34.4.4 Thermal loads
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
References
“Defining a concentrated heat flux,” Section 16.9.19 of the Abaqus/CAE User's Guide
“Defining a body heat flux,” Section 16.9.18 of the Abaqus/CAE User's Guide
“Defining a surface heat flux,” Section 16.9.17 of the Abaqus/CAE User's Guide
“Defining a fluid wall boundary condition,” Section 16.10.12 of the Abaqus/CAE User's Guide
“Defining a surface film condition interaction,” Section 15.13.22 of the Abaqus/CAE User's Guide
“Defining a surface radiative interaction,” Section 15.13.24 of the Abaqus/CAE User's Guide
“Defining a concentrated radiative interaction,” Section 15.13.25 of the Abaqus/CAE User's Guide
Overview
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 “Prescribed conditions: overview,” Section 34.1.1. 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.
Modeling thermal radiation
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,” Section 37.2.1.
Exchange between surfaces that constitute a cavity. This type of radiation is modeled using the cavity radiation capability available in Abaqus/Standard and described in “Cavity radiation,” Section 41.1.1, or through the average-temperature radiation condition described in “Specifying average-temperature radiation conditions,” below.
Prescribing heat fluxes directly
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,” Section 29.6.2.
| Input File Usage: | *CFLUX node 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 |
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.
| Input File Usage: | *CFLUX, FILE=file, STEP=step, INC=inc |
| Abaqus/CAE Usage: | 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 upon 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. Part VI, “Elements,” lists the distributed fluxes that are available for particular elements.
| Input File Usage: | *DFLUX element 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,” Section 2.3.2. You must specify the surface name, the heat flux label, and the heat flux magnitude.
| Input File Usage: | *DSFLUX surface name, S, flux magnitude |
| Abaqus/CAE Usage: | 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 Use the following input to specify surface-based distributed wall heat fluxes in Abaqus/CFD: Load module: Create Boundary Condition: Step: flow_step: choose Fluid for the Category and Fluid wall condition for the Types for Selected Step: select region: Thermal Energy: Specify: Heat flux, Magnitude: flux magnitude |
Modifying or removing heat fluxes
Heat fluxes can be added, modified, or removed as described in “Applying loads: overview,” Section 34.4.1.
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 “Prescribed conditions: overview,” Section 34.1.1, and “Amplitude curves,” Section 34.1.2, 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,” Section 1.1.3 of the Abaqus User Subroutines Reference Guide). 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,” Section 1.2.1 of the Abaqus User Subroutines Reference Guide).
| Input File Usage: | Use the following option to define a nonuniform element-based heat flux: |
*DFLUX element 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: *DSFLUX surface name, SNU |
| Abaqus/CAE Usage: | 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. |
Prescribing boundary convection
Heat flux on a surface due to convection is governed by
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.
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 upon which the film is placed is identified by a film load type label and depends on the element type (see Part VI, “Elements”). 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: | *FILM element number or element set name, film load type label, |
| 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 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,” Section 2.3.2. You must specify the surface name, the film load type, a sink temperature, and a film coefficient.
| Input File Usage: | *SFILM surface name, F or FNU, |
| Abaqus/CAE Usage: | 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,” Section 35.2.1).
| Input File Usage: | *CFILM node number or node set name, nodal area, |
| 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 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 name *FILM element number or element set name, film load type label, For surface-based film conditions, use the following options: *FILM PROPERTY, NAME=film property table name *SFILM surface name, F, For node-based film conditions, use the following options: *FILM PROPERTY, NAME=film property table name *CFILM node number or node set name, nodal area, 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 Film
condition |
Modifying or removing film conditions
Film conditions can be added, modified, or removed as described in “Applying loads: overview,” Section 34.4.1.
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 “Prescribed conditions: overview,” Section 34.1.1, and “Amplitude curves,” Section 34.1.2, for more information.
| Input File Usage: | Use the following options to define time-dependent film conditions: |
*AMPLITUDE, NAME=temp_amp *AMPLITUDE, NAME=h_amp *FILM, AMPLITUDE=temp_amp, FILM AMPLITUDE=h_amp *SFILM, AMPLITUDE=temp_amp, FILM AMPLITUDE=h_amp *CFILM, 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_amp |
Examples
A uniform, time-dependent film condition can be defined for face 2 of element 3 by
*AMPLITUDE, NAME=sink 0.0, 0.5, 1.0, 0.9 *AMPLITUDE, NAME=famp 0.0, 1.0, 1.0, 22.0 … *STEP ** For an Abaqus/Standard analysis: *HEAT TRANSFER ** For an Abaqus/Explicit analysis: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT … *FILM, AMPLITUDE=sink, FILM AMPLITUDE=famp 3, F2, 90.0, 2.0
A uniform, temperature-dependent film coefficient and a time-dependent sink temperature can be defined for face 2 of element 3 by
*AMPLITUDE, NAME=sink 0.0, 0.5, 1.0, 0.9 *FILM PROPERTY, NAME=filmp 2.0, 80.0 2.3, 90.0 8.5, 180.0 … *STEP ** For an Abaqus/Standard analysis: *HEAT TRANSFER ** For an Abaqus/Explicit analysis: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT … *FILM, AMPLITUDE=sink 3, F2, 90.0, filmp
A uniform, temperature-dependent film coefficient and a time-dependent sink temperature can be defined for node 2, where the nodal area is 50, by
*AMPLITUDE, NAME=sink 0.0, 0.5, 1.0, 0.9 *FILM PROPERTY, NAME=filmp 2.0, 80.0 2.3, 90.0 8.5, 180.0 … *STEP ** For an Abaqus/Standard analysis: *HEAT TRANSFER ** For an Abaqus/Explicit analysis: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT … *CFILM, AMPLITUDE=sink, 2, 50, 90.0, filmp
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.
| Input File Usage: | Use the following option to define a nonuniform film coefficient for an element-based film condition: |
*FILM element number or element set name, FnNU Use the following option to define a nonuniform film coefficient for a surface-based film condition: *SFILM surface name, FNU Use the following option to define a nonuniform film coefficient for a node-based film condition: *CFILM, USER node 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: |
Interaction module: Create Interaction: Surface film condition: select region: Definition: User-defined Use the following option to define a nonuniform film coefficient for a node-based film condition: Interaction module: Create Interaction: Concentrated film condition: select region: Definition: User-defined |
Prescribing boundary radiation
Heat flux on a surface due to radiation to the environment is governed by
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 upon which the radiation occurs is identified by a radiation type label depending on the element type (see Part VI, “Elements”).
| Input File Usage: | *RADIATE element number or element set name, Rn, |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Surface radiation: select region: Radiation type: To ambient, Emissivity distribution: select an analytical field, Emissivity: |
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,” Section 2.3.2. You must specify the surface name; the radiation load type label, R (or RPOS, RNEG in the case of shells); the ambient temperature value, ; and the emissivity of the surface, .
| Input File Usage: | *SRADIATE surface name, R, |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Surface radiation: select region: Radiation type: To ambient, Emissivity distribution: Uniform, Emissivity: |
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: | *CRADIATE node number or node set name, nodal area, |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Concentrated radiation to ambient: select region: Associated nodal area: Emissivity: |
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 “Applying loads: overview,” Section 34.4.1, and “Amplitude curves,” Section 34.1.2, for details.
Specifying average-temperature radiation conditions
The average-temperature radiation condition is an approximation to the cavity radiation problem, where the radiative flux per unit area into a facet is
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.
| Input File Usage: | Use the following option to define the average-temperature radiation condition on a surface: |
*SRADIATE surface name, AVG, , |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Surface radiation: select the surface region: Radiation type: Cavity approximation (3D only), Emissivity: |
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.
| Input File Usage: | *PHYSICAL CONSTANTS, ABSOLUTE ZERO= |
| Abaqus/CAE Usage: | Any module: Model |
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.
| Input File Usage: | *PHYSICAL CONSTANTS, STEFAN BOLTZMANN= |
| Abaqus/CAE Usage: | Any module: Model |
Modifying or removing boundary radiation
Boundary radiation conditions can be added, modified, or removed as described in “Applying loads: overview,” Section 34.4.1.