Product: ABAQUS/Standard
User subroutine UEXPAN:
can be used to define incremental thermal strains as functions of temperature, predefined field variables, and state variables;
is intended for models in which the thermal strains depend on temperature and/or predefined field variables in complex ways or depend on state variables, which can be used and updated in this routine;
is called at all integration points of elements for which the material or gasket behavior definition contains user-subroutine-defined thermal expansion; and
is called twice per material point in each iteration during coupled temperature-displacement analysis.
SUBROUTINE UEXPAN(EXPAN,DEXPANDT,TEMP,TIME,DTIME,PREDEF,
1 DPRED,STATEV,CMNAME,NSTATV,NOEL)
C
INCLUDE 'ABA_PARAM.INC'
C
CHARACTER*80 CMNAME
C
DIMENSION EXPAN(*),DEXPANDT(*),TEMP(2),TIME(2),PREDEF(*),
1 DPRED(*),STATEV(NSTATV)
user coding to define EXPAN, DEXPANDT and update
STATEV if necessary.
RETURN
ENDEXPAN(*)
Increments of thermal strain. The number of values to be defined and the order in which they are arranged depend on the type of thermal expansion being defined.
For isotropic expansion give the isotropic thermal strain increment as the first and only component of the matrix.
For orthotropic expansion give 
, 
, and 
as the first, second, and third components of the matrix, respectively.
For anisotropic expansion give , , , 
, 
, and 
. Direct components are stored first, followed by shear components in the order presented here. For plane stress only three components of the matrix are needed; give , , and , as the first, second, and third components, respectively.
DEXPANDT(*)
Variation of thermal strains with respect to temperature, 
. The number of values and the order in which they are arranged depend on the type of thermal expansion being defined.
For isotropic expansion give the variation of the isotropic thermal strain with respect to temperature as the first and only component of the matrix.
For orthotropic expansion give 
, 
, and 
as the first, second, and third components of the matrix, respectively.
For anisotropic expansion give , , , 
, 
, and 
. Direct components are stored first, followed by shear components in the order presented here. For plane stress only three components of the matrix are needed; give , , and , as the first, second, and third components, respectively.
STATEV(NSTATV)
Array containing the user-defined solution-dependent state variables at this point. Except for coupled temperature-displacement analysis, these are supplied as values at the start of the increment and can be updated to their values at the end of the increment. For coupled temperature-displacement analysis, UEXPAN is called twice per material point per iteration. In the first call for a given material point and iteration, the values supplied are those at the start of the increment and can be updated. In the second call for the same material point and iteration, the values supplied are those returned from the first call, and they can be updated again to their values at the end of the increment.
User subroutine UEXPAN allows for the incremental thermal strains to be only weakly dependent on the state variables. The Jacobian terms arising from the derivatives of the thermal strains with respect to the state variables are not taken into account.
TEMP(1)
Current temperature (at the end of the increment).
TEMP(2)
Temperature increment.
TIME(1)
Step time at the end of the increment.
TIME(2)
Total time at the end of the increment.
DTIME
Time increment.
PREDEF(*)
Array containing the values of all the user-specified predefined field variables at this point (initial values at the beginning of the analysis and current values during the analysis).
DPRED(*)
Array of increments of predefined field variables.
CMNAME
User-specified material name or gasket behavior name, left justified.
NSTATV
Number of solution-dependent state variables associated with this material or gasket behavior type (specified when space is allocated for the array; see “Allocating space” in “User subroutines: overview,” Section 13.2.1 of the ABAQUS Analysis User's Manual).
NOEL
User-defined element number.