MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide5/AbaqusAnalysisUserGuide5_016.md

Specifying shear, normal, and transverse edge tractions

The loading directions of shear, normal, and transverse edge tractions are determined by the underlying elements. A positive shear edge traction acts in the positive direction of the shell edge as determined by the element connectivity. A positive normal edge traction acts in the plane of the shell in the inward direction. A positive transverse edge traction acts in a sense opposite to the facet normal. The directions of positive shear, normal, and transverse edge tractions are shown in Figure 34.4.3–6.

To define a shear, normal, or transverse edge traction, you must provide a magnitude, for the load.

If a nonuniform shear, normal, or transverse edge traction is specified, the magnitude, , must be specified in user subroutine UTRACLOAD.

In a geometrically linear step, the shear, normal, and transverse edge tractions act in the tangential, normal, and transverse directions of the shell, as shown in Figure 34.4.3–6. In a geometrically nonlinear analysis the shear, normal, and transverse edge tractions rotate with the shell edge so they always act in the tangential, normal, and transverse directions of the shell, as shown in Figure 34.4.3–6.

Input File Usage: Use one of the following options to define a directed edge traction:

*DLOAD

element number or element set, directed edge traction label, magnitude

*DSLOAD

surface name, directed edge traction label, magnitude

For element-based loads the directed edge traction label can be EDSHRn or EDSHRnNU for shear edge tractions, EDNORn or EDNORnNU for normal edge tractions, or EDTRAn or EDTRAnNU for transverse edge tractions.

For surface-based loads the directed edge traction label can be EDSHR or EDSHRNU for shear edge tractions, EDNOR or EDNORNU for normal edge tractions, or EDTRA or EDTRANU for transverse edge tractions.

Abaqus/CAE Usage: Use the following input to define an element-based directed edge traction:

Load module: Create Load; choose Mechanical for the Category and Shell edge load for the Types for Selected Step; Traction: Normal, Transverse, or Shear; Distribution: select an analytical field

Use the following input to define a surface-based directed edge traction:

Load module: Create Load; choose Mechanical for the Category and Shell edge load for the Types for Selected Step; Traction: Normal, Transverse, or Shear; Distribution: Uniform or User-defined

Nonuniform element-based directed edge traction is not supported in Abaqus/CAE.

Specifying edge moments

An edge moment acts about the shell edge with the positive direction determined by the element connectivity. The directions of positive edge moments are shown in Figure 34.4.3–7.

flowchart

graph TD
    1 --> 2
    2 --> 3
    3 --> 4
    4 --> 1

flowchart

graph TD
    1 --> 2
    2 --> 3
    3 --> 1

Figure 34.4.3–7 Positive edge moments.

To define a distributed edge moment, you must provide a magnitude, , for the load.

If a nonuniform edge moment is specified, the magnitude, , must be specified in user subroutine UTRACLOAD.

An edge moment always acts about the current shell edge in both geometrically linear and nonlinear analyses.

In a geometrically linear step an edge moment acts about the shell edge as shown in Figure 34.4.3–7. In a geometrically nonlinear analysis an edge moment always acts about the shell edge as shown in Figure 34.4.3–7.

Input File Usage: Use one of the following options to define an edge moment:

*DLOAD

element number or element set, EDMOMn or EDMOMnNU, magnitude

*DSLOAD

surface name, EDMOM or EDMOMNU, magnitude

Abaqus/CAE Usage: Use the following input to define an element-based edge moment:

Load module: Create Load: choose Mechanical for the Category

and Shell edge load for the Types for Selected Step: Traction:

Moment, Distribution: select an analytical field

Use the following input to define a surface-based edge moment:

Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction: General, Distribution: Uniform or User-defined

Nonuniform element-based edge moments are not supported in Abaqus/CAE.

Resultant loads due to edge tractions and moments

You can choose to integrate edge tractions and moments over the current or the reference configuration by specifying whether or not a constant resultant should be maintained. In general, the constant resultant method is best suited for cases where the magnitude of the resultant load should not vary with changes in the edge length. However, it is up to you to decide which approach is best for your analysis.

Choosing not to have a constant resultant

If you choose not to have a constant resultant, an edge traction or moment is integrated over the edge in the current configuration, an edge whose length changes during a geometrically nonlinear analysis.

Input File Usage: Use one of the following options:

*DLOAD, CONSTANT RESULTANT=NO *DSLOAD, CONSTANT RESULTANT=NO

Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction is defined per unit deformed area

Maintaining a constant resultant

If you choose to have a constant resultant, an edge traction or moment is integrated over the edge in the reference configuration, whose length is constant.

Input File Usage: Use one of the following options:

*DLOAD, CONSTANT RESULTANT=YES *DSLOAD, CONSTANT RESULTANT=YES

Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction is defined per unit undeformed area

Specifying line loads on beam elements

You can specify line loads on beam elements in the global X-, Y-, or Z-direction. In addition, you can specify line loads on beam elements in the beam local 1- or 2-direction.

Input File Usage: Use the following option to define a force per unit length in the global X-, Y-, or Z-direction on beam elements:

*DLOAD element number or element set, load type label, magnitude

where load type label is PX, PY, PZ, PXNU, PYNU, or PZNU.

Use the following option to define a force per unit length in the beam local 1- or 2-direction:

*DLOAD

element number or element set, load type label, magnitude

where load type label is P1, P2, P1NU, or P2NU.

Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Line load for the Types for Selected Step

Additional references

• Genta, G., Dynamics of Rotating Systems, Springer, 2005.

34.4.4 THERMAL LOADS

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE

References

• “Applying loads: overview,” Section 34.4.1
• *CFLUX
• *DFLUX
• *DSFLUX
• *CFILM
• *FILM
• *SFILM
• *FILM PROPERTY
• *CRADIATE
• *RADIATE
• *SRADIATE
• “Defining a concentrated heat flux,” Section 16.9.19 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Defining a body heat flux,” Section 16.9.18 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Defining a surface heat flux,” Section 16.9.17 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Defining a fluid wall boundary condition,” Section 16.10.12 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Defining a surface film condition interaction,” Section 15.13.22 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Defining a concentrated film condition interaction,” Section 15.13.23 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Defining a surface radiative interaction,” Section 15.13.24 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Defining a concentrated radiative interaction,” Section 15.13.25 of the Abaqus/CAE User’s Guide, in the HTML version of this 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.

See “Applying loads: overview,” Section 34.4.1, for general information that applies to all types of loading.

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 = - h (\theta - \theta^ {0}),

where

q is the heat flux across the surface, h is a reference film coefficient, \theta is the temperature at this point on the surface, and \theta^{0} 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, \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 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, \theta ^ { 0 } , 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 surface-based film conditions

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,” 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, , h

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

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, , 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: \theta ^ { 0 }

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, , film property table name For surface-based film conditions, use the following options: *FILM PROPERTY, NAME=film property table name *SFILM surface name, F, , film property table name 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, , film property table name