Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
“Defining a concentrated heat flux,” Section 16.9.17 of the ABAQUS/CAE User's Manual
“Defining a body heat flux,” Section 16.9.16 of the ABAQUS/CAE User's Manual
“Defining a surface heat flux,” Section 16.9.15 of the ABAQUS/CAE User's Manual
“Defining a surface convective interaction,” Section 15.12.10 of the ABAQUS/CAE User's Manual
“Defining a concentrated convective interaction,” Section 15.12.11 of the ABAQUS/CAE User's Manual
“Defining a surface radiative interaction,” Section 15.12.12 of the ABAQUS/CAE User's Manual
“Defining a concentrated radiative interaction,” Section 15.12.13 of the ABAQUS/CAE User's Manual
Thermal loads can be applied in heat transfer analysis, in fully coupled temperature-displacement analysis, and in coupled thermal-electrical analysis, as outlined in “Prescribed conditions: overview,” Section 19.1.1. 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.
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 22.2.1.
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 24.1.1.
Concentrated heat fluxes can be prescribed at nodes (or node sets). Distributed heat fluxes can be defined on element faces or surfaces.
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 15.6.2.
| 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 |
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 V, “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 |
| ABAQUS/CAE Usage: | Load module: Create Load: choose Thermal for the Category and Body heat flux for the Types for Selected Step |
| Distributed surface fluxes in ABAQUS/CAE are always specified as surface-based loads (see below). |
When you specify distributed surface fluxes on a surface, the surface that contains the element and face information is defined as described in “Defining element-based surfaces,” 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 or SNU, flux magnitude |
| ABAQUS/CAE Usage: | Load module: Create Load: choose Thermal for the Category and Surface heat flux for the Types for Selected Step |
Heat fluxes can be added, modified, or removed as described in “Applying loads: overview,” Section 19.4.1.
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 19.1.1, and “Amplitude curves,” Section 19.1.2, for details.
In ABAQUS/Standard a nonuniform distributed flux (element-based or surface-based) can be defined in user subroutine DFLUX (see “DFLUX,” Section 25.2.3). The specified reference magnitude will be passed into user subroutine DFLUX as FLUX(1). If the magnitude is omitted, FLUX(1) will be passed in as zero.
| Input File Usage: | Use the following option to define a nonuniform element-based heat flux: |
*DFLUX element number or element set name, SnNU, magnitude Use the following option to define a nonuniform surface-based heat flux: *DSFLUX surface name, SNU, magnitude For example, for general heat transfer shell elements (“Three-dimensional conventional shell element library,” Section 15.6.7) a uniform surface flux of 10.0 per unit area on the top face (SPOS) of shell element 100 can be applied by *DFLUX 100, SPOS, 10.0 When the variation of the (nonuniform) flux magnitude is defined by means of user subroutine DFLUX, the distributed flux type label SPOSNU is used. *DFLUX 100, SPOSNU, magnitude |
| ABAQUS/CAE Usage: | Load module: Create Load: choose Thermal for the Category and Surface heat flux or Body heat flux for the Types for Selected Step: select region: Distribution: User-defined |
Heat flux on a surface due to convection is governed by
is the heat flux across the surface,
is a reference film coefficient,
is the temperature at this point on the surface, and
is a reference sink temperature value.
You can define the sink temperature value, , and the film coefficient, , 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 V, “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 not supported in ABAQUS/CAE. However, similar functionality is available using surface-based film conditions. |
Interaction module: Create Interaction: Surface film condition: select region: Film coefficient: |
You can define the sink temperature value, , and the film coefficient, , on a surface. The surface that contains the element and face information is defined as described in “Defining element-based surfaces,” 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: Film coefficient: |
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, . 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 20.2.1).
| Input File Usage: | *CFILM node number or node set name, nodal area, |
| ABAQUS/CAE Usage: | Interaction module: Create Interaction: Concentrated film condition:
select region: Associated nodal area: Film coefficient: |
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, , 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 |
Film conditions can be added, modified, or removed as described in “Applying loads: overview,” Section 19.4.1.
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, , with time. See “Prescribed conditions: overview,” Section 19.1.1, and “Amplitude curves,” Section 19.1.2, 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: | Interaction module:
Create Amplitude: Name: h_amp |
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
In ABAQUS/Standard a nonuniform film coefficient can be defined as a function of position, time, temperature, etc. in user subroutine FILM (see “FILM,” Section 25.2.6) 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: | User subroutine FILM is not supported in ABAQUS/CAE. |
Heat flux on a surface due to radiation to the environment is governed by
is the heat flux across the surface,
is the radiation 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.
Typically the radiation constant should be defined as
is the emissivity of the surface and
is the Stefan-Boltzmann constant.
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 V, “Elements”).
| Input File Usage: | *RADIATE element number or element set name, Rn, |
| ABAQUS/CAE Usage: | Element-based radiation is not supported in ABAQUS/CAE. However, similar functionality is available using surface-based radiation. |
Interaction module: Create Interaction: Surface radiation to ambient: select region: Emissivity: |
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 “Defining element-based surfaces,” Section 2.3.2. You must specify the surface name; the radiation load type label, R; 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 to ambient: select region: Emissivity: |
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: |
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 |
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 |
Boundary radiation conditions can be added, modified, or removed as described in “Applying loads: overview,” Section 19.4.1.
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 19.4.1, and “Amplitude curves,” Section 19.1.2, for details.
Edit Attributes