bfe#

FeBodyLoads.bfe(elem='', lab='', stloc='', val1='', val2='', val3='', val4='', **kwargs)#

Defines an element body-force load.

Mechanical APDL Command: BFE

Parameters:
elemstr

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

labstr

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

This command contains some tables and extra information which can be inspected in the original documentation pointed above.

stlocstr

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.

val1str

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 unidirectional Mechanical APDL to Ansys CFX analysis, VAL2 is the volume interface number (not available from within the GUI), and VAL1, VAL3, and VAL4 are not used.

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

For analyses that allow complex input, if Lab = FORC and STLOC = 4, VAL1, VAL2, and VAL3 are the imaginary X, Y, and Z components of force density (in the global Cartesian coordinate system).

val2str

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 unidirectional Mechanical APDL to Ansys CFX analysis, VAL2 is the volume interface number (not available from within the GUI), and VAL1, VAL3, and VAL4 are not used.

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

For analyses that allow complex input, if Lab = FORC and STLOC = 4, VAL1, VAL2, and VAL3 are the imaginary X, Y, and Z components of force density (in the global Cartesian coordinate system).

val3str

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 unidirectional Mechanical APDL to Ansys CFX analysis, VAL2 is the volume interface number (not available from within the GUI), and VAL1, VAL3, and VAL4 are not used.

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

For analyses that allow complex input, if Lab = FORC and STLOC = 4, VAL1, VAL2, and VAL3 are the imaginary X, Y, and Z components of force density (in the global Cartesian coordinate system).

val4str

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 unidirectional Mechanical APDL to Ansys CFX analysis, VAL2 is the volume interface number (not available from within the GUI), and VAL1, VAL3, and VAL4 are not used.

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

For analyses that allow complex input, if Lab = FORC and STLOC = 4, VAL1, VAL2, and VAL3 are the imaginary X, Y, and Z components of force density (in the global Cartesian coordinate system).

Notes

Defines an element body-force load (such as the temperature in a structural analysis or the heat- generation rate in a thermal analysis). 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-force load to an element, the bfe command takes precedence.

Imaginary values for FORC loading via bfe is supported by current-technology solid elements ( PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, and SOLID285 ) and reinforcing elements ( REINF263, REINF264, and REINF265 ). Use only for modal or harmonic analyses. Large-deflection effects must be disabled ( nlgeom,OFF).

The following topics for applying HGEN loading via the bfe command are available:

For 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, specify VAL1 through VAL4 to specify the heat-generation values for the appropriate layers. Heat generation is constant over the layer.

For HGEN loading on reinforcing elements REINF263, REINF264, and REINF265, STLOC refers to the corner locations of the reinforcing members (individual reinforcings):

  • REINF263 and REINF264 : Specify VAL1 and VAL2 for each member. For tables, specify VAL1 only.

  • REINF265 : Specify VAL1, VAL2, VAL3, and VAL4 for each member. For tables, specify VAL1 only.

For FORC loading on reinforcing elements, STLOC refers to real ( STLOC = 1) or imaginary ( STLOC = 4) components.

When using the standard method for defining reinforcing, this is the only way to apply a body load (HGEN or FORC) on the reinforcing members created after generating the REINF nnn reinforcing elements ( ereinf ). If applying FORC loading, Mechanical APDL applies a uniform load to all reinforcing members if there are multiple members in selected elements.

When using the mesh-independent method for defining reinforcing, you can apply a body load on the reinforcing members in the same way. The preferred method, however, is to apply loads on the MESH200 elements (via bfe or bf for HGEN, BFE for FORC) before generating the REINF nnn reinforcing elements ( ereinf ). Mechanical APDL maps the loads from the MESH200 elements to the newly generated REINF nnn reinforcing elements automatically. If you need to apply the loads after generating the reinforcing elements, apply them to MESH200 elements and issue bfport to transfer the loads to the reinforcing members.

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.

For the body-force-density label (FORC), you can specify a table for any of the VAL1 through VAL3 arguments. Both 1D and 2D tables are valid; however, only 1D tables are valid in mode- superposition harmonic and mode-superposition transient analyses.

Enclose the table name ( tabname ) in percent signs (%), for example :

bfe, Elem, Lab, STLOC,``tabname``

Use the dim command to define a table. For information on primary variables for each load type, see Applying Loads Using Tabular Input

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.

In a mode-superposition harmonic or transient analysis, you must apply the load in the modal portion of the analysis. Mechanical APDL calculates a load vector and writes it to the MODE file, which you can apply via the lvscale command.

This command is also valid in PREP7.