Thermal loads can be applied in heat transfer analysis, in fully coupled
temperature-displacement analysis, fully coupled thermal-electrical-structural
analysis, and in coupled thermal-electrical analysis, as outlined in
About Prescribed Conditions.
The following types of thermal loads are available:
Concentrated heat flux prescribed at nodes.
Distributed heat flux prescribed on element faces or surfaces.
Body heat flux per unit volume.
Boundary convection defined at nodes, on element faces, or on
surfaces.
Boundary radiation defined at nodes, on element faces, or on surfaces.
Moving or stationary concentrated heat fluxes defined in user
subroutine
UMDFLUX.
See
About Loads
for general information that applies to all types of loading.
The following types of radiation heat exchange can be modeled using
Abaqus:
Exchange between a nonconcave surface and a nonreflecting environment.
This type of radiation is modeled using boundary radiation loads defined at
nodes, on element faces, or on surfaces, as described below.
Exchange between two surfaces within close proximity of each other in
which temperature gradients along the surfaces are not large. This type of
radiation is modeled using the gap radiation capability described in
Thermal Contact Properties.
Concentrated heat fluxes can be prescribed at nodes (or node sets).
Distributed heat fluxes can be defined on element faces or surfaces.
Specifying Concentrated Heat Fluxes
By default, a concentrated heat flux is applied to degree of freedom 11. For
shell heat transfer elements concentrated heat fluxes can be prescribed through
the thickness of the shell by specifying degree of freedom 11, 12, 13, etc.
Temperature variation through the thickness of shell elements is described in
Choosing a Shell Element.
Specifying Concentrated Heat Fluxes at Phantom Nodes for Enriched Elements
Alternatively, you can apply concentrated heat flux at a phantom node located at an
element edge between two specified real corner nodes. This setting applies only to nodes
with both pore pressure and temperature degrees of freedom.
Defining the Values of Concentrated Nodal Flux from a User-Specified File
You can define nodal flux using nodal flux output from a particular step and
increment in the output database (.odb) file of a previous
Abaqus
analysis. The part (.prt) file from the original analysis
is also required when reading data from the output database file. In this case
both the previous model and the current model must be defined consistently,
including node numbering, which must be the same in both models. If the models
are defined in terms of an assembly of part instances, part instance naming
must be the same.
Specifying Element-Based Distributed Heat Fluxes
You can specify element-based distributed surface fluxes (on element faces) or body fluxes (flux
per unit volume). For surface fluxes you must identify the face of the element on which
the flux is prescribed in the flux label (for example,
Sn or
SnNU for continuum
elements). The distributed flux types available depend on the element type. About the Element Library lists the
distributed fluxes that are available for particular elements.
Specifying Surface-Based Distributed Heat Fluxes
When you specify distributed surface fluxes on a surface, the surface that
contains the element and face information is defined as described in
Element-Based Surface Definition.
You must specify the surface name, the heat flux label, and the heat flux
magnitude.
Modifying or Removing Heat Fluxes
Heat fluxes can be added, modified, or removed as described in
About Loads.
Specifying Time-Dependent Heat Fluxes
The magnitude of a concentrated or a distributed heat flux can be controlled
by referring to an amplitude curve. If different magnitude variations are
needed for different fluxes, the flux definitions can be repeated, with each
referring to its own amplitude curve. See
About Prescribed Conditions
and
Amplitude Curves
for details.
Defining Nonuniform Distributed Heat Flux in a User Subroutine
A nonuniform element-based or surface-based distributed flux can be defined
in
Abaqus/Standard
and
Abaqus/Explicit
by using user subroutines
DFLUX and
VDFLUX, respectively. In
Abaqus/Standard
the specified reference magnitude is passed into the user subroutine
DFLUX as FLUX(1) (see
DFLUX).
If the magnitude is omitted, FLUX(1) is passed
in as zero. In
Abaqus/Explicit
the specified reference magnitude to be defined by the user is the variable
VALUE (see
VDFLUX).
Defining Moving or Stationary Nonuniform Heat Flux in User Subroutine UMDFLUX
Multiple nonuniform concentrated heat fluxes can be defined in user
subroutine
UMDFLUX in
Abaqus/Standard.
These heat fluxes can be stationary or moving between start points and end
points inside the element.
Prescribing Boundary Convection
Heat flux on a surface due to convection is governed by
where
q
is the heat flux across the surface,
h
is a reference film coefficient,
is the temperature at this point on the surface, and
is a reference sink temperature value.
Heat flux due to convection can be defined on element faces, on surfaces, or
at nodes.
Specifying Element-Based Film Conditions
You can define the sink temperature value, , and the film coefficient, h, on element faces. The
convection is applied to element edges in two dimensions and to element faces in three
dimensions. The edge or face of the element on which the film is placed is identified by a
film load type label and depends on the element type (see About the Element Library). You must
specify the element number or element set name, the film load type label, a sink
temperature, and a film coefficient.
Specifying Element-Based Film Conditions on Evolving Faces of an Element in Abaqus/Standard
You can define the sink temperature value, , and the film coefficient, h, on three-dimensional
heat transfer elements. The convection is applied to element faces in three dimensions.
The face of the element on which the film is to be placed is identified automatically at
the start of an increment. When elements are added or removed using model change during an
analysis or using element activation or element deletion during an increment of a step,
the film convection is applied automatically at the start of an increment on the new
exposed faces and removed from the unexposed faces. You must specify the element number or
element set name, the film load type label, a sink temperature, and a film coefficient.
By default, convection is applied on the exposed full element facet area.
When you use partial element activation (see
Progressive Element Activation),
you can use user subroutine
UEPACTIVATIONFACET to modify the exposed area over which convection is
applied. For example,
Figure 1
displays the area fractions of the partially filled facets C-I1-I4, C-B-I2-I1,
and B-I3-I2 when partial activation is used. Partial element activation exposes
an internal cut surface area represented as I1-I2-I3-I4. You can use user
subroutine
UEPACTIVATIONFACET to specify the convection area on this cut surface. In
addition, you can use user subroutine
FILM to specify different film coefficients for the internal
cut surface versus the element facets.
Specifying Surface-Based Film Conditions
You can define the sink temperature value, ,
and the film coefficient, h, on a surface. The surface
that contains the element and face information is defined as described in
Element-Based Surface Definition.
You must specify the surface name, the film load type, a sink temperature, and
a film coefficient.
Specifying Node-Based Film Conditions
A node-based film condition requires that you define the nodal area for a
specified node number or node set; the sink temperature value,
;
and the film coefficient, h. The associated degree of
freedom is 11. For shell type elements where the film is associated with a
degree of freedom other than 11, you can specify the concentrated film for a
duplicate node that is constrained to the appropriate degree of freedom of the
shell node by using an equation constraint (see
Linear Constraint Equations).
Specifying Node-Based Film Conditions at Phantom Nodes for Enriched Elements
Alternatively, you can define the nodal area; the sink temperature value, ; and the film coefficient, h, at a phantom node
located at an element edge between two specified real corner nodes. This setting applies
only to nodes with both pore pressure and temperature degrees of freedom.
Specifying Temperature- and Field-Variable-Dependent Film Conditions
If the film coefficient is a function of temperature, you can specify the
film property data separately and specify the name of the property table
instead of the film coefficient in the film condition definition.
You can specify multiple film property tables to define different variations
of the film coefficient, h, as a function of surface
temperature and/or field variables. Each film property table must be named.
This name is referred to by the film condition definitions.
A new film property table can be defined in a restart step. If a film
property table with an existing name is encountered, the second definition is
ignored.
Modifying or Removing Film Conditions
Film conditions can be added, modified, or removed as described in
About Loads.
Specifying Time-Dependent Film Conditions
For a uniform film both the sink temperature and the film coefficient can be
varied with time by referring to amplitude definitions. One amplitude curve
defines the variation of the sink temperature, ,
with time. Another amplitude curve defines the variation of the film
coefficient, h, with time. See
About Prescribed Conditions
and
Amplitude Curves
for more information.
Examples
A uniform, time-dependent film condition can be defined for face 2 of
element 3 by
Defining Nonuniform Film Conditions in a User Subroutine
In
Abaqus/Standard
a nonuniform film coefficient can be defined as a function of position, time,
temperature, etc. in user subroutine
FILM for element-based, surface-based, as well as node-based
film conditions. Amplitude references are ignored if a nonuniform film is
prescribed.
Prescribing Boundary Radiation
Heat flux on a surface due to radiation to the environment is governed by
where
q
is the heat flux across the surface,
is the emissivity of the surface,
is the Stefan-Boltzmann constant,
is the temperature at this point on the surface,
is an ambient temperature value, and
is the value of absolute zero on the temperature scale being used.
Heat flux due to radiation can be defined on element faces, on surfaces, or
at nodes.
Specifying Element-Based Radiation
To specify element-based radiation within a heat transfer or coupled temperature-displacement
step definition, you must provide the ambient temperature value, , and the emissivity of the surface, . The radiation is applied to element edges in two dimensions and to
element faces in three dimensions. The edge or face of the element on which the radiation
occurs is identified by a radiation type label depending on the element type (see About the Element Library).
Specifying Element-Based Radiation Conditions on Evolving Faces of an Element in Abaqus/Standard
To specify element-based radiation within a heat transfer or coupled temperature-displacement
step definition, you must provide the ambient temperature value, , and the emissivity of the surface, for heat transfer elements in 3D. The radiation is applied to element
faces in three dimensions. The face of the element on which the radiation is to be placed
is automatically identified at the start of an increment. When elements are added or
removed using model change during an analysis or using element activation or element
deletion during an increment of a step, the radiation boundary condition is automatically
applied at the start of an increment on the new exposed faces and removed from the
nonexposed faces. You must specify the element number or elset name and the radiation load
type label. (see About the Element Library).
By default, radiation is applied on the exposed full element facet area.
When you use partial element activation (see
Progressive Element Activation),
you can use user subroutine
UEPACTIVATIONFACET to modify the exposed area over which radiation is
specified. When elements are partially activated, you can apply radiation on
the activated facet areas C-I1-I4, C-B-I2-I1, and B-I3-I2 by specifying the
area fraction per element facet. On the internal cut area I1-I2-I3-I4 of the
element as shown in
Figure 2,
you can use user subroutine
UEPACTIVATIONFACET to specify the exposed internal surface area. Radiation is
applied on the prescribed internal cut surface area.
Specifying Surface-Based Radiation to Ambient
You can apply the radiation to a surface rather than to individual element
faces. The surface that contains the element and face information is defined as
described in
Element-Based Surface Definition.
You must specify the surface name; the radiation load type label, R; the ambient temperature value, ;
and the emissivity of the surface, .
Specifying Node-Based Radiation to Ambient
To specify node-based radiation within a heat transfer or coupled
temperature-displacement step definition, you must provide the nodal area for a
specified node number or node set; the ambient temperature value,
;
and the emissivity of the surface, .
The associated degree of freedom is 11. For shell elements where the
concentrated radiation is associated with a degree of freedom other than 11,
you can specify the required data for a duplicate node that is constrained to
the appropriate degree of freedom of the shell node by using an equation
constraint.
Specifying Node-Based Radiation to Ambient at Phantom Nodes for Enriched Elements
Alternatively, you can define the nodal area; the ambient temperature value, ; and the emissivity of the surface, , at a phantom node located at an element edge between two specified real
corner nodes. This setting applies only to nodes with both pore pressure and temperature
degrees of freedom.
Specifying Time-Dependent Radiation
The user-specified value of the ambient temperature,
,
can be varied throughout the step by referring to an amplitude definition. See
About Loads
and
Amplitude Curves
for details.
The average-temperature radiation condition is an approximation to the
cavity radiation problem, where the radiative flux per unit area into a facet
is
with the average temperature for the surface
being calculated as
The average temperature in the cavity is computed at the beginning of each
increment and held constant over the increment. Therefore, the
average-temperature radiation condition has some dependency on the increment
size, and you need to ensure that the increment size you use is appropriate for
your model. If you see large changes in temperature over an increment, you may
need to reduce the increment size. This option can only be used in
three-dimensional analyses.
Specifying the Value of Absolute Zero
You can specify the value of absolute zero, ,
on the temperature scale being used; you must specify this value as model data.
By default, the value of absolute zero is 0.0.
Specifying the Value of the Stefan-Boltzmann Constant
If boundary radiation is prescribed, you must specify the Stefan-Boltzmann
constant, ;
this value must be specified as model data.
Modifying or Removing Boundary Radiation
Boundary radiation conditions can be added, modified, or removed as
described in
About Loads.