is performed when the mechanical and thermal solutions affect each other strongly and,
therefore, must be obtained simultaneously;
requires the existence of elements with both temperature and displacement degrees of
freedom in the model;
can be used to analyze time-dependent material response;
cannot include cavity radiation effects but might include average-temperature radiation
conditions (see Thermal Loads); and
takes into account temperature dependence of material properties only for the properties
that are assigned to elements with temperature degrees of freedom.
In Abaqus/Standard a fully coupled thermal-stress analysis:
neglects inertia effects; and
can be transient or steady-state.
In Abaqus/Explicit a fully coupled thermal-stress analysis:
Fully coupled thermal-stress analysis is needed when the stress analysis is dependent on
the temperature distribution and the temperature distribution depends on the stress
solution. For example, metalworking problems might include significant heating due to
inelastic deformation of the material that, in turn, changes the material properties. In
addition, contact conditions exist in some problems where the heat conducted between
surfaces might depend strongly on the separation of the surfaces or the pressure transmitted
across the surfaces (see Thermal Contact Properties). For such cases
the thermal and mechanical solutions must be obtained simultaneously rather than
sequentially. Coupled temperature-displacement elements are provided for this purpose in
both Abaqus/Standard and Abaqus/Explicit; however, each program uses different algorithms to solve coupled thermal-stress
problems.
Fully Coupled Thermal-Stress Analysis in Abaqus/Standard
In Abaqus/Standard the temperatures are integrated using a backward-difference scheme, and the nonlinear
coupled system is solved using Newton's method. Abaqus/Standard offers an exact as well as an approximate implementation of Newton's method for fully
coupled temperature-displacement analysis.
Exact Implementation
An exact implementation of Newton's method involves a nonsymmetric Jacobian matrix as is
illustrated in the following matrix representation of the coupled equations:
where and are the respective corrections to the incremental displacement and
temperature, are submatrices of the fully coupled Jacobian matrix, and and are the mechanical and thermal residual vectors, respectively.
Solving this system of equations requires the use of the unsymmetric matrix storage and
solution scheme. In addition, the mechanical and thermal equations must be solved
simultaneously. The method provides quadratic convergence when the solution estimate is
within the radius of convergence of the algorithm. The exact implementation is used by
default.
Approximate Implementation
Some problems require a fully coupled analysis in the sense that the mechanical and
thermal solutions evolve simultaneously, but with a weak coupling between the two
solutions. In other words, the components in the off-diagonal submatrices are small compared to the components in the diagonal submatrices . An example of such a situation is the disc brake problem (Thermal-stress analysis of a disc brake). For these
problems a less costly solution might be obtained by setting the off-diagonal submatrices
to zero so that we obtain an approximate set of equations:
As a result of this approximation the thermal and mechanical equations can be solved
separately, with fewer equations to consider in each subproblem. The savings due to this
approximation, measured as solver time per iteration, will be of the order of a factor of
two, with similar significant savings in solver storage of the factored stiffness matrix.
Further, in many situations the subproblems might be fully symmetric or approximated as
symmetric, so that the less costly symmetric storage and solution scheme can be used. The
solver time savings for a symmetric solution is an additional factor of two. Unless you
explicitly choose the unsymmetric matrix storage and solution scheme, selection of the
scheme depends on other details of the problem (see Defining an Analysis).
This modified form of Newton's method does not affect solution accuracy since the fully
coupled effect is considered through the residual vector at each increment in time. However, the rate of convergence is no longer
quadratic and depends strongly on the magnitude of the coupling effect, so more iterations
are generally needed to achieve equilibrium than with the exact implementation of Newton's
method. When the coupling is significant, the convergence rate becomes very slow and may
prohibit obtaining a solution. In such cases the exact implementation of Newton's method
is required. In cases where it is possible to use this approximation, the convergence in
an increment depends strongly on the quality of the first guess to the incremental
solution, which you can control by selecting the extrapolation method used for the step
(see Defining an Analysis).
Input File Usage
Use the following option to specify a separated solution scheme:
A steady-state coupled temperature-displacement analysis can be performed in Abaqus/Standard. In steady-state cases you should assign an arbitrary “time” scale to the step: you
specify a “time” period and “time” incrementation parameters. This time scale is
convenient for changing loads and boundary conditions through the step and for obtaining
solutions to highly nonlinear (but steady-state) cases; however, for the latter purpose,
transient analysis often provides a natural way of coping with the nonlinearity.
Frictional slip heat generation is normally neglected in for the steady-state case.
However, it can still be accounted for if user subroutine FRIC provides the incremental
frictional dissipation through the variable SFD. If
frictional heat generation is present, the heat flux into the two contact surfaces depends
on the slip rate of the surfaces. The “time” scale in this case cannot be described as
arbitrary, and a transient analysis should be performed.
Alternatively, you can perform a transient coupled temperature-displacement analysis. You
can control the time incrementation in a transient analysis directly, or Abaqus/Standard can control it automatically. Automatic time incrementation is generally preferred.
Automatic Incrementation Controlled by a Maximum Allowable Temperature
Change
The time increments can be selected automatically based on a user-prescribed maximum
allowable nodal temperature change in an increment, . Abaqus/Standard restricts the time increments to ensure that this value is not exceeded at any node
(except nodes with boundary conditions) during any increment of the analysis (see Time Integration Accuracy in Transient Problems).
Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient; Incrementation: Type: Automatic, Max. allowable temperature change per increment:
Fixed Incrementation
If you do not specify , fixed time increments equal to the user-specified initial time
increment, , is used throughout the analysis, except when the explicit creep
integration scheme is used. In this case Abaqus/Standard might decrease the time increment if the stability limit is exceeded.
Spurious Oscillations due to Small Time Increments
In transient analysis with second-order elements there is a relationship between the
minimum usable time increment and the element size. A simple guideline is
where is the time increment, is the density, c is the specific heat,
k is the thermal conductivity, and is a typical element dimension (such as the length of a side of an
element). If time increments smaller than this value are used in a mesh of second-order
elements, spurious oscillations can appear in the solution, in particular in the
vicinity of boundaries with rapid temperature changes. These oscillations are
nonphysical and might cause problems if temperature-dependent material properties are
present. In transient analyses using first-order elements the heat capacity terms are
lumped, which eliminates such oscillations but can lead to locally inaccurate solutions
for small time increments. If smaller time increments are required, a finer mesh should
be used in regions where the temperature changes rapidly.
There is no upper limit on the time increment size (the integration procedure is
unconditionally stable) unless nonlinearities cause convergence problems.
Automatic Incrementation Controlled by the Creep Response
The accuracy of the integration of time-dependent (creep) material behavior is governed
by the user-specified accuracy tolerance parameter, . This parameter is used to prescribe the maximum strain rate change
allowed at any point during an increment, as described in Rate-Dependent Plasticity: Creep and Swelling. The accuracy
tolerance parameter can be specified together with the maximum allowable nodal
temperature change in an increment, (described above); however, specifying the accuracy tolerance
parameter activates automatic incrementation even if is not specified.
Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient, Include creep/swelling/viscoelastic behavior; Incrementation: Type: Automatic, Max. allowable temperature change per increment: , Creep/swelling/viscoelastic strain error tolerance:tolerance
Selecting Explicit Creep Integration
Nonlinear creep problems (Rate-Dependent Plasticity: Creep and Swelling) that exhibit
no other nonlinearities can be solved efficiently by forward-difference integration of
the inelastic strains if the inelastic strain increments are smaller than the elastic
strains. This explicit method is efficient computationally because, unlike implicit
methods, iteration is not required if no other nonlinearities are present. Although this
method is only conditionally stable, the numerical stability limit of the explicit
operator is in many cases sufficiently large to allow the solution to be developed in a
reasonable number of time increments.
For most coupled thermal-stress analyses, however, the unconditional stability of the
backward difference operator (implicit method) is desirable. In such cases the implicit
integration scheme may be invoked automatically by Abaqus/Standard.
Explicit integration can be less expensive computationally and simplifies
implementation of user-defined creep laws in user subroutine CREEP; you can restrict Abaqus/Standard to using this method for creep problems (with or without geometric nonlinearity
included). See Rate-Dependent Plasticity: Creep and Swelling for further
details.
Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient, toggle off Include creep/swelling/viscoelastic behavior
Unstable Problems
Some types of analyses may develop local instabilities, such as surface wrinkling,
material instability, or local buckling. In such cases it may not be possible to obtain
a quasi-static solution, even with the aid of automatic incrementation. Abaqus/Standard offers a method of stabilizing this class of problems by applying damping throughout
the model in such a way that the viscous forces introduced are sufficiently large to
prevent instantaneous buckling or collapse but small enough not to affect the behavior
significantly while the problem is stable. The available automatic stabilization schemes
are described in detail in Automatic Stabilization of Unstable Problems.
Units
In coupled problems where two different fields are active, take care when choosing the
units of the problem. If the choice of units is such that the terms generated by the
equations for each field are different by many orders of magnitude, the precision on some
computers might be insufficient to resolve the numerical ill-conditioning of the coupled
equations. Therefore, choose units that avoid ill-conditioned matrices. For example,
consider using units of megapascal (MPa) instead of pascal (Pa) for the stress equilibrium
equations to reduce the disparity between the magnitudes of the stress equilibrium
equations and the heat flux continuity equations.
Fully Coupled Thermal-Stress Analysis in Abaqus/Explicit
In Abaqus/Explicit the heat transfer equations are integrated using the explicit forward-difference time
integration rule
where is the temperature at node N and the subscript
i refers to the increment number in an explicit dynamic step. The
forward-difference integration is explicit in the sense that no equations need to be solved
when a lumped capacitance matrix is used. The current temperatures are obtained using known
values of from the previous increment. The values of are computed at the beginning of the increment by
where is the lumped capacitance matrix, is the applied nodal source vector, and is the internal flux vector.
The mechanical solution response is obtained using the explicit central-difference
integration rule with a lumped mass matrix as described in Explicit Dynamic Analysis. Since both the forward-difference and central-difference
integrations are explicit, the heat transfer and mechanical solutions are obtained
simultaneously by an explicit coupling. Therefore, no iterations or tangent stiffness
matrices are required.
Explicit integration can be less expensive computationally and simplifies the treatment of
contact. For a comparison of explicit and implicit direct-integration procedures, see About Dynamic Analysis Procedures.
Stability
The explicit procedure integrates through time by using many small time increments. The
central-difference and forward-difference operators are conditionally stable. The
stability limit for both operators (with no damping in the mechanical solution response)
is obtained by choosing
where is the highest frequency in the system of equations of the mechanical
solution response and is the largest eigenvalue in the system of equations of the thermal
solution response.
Estimating the Time Increment Size
An approximation to the stability limit for the forward-difference operator in the
thermal solution response is given by
where is the smallest element dimension in the mesh and is the thermal diffusivity of the material. The parameters
k, , and c represent the material's thermal
conductivity, density, and specific heat, respectively.
In most applications of explicit analysis the mechanical response governs the stability
limit. The thermal response might govern the stability limit when material parameter
values are nonphysical or a very large amount of mass scaling is used. The calculation
of the time increment size for the mechanical solution response is discussed in Explicit Dynamic Analysis.
Stable Time Increment Report
Abaqus/Explicit writes a report to the status (.sta) file during the data check
phase of the analysis that contains an estimate of the minimum stable time increment and
a listing of the elements with the smallest stable time increments and their values. The
initial minimum stable time increment accounts for the stability requirements of both
the thermal and mechanical solution responses. The initial stable time increments listed
do not include damping (bulk viscosity), mass scaling, or penalty contact effects in the
mechanical solution response.
This listing is provided because often a few elements have much smaller stability
limits than the rest of the elements in the mesh. The stable time increment can be
increased by modifying the mesh to increase the size of the controlling element or by
using appropriate mass scaling.
Time Incrementation
The time increment used in an analysis must be smaller than the stability limits of the
central- and forward-difference operators. Failure to use such a time increment results in
an unstable solution. When the solution becomes unstable, the time history response of
solution variables, such as displacements, usually oscillates with increasing amplitudes.
The total energy balance also changes significantly.
Abaqus/Explicit has two strategies for time incrementation control: fully automatic time incrementation
(where the code accounts for changes in the stability limit) and fixed time
incrementation.
Scaling the Time Increment
To reduce the chance of a solution going unstable, the stable time increment computed
by Abaqus/Explicit can be adjusted by a constant scaling factor. This factor can be used to scale the
default global time estimate, the element-by-element estimate, or the fixed time
increment based on the initial element-by-element estimate; it cannot be used to scale a
fixed time increment that you specified directly.
The default time incrementation scheme in Abaqus/Explicit is fully automatic and requires no user intervention. Two types of estimates are used
to determine the stability limit: element-by-element for both the thermal and mechanical
solution responses and global for the mechanical solution response. An analysis always
starts by using the element-by-element estimation method and may switch to the global
estimation method under certain circumstances, as explained in Explicit Dynamic Analysis.
In an analysis Abaqus/Explicit initially uses a stability limit based on the thermal and mechanical solution
responses in the whole model. This element-by-element estimate is determined using the
smallest time increment size due to the thermal and mechanical solution responses in
each element.
The element-by-element estimate is conservative; it gives a smaller stable time
increment than the true stability limit, which is based on the maximum frequency of the
entire model. In general, constraints such as boundary conditions and kinematic contact
have the effect of compressing the eigenvalue spectrum, and the element-by-element
estimates do not take this into account (see Explicit Dynamic Analysis)
The stable time increment size due to the mechanical solution response is determined by
the global estimator as the step proceeds unless the element-by-element estimator is
chosen, fixed time incrementation is specified, or one of the conditions explained in
Explicit Dynamic Analysis prevents the use of global estimation. The
stable time increment size due to the thermal solution response is always determined by
using an element-by-element estimation method. The switch to the global estimation
method in mechanical solution response occurs once the algorithm determines that the
accuracy of the global estimation method is acceptable. For details, see Explicit Dynamic Analysis
For three-dimensional continuum elements and elements with plane stress formulations
(shell, membrane, and two-dimensional plane stress elements) an improved
estimate of the element characteristic length is used by default. This
improved method usually results in a larger element stable time increment
than a more traditional method. For analyses using variable mass scaling, the total mass
added to achieve a given stable time increment is less with the improved estimate.
Input File Usage
Use the following option to specify the element-by-element estimation
method:
A fixed time incrementation scheme is also available in Abaqus/Explicit. The fixed time increment size is determined either by the initial element-by-element
stability estimate for the step or by a user-specified time increment.
Fixed time incrementation might be useful when a more accurate representation of the
higher mode response of a problem is required. In this case a time increment size
smaller than the element-by-element estimates may be used. The element-by-element
estimate can be obtained by running a data check analysis (see Abaqus/Standard and Abaqus/Explicit Execution).
When fixed time incrementation is used, Abaqus/Explicit does not check that the computed response is stable during the step. You should
ensure that a valid response has been obtained by carefully checking the energy history
and other response variables.
If you choose to use time increments the size of the initial element-by-element
stability limit throughout a step, the dilatational wave speed and the thermal
diffusivity in each element at the beginning of the step are used to compute the fixed
time increment size. To reduce the chance of a solution going unstable, the initial
stable time increment that Abaqus/Explicit computes can be adjusted by a constant scaling factor, as described above in Scaling the Time Increment. Alternatively, you can specify a time increment size directly.
Input File Usage
Use the following option to request time increments the size of the
element-by-element stability limit:
Step module: Create Step: General: Dynamic, Temp-disp, Explicit: Incrementation: Type: Fixed, Use element-by-element time increment estimator or User-defined time increment:
Reducing the Computational Cost by Using Selective Subcycling
The selective subcycling method can be used in a coupled thermal-stress analysis exactly
as in a pure mechanical analysis, as described in Explicit Dynamic Analysis
and Selective Subcycling.
Monitoring Output Variables for Extreme Values
The extreme values defined as the element and nodal variables in a coupled thermal-stress
analysis can be monitored exactly as described in Explicit Dynamic Analysis
for a pure mechanical analysis.
Initial Conditions
By default, the initial temperature of all nodes is zero. You can specify nonzero initial
temperatures. Initial stresses, field variables, etc. can also be defined; Initial Conditions describes all the
initial conditions that are available for a fully coupled thermal-stress analysis.
Boundary Conditions
Boundary conditions can be used to prescribe both temperatures (degree of freedom 11) and
displacements/rotations (degrees of freedom 1–6) at nodes in fully coupled thermal-stress
analysis (see Boundary Conditions). Shell elements
in Abaqus/Standard have additional temperature degrees of freedom 12, 13, etc. through the thickness (see
Conventions).
Boundary conditions can be specified as functions of time by referring to amplitude curves
(Amplitude Curves).
Boundary conditions applied during a dynamic coupled temperature-displacement response step
should use appropriate amplitude references (Amplitude Curves). If boundary
conditions are specified for the step without amplitude references, they are applied
instantaneously at the beginning of the step. Since Abaqus/Explicit does not admit jumps in displacement, the value of a nonzero displacement boundary
condition that is specified without an amplitude reference is ignored, and a zero velocity
boundary condition is enforced.
Loads
The following types of thermal loads can be prescribed in a fully coupled thermal-stress
analysis, as described in Thermal Loads:
Concentrated heat fluxes.
Body fluxes and distributed surface fluxes.
Node-based film and radiation conditions.
Average-temperature radiation conditions.
Element and surface-based film and radiation conditions.
The following types of mechanical loads can be prescribed:
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6);
see Concentrated Loads.
Distributed pressure forces or body forces can be applied; see Distributed Loads. The
distributed load types available with particular elements are described in Abaqus Elements Guide.
Predefined Fields
Predefined temperature fields are not allowed in a fully coupled thermal-stress analysis.
Boundary conditions should be used instead to prescribe temperature degree of freedom 11
(and 12, 13, etc. in Abaqus/Standard shell elements), as described earlier.
Other predefined field variables can be specified in a fully coupled thermal-stress
analysis. These values affect only field-variable-dependent material properties, if any. See
Predefined Fields.
Material Options
The materials in a fully coupled thermal-stress analysis must have both thermal properties,
such as conductivity, and mechanical properties, such as elasticity, defined. See Abaqus Materials Guide for details on the material models
available in Abaqus.
Thermal strain arises if thermal expansion (Thermal Expansion) is included in
the material property definition.
Rate-Dependent Yield and Friction in Abaqus/Standard
In Abaqus/Standard you can control whether to consider or ignore the strain rate–dependence of the yield
stress and the slip rate–dependence of the friction coefficient within the step.
Input File Usage
Use the following option to consider rate dependence within the step:
Abaqus/CAE always considers the strain rate–dependence of the yield stress and the slip
rate–dependence of the friction coefficient.
Internal Heat Generation
In Abaqus/Standard analyses, you can define volumetric heat generation within a material in user
subroutine HETVAL or user subroutine UMATHT. You can use these two user
subroutines in the same analysis.
In Abaqus/Explicit analyses, you can define volumetric heat generation within a material in user
subroutine VHETVAL or user subroutine VUMATHT. You can use these two user
subroutines in the same analysis.
Defining Internal Heat Generation in User Subroutine
HETVAL or
VHETVAL
If you define internal heat generation in user subroutine HETVAL or VHETVAL, you must include heat
generation in the material definition with the other thermal property definitions.
Heat generation might be associated with (relatively low) energy phase changes
occurring during the solution. Such heat generation usually depends on state variables
(such as the fraction transformed), which themselves evolve with the solution and are
stored as solution-dependent state variables (see About User Subroutines and Utilities). The heat
generation is computed in user subroutine HETVAL or VHETVAL, where any associated
state variables can also be updated. The subroutine is called at all material
calculation points for which the material definition includes heat generation.
Property module: material editor: Thermal: Heat Generation
Defining Internal Heat Generation in User Subroutine
UMATHT or
VUMATHT
If user subroutine UMATHT or VUMATHT is used to define internal
heat generation, the constitutive thermal behavior must also be defined within the
subroutine.
Property module: material editor: General: User Material: User material type: Thermal
Inelastic Energy Dissipation as a Heat Source
You can specify an inelastic heat fraction in a fully coupled thermal-stress analysis to
provide for inelastic energy dissipation as a heat source. The heat flux per unit volume, , that is added into the thermal energy balance is computed using the
equation
or, in the case when the nonlinear isotropic/kinematic hardening model is used, from the
following equation:
where is a user-defined factor (assumed constant), is the stress, is the backstress, and is the rate of plastic straining.
Inelastic heat fractions are typically used in the simulation of high-speed manufacturing
processes involving large amounts of inelastic strain, where the heating of the material
caused by its deformation significantly influences temperature-dependent material
properties. The generated heat is treated as a volumetric heat flux source term in the
heat balance equation.
An inelastic heat fraction can be specified for materials with plastic behavior that use
the Mises or Hill yield surface (Inelastic Behavior), and it can
also be used with the combined isotropic/kinematic hardening model. The inelastic heat
fraction can be specified for user-defined material behavior in Abaqus/Explicit and is multiplied by the inelastic energy dissipation coded in the user subroutine to
obtain the heat flux. In Abaqus/Standard the inelastic heat fraction cannot be used with user-defined material behavior; in this
case the heat flux that must be added to the thermal energy balance is computed directly
in the user subroutine.
An inelastic heat fraction can also be specified for material definitions that include
time-domain linear viscoelasticity (Time Domain Viscoelasticity) and time-domain
nonlinear viscoelasticity defined within the parallel rheological framework (Parallel Rheological Framework), except in Abaqus/Explicit for large-strain linear viscoelasticity. For large-strain linear viscoelasticity in Abaqus/Standard (Time Domain Viscoelasticity), the energy
dissipation is computed only approximately. Hence, the fraction of the dissipated energy
converted into heat can be computed only approximately.
The default value of the inelastic heat fraction is 0.9. If you do not include the
inelastic heat fraction behavior in the material definition, the heat generated by
inelastic deformation is not included in the analysis.
Property module: material editor: Thermal: Inelastic Heat Fraction:
Fraction:
Elements
Coupled temperature-displacement elements that have both displacements and temperatures as
nodal variables are available in both Abaqus/Standard and Abaqus/Explicit (see Choosing the Appropriate Element for an Analysis Type). In Abaqus/Standard simultaneous temperature/displacement solution requires the use of such elements; pure
displacement elements can be used in part of the model in the fully coupled thermal-stress
procedure, but pure heat transfer elements cannot be used. In Abaqus/Explicit any of the available elements can be used in the fully coupled thermal-stress procedure;
however, the thermal solution is obtained only at nodes where the temperature degree of
freedom has been activated (that is, at nodes attached to coupled temperature-displacement
elements).
The first-order coupled temperature-displacement elements in Abaqus use a constant temperature over the element to calculate thermal expansion. The
second-order coupled temperature-displacement elements in Abaqus/Standard use a lower-order interpolation for temperature than for displacement (parabolic
variation of displacements and linear variation of temperature) to obtain a compatible
variation of thermal and mechanical strain.