BFE, Elem, Lab, STLOC, VAL1, VAL2, VAL3, VAL4
Defines an element body force load.

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | –


The element to which body load applies. If ALL, apply to all selected elements (ESEL). A component name may also be substituted for Elem.


Valid body load label. Valid labels are also listed for each element type in the Element Reference under "Body Loads" in the input table.

DisciplineBody Load LabelLabel Description
FREQFrequency (harmonic analyses only)
FORCBody force density in momentum equation
ThermalHGENHeat generation rate (updated by volume changes when large-deflection effects are included [NLGEOM,ON])
MagneticEFElectric field
JSCurrent density
MVDIMagnetic virtual displacements flag
CHRGDCharge density
Field volume interfaceFVINField volume interface flag
PoromechanicsFSOUFluid flow source
Diffusion TEMPTemperature
DGENDiffusing substance generation rate

Starting location for entering VAL data, below. For example, if STLOC = 1, data input in the VAL1 field applies to the first element body load item available for the element type, VAL2 applies to the second element item, etc. If STLOC = 5, data input in the VAL1 field applies to the fifth element item, etc. Defaults to 1.


For Lab = TEMP, FLUE, DGEN, HGEN, and CHRGD, VAL1--VAL4 represent body load values at the starting location and subsequent locations (usually nodes) in the element. VAL1 can also represent a table name for use with tabular boundary conditions. Enter only VAL1 for a uniform body load across the element. For nonuniform loads, the values must be input in the same order as shown in the input table for the element type. Values initially default to the BFUNIF value (except for CHRGD which defaults to zero). For subsequent specifications, a blank leaves a previously specified value unchanged; if the value was not previously specified, the default value as described in the Element Reference is used.

For Lab = JS and STLOC = 1, VAL1, VAL2 and VAL3 are the X, Y, and Z components of current density (in the element coordinate system), and VAL4 is the phase angle.

For Lab = EF and STLOC = 1, VAL1, VAL2, and VAL3 are the X, Y, and Z components of electric field (in the global Cartesian coordinate system).

If Lab = FVIN in a Multi-field solver (single or multiple code coupling) analysis, VAL1 is the volume interface number. If Lab = FVIN in a unidirectional ANSYS to CFX analysis, VAL2 is the volume interface number (not available from within the GUI) and VAL1 is not used unless the ANSYS analysis is performed using the Multi-field solver. VAL3 and VAL4 are not used.

For Lab = FORC and STLOC = 1, VAL1, VAL2, and VAL3 are the X, Y, and Z components of force density (in the global Cartesian coordinate system).


Defines an element body force load (such as temperature in a structural analysis, heat generation rate in a thermal analysis, etc.). Body loads and element specific defaults are described for each element type in the Element Reference. If both the BF and BFE commands are used to apply a body load to an element, the BFE command takes precedence.

For heat-generation (HGEN) loading on layered thermal solid elements SOLID278 / SOLID279 (KEYOPT(3) = 1 or 2), or layered thermal shell elements SHELL131 / SHELL132 (KEYOPT(3) = 1), STLOC refers to the layer number (not the node). In such cases, use VAL1 through VAL4 to specify the heat-generation values for the appropriate layers. Heat generation is constant over the layer.

Specifying a Table

You can specify a table name (VAL1) when using temperature (TEMP), diffusing substance generation rate (DGEN), heat generation rate (HGEN), and current density (JS) body load labels.

Enclose the table name (tabname) in percent signs (%), as shown:

BFE,Elem, Lab,STLOC,%tabname%

Use the *DIM command to define a table.

For Lab = TEMP, each table defines NTEMP temperatures, as follows:

  • For layered elements, NTEMP is the number of layer interface corners that allow temperature input.

  • For non-layered elements, NTEMP is the number of corner nodes.

The temperatures apply to element items with a starting location of STLOC + n, where n is the value field location (VALn) of the table name input.

For layered elements, a single BFE command returns temperatures for one layer interface. Multiple BFE commands are necessary for defining all layered temperatures.

For beam, pipe and elbow elements that allow multiple temperature inputs per node, define the tabular load for the first node only (Node I), as loads on the remaining nodes are applied automatically. For example, to specify a tabular temperature load on a PIPE288 element with the through-wall-gradient option (KEYOPT(1) = 0), the BFE command looks like this:

BFE,Elem,TEMP,1,%tabOut%, %tabIn%

where %tabOut% and %tabIn% and are the tables applied to the outer and inner surfaces of the pipe wall, respectively.

When a tabular function load is applied to an element, the load does not vary according to the positioning of the element in space.

Graphical picking is available only via the listed menu paths.

This command is also valid in PREP7.

Menu Paths

Main Menu>Preprocessor>Loads>Define Loads>Apply>Electric>Boundary>Temperature>On Elements
Main Menu>Preprocessor>Loads>Define Loads>Apply>Electric>Excitation>AppCharDens>On Elements
Main Menu>Preprocessor>Loads>Define Loads>Apply>Field Volume Intr>On Elements
Main Menu>Preprocessor>Loads>Define Loads>Apply>Fluid/ANSYS>Heat Generat>On Elements
Main Menu>Preprocessor>Loads>Define Loads>Apply>Fluid/ANSYS>Normal Velo>On Elements
Main Menu>Preprocessor>Loads>Define Loads>Apply>Magnetic>Boundary>Temperature>On Elements
Main Menu>Preprocessor>Loads>Define Loads>Apply>Magnetic>Excitation>AppCurrDens>On Elements
Main Menu>Preprocessor>Loads>Define Loads>Apply>Magnetic>Other>Electric Field>On Elements
Main Menu>Preprocessor>Loads>Define Loads>Apply>Structural>Other>Fluence>On Elements
Main Menu>Preprocessor>Loads>Define Loads>Apply>Thermal>Heat Generat>On Elements
Main Menu>Solution>Define Loads>Apply>Electric>Boundary>Temperature>On Elements
Main Menu>Solution>Define Loads>Apply>Electric>Excitation>AppCharDens>On Elements
Main Menu>Solution>Define Loads>Apply>Field Volume Intr>On Elements
Main Menu>Solution>Define Loads>Apply>Fluid/ANSYS>Heat Generat>On Elements
Main Menu>Solution>Define Loads>Apply>Fluid/ANSYS>Normal Velo>On Elements
Main Menu>Solution>Define Loads>Apply>Magnetic>Boundary>Temperature>On Elements
Main Menu>Solution>Define Loads>Apply>Magnetic>Excitation>AppCurrDens>On Elements
Main Menu>Solution>Define Loads>Apply>Magnetic>Other>Electric Field>On Elements
Main Menu>Solution>Define Loads>Apply>Structural>Other>Fluence>On Elements
Main Menu>Solution>Define Loads>Apply>Thermal>Heat Generat>On Elements

Release 18.2 - © ANSYS, Inc. All rights reserved.