Thermal Loads

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.

CFLUX
node number or node set name, degree of freedom, heat flux magnitude 

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 

For an enriched element (see Modeling Discontinuities as an Enriched Feature Using the Extended Finite Element Method), you can apply concentrated heat flux at a phantom node that is originally located coincident with the specified real node.

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.

CFLUX, PHANTOM=NODE
node number, degree of freedom, heat flux magnitude 

CFLUX, PHANTOM=EDGE
first corner node number, second corner node number, heat flux magnitude 

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.

CFLUX, FILE=file, STEP=step, INC=inc

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.

DFLUX
element number or element set name, load type label, flux magnitude

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

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

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.

DSFLUX
surface name, S, flux magnitude

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

Heat fluxes can be added, modified, or removed as described in About Loads.

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.

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).

DFLUX
element number or element set name, load type label

DSFLUX
surface name, SNU

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

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

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.

DFLUX
element set name, MBFNU, blank entry, table collection name or leave blank if no table collection is used

You can define the sink temperature value, ${\theta }^0$ , 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.

FILM
element number or element set name, film load type label, ${\theta }^0$, h

Interaction module: Create Interaction: Surface film condition: select region: Definition: select an analytical field: Film coefficient: h 

You can define the sink temperature value, ${\theta }^0$ , 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.

FILM
element number or element set name, FFS or FFSNU, ${\theta }^0$, h

You can define the sink temperature value, ${\theta }^0$ , 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.

SFILM
surface name, F or FNU, ${\theta }^0$, h

Interaction module: Create Interaction: Surface film condition: select region: Definition: Embedded Coefficient or User-defined: Film coefficient: h and Sink temperature: ${\theta }^0$

A node-based film condition requires that you define the nodal area for a specified node number or node set; the sink temperature value, ${\theta }^0$ ; 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).

CFILM
node number or node set name, nodal area, ${\theta }^0$, h

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: ${\theta }^0$

For an enriched element (see Modeling Discontinuities as an Enriched Feature Using the Extended Finite Element Method), you can define the nodal area; the sink temperature value, ${\theta }^0$ ; and the film coefficient, h, at a phantom node that is originally located coincident with the specified real node.

Alternatively, you can define the nodal area; the sink temperature value, ${\theta }^0$ ; 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.

CFILM, PHANTOM=NODE
node number, nodal area, ${\theta }^0$, h

CFILM, PHANTOM=EDGE
first corner node number, second corner node number, nodal area, ${\theta }^0$, h

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.

FILM PROPERTY, NAME=film property table name 
FILM   
element number or element set name, film load type label, ${\theta }^0$, film property table name

FILM PROPERTY, NAME=film property table name 
SFILM  
surface name, F, ${\theta }^0$, film property table name

FILM PROPERTY, NAME=film property table name  
CFILM
node number or node set name, nodal area, ${\theta }^0$, film property table name

Interaction module: 
Create Interaction Property: Name: film property table name and Film
condition
Create Interaction: Surface film condition or Concentrated film condition: select region: Definition: Property Reference and Film interaction property: film property table name

Film conditions can be added, modified, or removed as described in About Loads.

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, ${\theta }^0$ , 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.

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

Interaction module: 
Create Amplitude: Name: h_amp
Create Amplitude: Name: temp_amp
Create 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

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

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.

FILM
element number or element set name, FnNU

SFILM
surface name, FNU

CFILM, USER
node number or node set name, nodal area

Interaction module: Create Interaction: Surface film condition: select region: Definition: User-defined

Interaction module: Create Interaction: Concentrated film condition: select region: Definition: User-defined

To specify element-based radiation within a heat transfer or coupled temperature-displacement step definition, you must provide the ambient temperature value, ${\theta }^0$ , and the emissivity of the surface, $ϵ$ . 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).

RADIATE
element number or element set name, Rn, ${\theta }^0$, $ϵ$

Interaction module: Create Interaction: Surface radiation: select region: Radiation type: To ambient, Emissivity distribution: select an analytical field, Emissivity: $ϵ$, and Ambient temperature: ${\theta }^0$

To specify element-based radiation on three-dimensional continuum elements that support the temperature degree of freedom, you must provide the ambient temperature value, ${\theta }^0$ , and the emissivity of the surface, $ϵ$ . 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.

RADIATE
element number or element set name, RFS, ${\theta }^0$, $ϵ$

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, ${\theta }^0$ ; and the emissivity of the surface, $ϵ$ .

SRADIATE
surface name, R, ${\theta }^0$, $ϵ$

Interaction module: Create Interaction: Surface radiation: select region: Radiation type: To ambient, Emissivity distribution: Uniform, Emissivity: $ϵ$, and Ambient temperature: ${\theta }^0$

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, ${\theta }^0$ ; and the emissivity of the surface, $ϵ$ . 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.

CRADIATE
node number or node set name, nodal area, ${\theta }^0$, $ϵ$

Interaction module: Create Interaction: Concentrated radiation to ambient: select region: Associated nodal area: Emissivity: $ϵ$ and Ambient temperature: ${\theta }^0$

For an enriched element (see Modeling Discontinuities as an Enriched Feature Using the Extended Finite Element Method), you can define the nodal area; the ambient temperature value, ${\theta }^0$ ; and the emissivity of the surface, $ϵ$ , at a phantom node that is originally located coincident with the specified real node.

Alternatively, you can define the nodal area; the ambient temperature value, ${\theta }^0$ ; and the emissivity of the surface, $ϵ$ , 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.

CRADIATE, PHANTOM=NODE
node number, nodal area, ${\theta }^0$, $ϵ$

CRADIATE, PHANTOM=EDGE
first corner node number, second corner node number, nodal area, ${\theta }^0$, $ϵ$

The user-specified value of the ambient temperature, ${\theta }^0$ , 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 ${\theta }_{AVG}$ 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.

SRADIATE
surface name, AVG, , $ϵ$ 

Interaction module: Create Interaction: Surface radiation: select the surface region: Radiation type: Cavity approximation (3D only), Emissivity: $ϵ$

You can specify the value of absolute zero, ${\theta }^Z$ , on the temperature scale being used; you must specify this value as model data. By default, the value of absolute zero is 0.0.

PHYSICAL CONSTANTS, ABSOLUTE ZERO=${\theta }^Z$

Any module: ModelEdit Attributesmodel_name: Absolute zero temperature: ${\theta }^Z$

If boundary radiation is prescribed, you must specify the Stefan-Boltzmann constant, $\sigma$ ; this value must be specified as model data.

PHYSICAL CONSTANTS, STEFAN BOLTZMANN=$\sigma$

Any module: ModelEdit Attributesmodel_name: Stefan-Boltzmann constant: $\sigma$

Boundary radiation conditions can be added, modified, or removed as described in About Loads.