called at the material point, such as the following:
Output of the user-defined field variables at the material points can be obtained with the
element integration point output variable
FV (see Element Integration Point Variables.)
State Variables
Since the redefinition of field variables in VUSDFLD is local to the current
increment (field variables are restored to the values interpolated from the nodal values at
the start of each increment,) any history dependence required to update material properties
by using this subroutine must be introduced with user-defined state variables.
The state variables can be updated in VUSDFLD and then passed into other
user subroutines that can be called at this material point, such as those listed above. The
number of such state variables can be specified as shown in the example at the end of this
section (see About User Subroutines and Utilities).
Accessing Material Point Data
The values of the material point quantities at the start of the increment can be accessed
through the utility routine VGETVRM described
in Obtaining Material Point Information in an Abaqus/Explicit Analysis. The values of the material point quantities are
obtained by calling VGETVRM with the
appropriate output variable keys.
Component Ordering in Symmetric Tensors
For symmetric tensors such as the stress and strain tensors there are
ndir+nshr components, and the component order is given as a
natural permutation of the indices of the tensor. The direct components are first and then
the indirect components, beginning with the 12-component. For example, a stress tensor
contains ndir direct stress components and
nshr shear stress components, which are returned as:
| Component |
2D Case |
3D Case |
| 1 |
|
|
| 2 |
|
|
| 3 |
|
|
| 4 |
|
|
| 5 |
|
|
| 6 |
|
|
The shear strain components in user subroutine VUSDFLD are stored as tensor
components and not as engineering components; unlike user subroutine USDFLD in Abaqus/Standard, which uses engineering components.
User Subroutine Interface
subroutine vusdfld(
c Read only variables -
1 nblock, nstatev, nfieldv, nprops, ndir, nshr,
2 jElem, kIntPt, kLayer, kSecPt,
3 stepTime, totalTime, dt, cmname,
4 coordMp, direct, T, charLength, props,
5 stateOld,
c Write only variables -
6 stateNew, field )
c
include 'vaba_param.inc'
c
dimension jElem(nblock), coordMp(nblock,*),
1 direct(nblock,3,3), T(nblock,3,3),
2 charLength(nblock), props(nprops),
3 stateOld(nblock,nstatev),
4 stateNew(nblock,nstatev),
5 field(nblock,nfieldv)
character*80 cmname
c
c Local arrays from vgetvrm are dimensioned to
c maximum block size (maxblk)
c
parameter( nrData=6 )
character*3 cData(maxblk*nrData)
dimension rData(maxblk*nrData), jData(maxblk*nrData)
c
do 100 k = 1, nblock
user coding to define field(nblock,nfieldv)
and, if necessary, stateNew(nblock,nstatev)
100 continue
c
return
end
Variables to Be Defined
-
field(nblock,nfieldv)
-
An array containing the field variables at the material points. These are passed in
with the values interpolated from the nodes at the end of the current increment, as
specified with initial condition definitions, predefined field variable definitions,
or user subroutine VUFIELD. The updated values
are used to calculate the values of material properties that are defined to depend on
field variables and are passed into other user subroutines that are called at the
material points.
Variables That Can Be Updated
-
stateNew(nblock,nstatev)
-
An array containing the solution-dependent state variables at the material points. In
all cases stateNew can be updated in this subroutine,
and the updated values are passed into other user subroutines that are called at the
material points. The number of state variables associated with this material point is
defined as described in Allocating Space for Solution-Dependent State Variables.
Variables Passed in for Information
-
nblock
-
Number of material points to be processed in this call to VUSDFLD.
-
nstatev
-
Number of user-defined state variables that are associated with this material type
(you define this as described in Allocating Space for Solution-Dependent State Variables).
-
nfieldv
-
Number of user-defined external field variables.
-
nprops
-
User-specified number of user-defined material properties.
-
ndir
-
Number of direct components in a symmetric tensor.
-
nshr
-
Number of indirect components in a symmetric tensor.
-
jElem
-
Array of element numbers.
-
kIntPt
-
Integration point number.
-
kLayer
-
Layer number (for composite shells).
-
kSecPt
-
Section point number within the current layer.
-
stepTime
-
Value of time since the step began.
-
totalTime
-
Value of total time. The time at the beginning of the step is given by
totalTime-stepTime.
-
dt
-
Time increment size.
-
cmname
-
User-specified material name, left justified. It is passed in as an uppercase
character string. 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.
-
coordMp(nblock,*)
-
Material point coordinates. It is the midplane material point for shell elements and
the centroid for beam elements.
-
direct(nblock,3,3)
-
An array containing the direction cosines of the material directions in terms of the
global basis directions. For material point k,
direct(k,1,1),
direct(k,2,1),
direct(k,3,1) give the (1, 2, 3) components of the
first material direction; direct(k,1,2),
direct(k,2,2),
direct(k,3,2) give the second material direction,
etc. For shell and membrane elements, the first two directions are in the plane of the
element and the third direction is the normal. This information is not available for
beam elements.
-
T(nblock,3,3)
-
An array containing the direction cosines of the material orientation components
relative to the element basis directions. For material point k, this is the
orientation that defines the material directions
(direct) in terms of the element basis directions.
For continuum elements T and
direct are identical. For shell and membrane elements
T(k,1,1)
, T(k,1,2)
, T(k,2,1)
, T(k,2,2)
, T(k,3,3)
and all other components are zero, where
is the counterclockwise rotation around the normal vector that
defines the orientation. If no orientation is used, T
is an identity matrix. Orientation is not available for beam elements.
-
charLength(nblock)
-
Characteristic element length, which is either the default value based on the
geometric mean or the user-defined characteristic element length defined in user
subroutine VUCHARLENGTH. The default value 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 the default value 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.
-
props(nprops)
-
User-supplied material properties.
-
stateOld (nblock, nstatev)
-
State variables at each material point at the beginning of the increment.
Example: Damaged Elasticity Model
Included below is an example of user subroutine VUSDFLD. In this example a truss
element is loaded in tension. A damaged elasticity model is introduced: the modulus
decreases as a function of the maximum tensile strain that occurred during the loading
history. The maximum tensile strain is stored as a solution-dependent state variable (see
Defining Solution-Dependent Field Variables).
- Input file
-
HEADING
Damaged elasticity model with user subroutine vusdfld
ELEMENT, TYPE=T2D2, ELSET=ONE
1, 1, 2
NODE, NSET=NALL
1, 0., 0.
2, 10., 0.
SOLID SECTION, ELSET=ONE, MATERIAL=ELASTIC
1.
MATERIAL, NAME=ELASTIC
ELASTIC, DEPENDENCIES=1
** Table of modulus values decreasing as a function
** of field variable 1.
2000., 0.3, 0., 0.00
1500., 0.3, 0., 0.01
1200., 0.3, 0., 0.02
1000., 0.3, 0., 0.04
DENSITY
1.0e-6
USER DEFINED FIELD
DEPVAR
1
1,EPSMAX,"Maximum strain value"
BOUNDARY
1, 1, 2
2, 2
AMPLITUDE, NAME=LOAD1
0.0, 0.0, 1.0, 1.0
AMPLITUDE, NAME=LOAD2
0.0, 0.0, 2.0, 1.0
AMPLITUDE, NAME=UNLOAD
0.0, 1.0, 1.0, 0.0
STEP, NLGEOM=NO
DYNAMIC, EXPLICIT
, 1.0
CLOAD, AMPLITUDE=LOAD1
2, 1, 20.
OUTPUT, FIELD, VARIABLE=PRESELECT
OUTPUT, HISTORY, VARIABLE=PRESELECT
ELEMENT OUTPUT, ELSET=ONE
S, E, SDV
NODE OUTPUT, NSET=NALL
RF, CF, U
END STEP
STEP, NLGEOM=NO
DYNAMIC, EXPLICIT
, 1.0
CLOAD, AMPLITUDE=UNLOAD
2, 1, 20.
END STEP
STEP, NLGEOM=NO
DYNAMIC, EXPLICIT
, 2.0
CLOAD, AMPLITUDE=LOAD2
2, 1, 40.
END STEP
- User subroutine
-
subroutine vusdfld(
c Read only -
* nblock, nstatev, nfieldv, nprops, ndir, nshr,
* jElem, kIntPt, kLayer, kSecPt,
* stepTime, totalTime, dt, cmname,
* coordMp, direct, T, charLength, props,
* stateOld,
c Write only -
* stateNew, field )
c
include 'vaba_param.inc'
c
dimension jElem(nblock), coordMp(nblock,*),
* direct(nblock,3,3), T(nblock,3,3),
* charLength(nblock), props(nprops),
* stateOld(nblock,nstatev),
* stateNew(nblock,nstatev),
* field(nblock,nfieldv)
character*80 cmname
c
c Local arrays from vgetvrm are dimensioned to
c maximum block size (maxblk)
c
parameter( nrData=6 )
character*3 cData(maxblk*nrData)
dimension rData(maxblk*nrData), jData(maxblk*nrData)
c
jStatus = 1
call vgetvrm( 'LE', rData, jData, cData, jStatus )
c
if( jStatus .ne. 0 ) then
call xplb_abqerr(-2,'Utility routine VGETVRM '//
* 'failed to get variable.',0,zero,' ')
call xplb_exit
end if
c
call setField( nblock, nstatev, nfieldv, nrData,
* rData, stateOld, stateNew, field)
c
return
end
subroutine setField( nblock, nstatev, nfieldv, nrData,
* strain, stateOld, stateNew, field )
c
include 'vaba_param.inc'
c
dimension stateOld(nblock,nstatev),
* stateNew(nblock,nstatev),
* field(nblock,nfieldv), strain(nblock,nrData)
c
do k = 1, nblock
c
c Absolute value of current strain:
eps = abs( strain(k,1) )
c
c Maximum value of strain up to this point in time:
epsmax = stateOld(k,1)
c
c Use the maximum strain as a field variable
field(k,1) = max( eps, epsmax )
c
c Store the maximum strain as a solution dependent state
stateNew(k,1) = field(k,1)
c
end do
c
return
end
|