You can apply thermal loads in heat transfer, fully coupled temperature-displacement,
fully coupled thermal-electrical-structural, and coupled thermal-electrical analyses to model
conduction, convection, and radiation.
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.
Input File Usage
CFLUXnode number or node set name, degree of freedom, heat flux magnitude
Abaqus/CAE Usage
Load module: Create Load: choose Thermal for the Category and Concentrated heat flux for the Types for Selected Step: select region: Magnitude: heat flux magnitude
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.
Input File Usage
Use the following option to specify concentrated heat fluxes at a phantom node
originally located coincident with the specified real node:
CFLUX, PHANTOM=NODEnode number, degree of freedom, heat flux magnitude
Use the following option to specify concentrated heat fluxes at a phantom node
located at an element edge:
Specifying concentrated heat fluxes at phantom nodes for enriched elements is not
supported in Abaqus/CAE.
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.
Defining the values of concentrated nodal flux from a user-specified file is not
supported in Abaqus/CAE.
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.
Input File Usage
DFLUXelement number or element set name, load type label, flux magnitude
where load type label is
Sn,
SPOS,
SNEG, or
BF
Abaqus/CAE Usage
Use the following input to define a distributed surface flux:
Load module: Create Load: choose Thermal for the Category and Surface heat flux for the Types for Selected Step: select region: Distribution: select an analytical field, Magnitude: flux magnitude
Use the following input to define a distributed body flux:
Load module: Create Load: choose Thermal for the Category and Body heat flux for the Types for Selected Step: select region: Distribution: Uniform or select an analytical field, Magnitude: flux magnitude
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.
Use the following input to specify surface-based distributed heat fluxes:
Load module: Create Load: choose Thermal for the Category and Surface heat flux for the Types for Selected Step: select region: Distribution: Uniform, Magnitude: 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 user subroutine DFLUX as
FLUX(1) (see DFLUX). If you omit
the magnitude, FLUX(1) is passed in as zero. In Abaqus/Explicit the specified reference magnitude that you must define is the variable
VALUE (see VDFLUX).
Input File Usage
Use the following option to define a nonuniform element-based heat flux:
DFLUXelement number or element set name, load type label
where load type label is
SnNU,
SPOSNU,
SNEGNU, or
BFNU.
Use the following option to define a nonuniform surface-based heat flux:
Use the following input to define a nonuniform element-based body flux:
Load module: Create Load: choose Thermal for the Category and Body heat flux for the Types for Selected Step: select region: Distribution: User-defined, Magnitude: flux magnitude
Use the following input to define a nonuniform surface-based heat flux:
Load module: Create Load: choose Thermal for the Category and Surface heat flux for the Types for Selected Step: select region: Distribution: User-defined, Magnitude: flux magnitude
Nonuniform element-based distributed surface fluxes are not supported in Abaqus/CAE.
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.
Input File Usage
Use the following option to define nonuniform moving concentrated heat
fluxes:
DFLUXelement set name, MBFNU, blank entry, table collection name or leave blank if no table collection is used
Abaqus/CAE Usage
Defining moving or stationary nonuniform heat flux in user subroutine UMDFLUX is not supported in Abaqus/CAE.
Prescribing Boundary Convection
Heat flux on a surface due to convection is governed by
where
is the heat flux across the surface,
is the film coefficient,
is the temperature at this point on the surface, and
is a reference sink temperature value.
You can define heat flux due to convection 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.
Input File Usage
FILMelement number or element set name, film load type label, , h
Abaqus/CAE Usage
Element-based film conditions are supported in Abaqus/CAE only for the film coefficient.
Interaction module: Create Interaction: Surface film condition: select region: Definition: select an analytical field: Film coefficient:h
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
continuum elements that support the temperature degree of freedom. 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.
Figure 1. Partial facets and internal free surface for film cooling.
Input File Usage
FILMelement number or element set name, FFS or FFSNU, , h
Abaqus/CAE Usage
Specifying element-based film conditions on evolving faces of an element is not
supported in Abaqus/CAE.
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.
Interaction module: Create Interaction: Surface film condition: select region: Definition: Embedded Coefficient or User-defined: Film coefficient:h and Sink temperature:
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).
Input File Usage
CFILMnode number or node set name, nodal area, , h
Abaqus/CAE Usage
Interaction module: Create Interaction: Concentrated film condition: select region: Definition: Embedded Coefficient, User-defined, or select an analytical field: Associated nodal area:nodal area, Film coefficient:h, Sink temperature:
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.
Input File Usage
Use the following option to define the film conditions at a phantom node originally
located coincident with the specified real node:
Use the following option to define the film conditions at a phantom node located at
an element edge:
CFILM, PHANTOM=EDGEfirst corner node number, second corner node number, nodal area, , h
Abaqus/CAE Usage
Defining film conditions at phantom nodes for enriched elements is not supported in
Abaqus/CAE.
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.
Input File Usage
For element-based film conditions, use the following options:
FILM PROPERTY, NAME=film property table nameFILMelement number or element set name, film load type label, , film property table name
For surface-based film conditions, use the following options:
FILM PROPERTY, NAME=film property table nameSFILMsurface name, F, , film property table name
For node-based film conditions, use the following options:
FILM PROPERTY, NAME=film property table nameCFILMnode number or node set name, nodal area, , film property table name
The FILM PROPERTY option must appear
in the model definition portion of the input file.
Abaqus/CAE Usage
Interaction module:
Create Interaction Property: Name: film property table name and FilmconditionCreate Interaction: Surface film condition or Concentrated film condition: select region: Definition: Property Reference and Film interaction property: film property table name
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.
Input File Usage
Use the following options to define time-dependent film conditions:
AMPLITUDE, NAME=temp_ampAMPLITUDE, NAME=h_ampFILM, AMPLITUDE=temp_amp, FILM AMPLITUDE=h_ampSFILM, AMPLITUDE=temp_amp, FILM AMPLITUDE=h_ampCFILM, AMPLITUDE=temp_amp, FILM AMPLITUDE=h_amp
Abaqus/CAE Usage
Use the following input to define time-dependent film conditions. If you select an
analytical field to define the interaction, the analytical field affects only the film
coefficient.
Interaction module:
Create Amplitude: Name:h_ampCreate Amplitude: Name:temp_ampCreate Interaction: Surface film condition or Concentrated film condition: select region: Definition: Embedded Coefficient or select an analytical field: Film coefficient amplitude: h_amp and Sink amplitude: temp_amp
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
A nonuniform film coefficient can be defined as a function of position, time,
temperature, etc. in user subroutine FILM in Abaqus/Standard and in user subroutine VFILM in Abaqus/Explicit
for element-based, surface-based, as well as node-based film conditions. If a nonuniform
film is prescribed, AMPLITUDE and
FILM AMPLITUDE references are used only
to modify the sink temperature and film coefficient that are passed into the user
subroutine.
Input File Usage
Use the following option to define a nonuniform film coefficient for an
element-based film condition:
Use the following option to define a nonuniform film coefficient for a node-based
film condition:
CFILM, USERnode number or node set name, nodal area
Abaqus/CAE Usage
Element-based film conditions to define a nonuniform film coefficient are not
supported in Abaqus/CAE. However, similar functionality is available using surface-based film conditions. Use
the following option to define a nonuniform film coefficient for a surface-based film
condition:
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).
Interaction module: Create Interaction: Surface radiation: select region: Radiation type: To ambient, Emissivity distribution: select an analytical field, Emissivity: , and Ambient temperature:
Specifying Element-Based Radiation Conditions on Evolving Faces of an Element in Abaqus/Standard
To specify element-based radiation on three-dimensional continuum elements that support
the temperature degree of freedom, you must provide the ambient temperature value, , and the emissivity of the surface, . 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.
Figure 2. Partial facets and internal free surface for radiation.
Specifying element-based radiation conditions on evolving faces of an element is not
supported in Abaqus/CAE.
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, .
Interaction module: Create Interaction: Surface radiation: select region: Radiation type: To ambient, Emissivity distribution:Uniform, Emissivity: , and Ambient temperature:
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.
Input File Usage
CRADIATEnode number or node set name, nodal area, ,
Abaqus/CAE Usage
Interaction module: Create Interaction: Concentrated radiation to ambient: select region: Associated nodal area:Emissivity: and Ambient temperature:
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.
Input File Usage
Use the following option to specify radiation conditions at a phantom node
originally located coincident with the specified real node:
Specifying radiation conditions at phantom nodes for enriched elements is not
supported in Abaqus/CAE.
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 might need to reduce the increment size. This option can only be used in
three-dimensional analyses.
Input File Usage
Use the following option to define the average-temperature radiation condition on a
surface:
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.