SF, Nlist, Lab, VALUE, VALUE2
Specifies surface loads on nodes.

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


Nodes defining the surface upon which the load is to be applied. Use the label ALL or P, or a component name. If ALL, all selected nodes [NSEL] are used (default). If P, graphical picking is enabled and all remaining command fields are ignored (valid only in the GUI).


Valid surface load label. Load labels are listed under "Surface Loads" in the input table for each element type in the Element Reference.

DisciplineSurface Load LabelLabel Description
FREQFrequency (harmonic analyses only)
MXWFEquivalent source surface flag
HFLUX[1]Heat flux
RDSFSurface-to-surface radiation
Acoustic fluid FSI[2]Fluid-structure interaction flag
IMPDImpedance or admittance coefficient
SHLDSurface normal velocity or acceleration
MXWFMaxwell surface flag or equivalent source surface flag
FREEFree surface flag
INFExterior Robin radiation boundary flag
PORTPort number
ATTNAttenuation coefficient
BLIViscous-thermal boundary layer surface flag
RIGWRigid wall flag (Neumann boundary)
MagneticMXWFMaxwell force flag
ElectricCHRGSSurface charge density
MXWFMaxwell force flag
Infinite elementINFExterior surface flag for INFIN110 and INFIN111
Field-surface interfaceFSINField-surface interface number
PoromechanicsFFLXFluid flow flux
DiffusionDFLUXDiffusion flux
  1. Thermal labels CONV and HFLUX are mutually exclusive.

  2. For an acoustic analysis, apply the fluid-structure interaction flag (Label = FSI) to only the FLUID29, FLUID30, FLUID220, and FLUID221 elements.


Surface load value or table name reference for specifying tabular boundary conditions.

If Lab = PRES, VALUE is the real component of the pressure.

If Lab = CONV, VALUE is typically the film coefficient and VALUE2 (below) is typically the bulk temperature. If VALUE = -N, the film coefficient may be a function of temperature and is determined from the HF property table for material N [MP]. (See the SCOPT command for a way to override this option and use -N as the film coefficient.) The temperature used to evaluate the film coefficient is usually the average between the bulk and wall temperatures, but may be user-defined for some elements.

If Lab = RAD, VALUE is surface emissivity.

If Lab = PORT, VALUE is a port number representing a waveguide exterior port. The port number must be an integer between 1 and 50. For acoustic 2×2 transfer admittance matrix, the port number can be any positive integer. The smaller port number corresponds to the port 1 of the 2×2 transfer admittance matrix and the greater number corresponds to the port 2. If one port of the transfer admittance matrix is connecting to the acoustic-structural interaction interface, the port number corresponds to the port 2 of the transfer admittance matrix. A pair of ports of the 2×2 transfer admittance matrix must be defined in the same element. In an acoustic analysis, the positive port number defines a transparent port, through which the reflected sound pressure wave propagates to the infinity; the negative port number defines a vibro port that is the structural vibration surface.

If Lab = SHLD, VALUE is the surface normal velocity in harmonic analysis and the surface normal acceleration in transient analysis.

If Lab = IMPD, VALUE is resistance in (N)(s)/m3 if VALUE > 0 and is conductance in mho if VALUE < 0 for acoustic or harmonic response analyses. In acoustic transient analyses, VALUE2 is not used.

If Lab = RDSF, VALUE is the emissivity value; the following conditions apply: If VALUE is between 0 and 1, apply a single value to the surface. If VALUE= -N, the emissivity may be a function of the temperature, and is determined from the EMISS property table for material N (MP). The material N does not need to correlate with the underlying solid thermal elements.

If Lab = FSIN in a Multi-field solver (single or multiple code coupling) analysis, VALUE is the surface interface number. If Lab = FSIN in a unidirectional ANSYS to CFX analysis, VALUE is not used unless the analysis is performed using the Multi-field solver.

If Lab = ATTN, VALUE is the attenuation coefficient of the surface.


Second surface load value (if any).

If Lab = PRES, VALUE2 is the imaginary component of the pressure. Imaginary pressures can only be used by SURF153, SURF154 and SURF159, and can only be used for a full harmonic analysis (HROPT,FULL), or by a mode-superposition harmonic analysis (HROPT,MSUP) if the mode extraction method is Block Lanczos (MODOPT,LANB), PCG Lanczos (MODOPT,LANPCG), Supernode (MODOPT,SNODE), or Subspace (MODOPT,SUBSP).

If Lab = CONV, VALUE2 is the bulk temperature for thermal analyses. For acoustic analyses, VALUE2 is not used.

If Lab = RAD, VALUE2 is the ambient temperature.

If Lab = SHLD, VALUE2 is the phase angle of the normal surface velocity (defaults to zero) for harmonic response analyses while VALUE2 is not used for transient analyses in acoustics.

If Lab = IMPD, VALUE2 is reactance in (N)(s)/m3 if VALUE > 0 and is the product of susceptance and angular frequency if VALUE < 0 for acoustics.

If Lab = RDSF, VALUE2 is the enclosure number. Radiation will occur between surfaces flagged with the same enclosure numbers. If the enclosure is open, radiation will also occur to ambient. If VALUE2 is negative radiation direction is reversed and will occur inside the element for the flagged radiation surfaces.

If Lab = FSIN in a unidirectional ANSYS to CFX analysis, VALUE2 is the surface interface number (not available from within the GUI).

If Lab = PORT, VALUE2 is not used.


Individual nodes may not be entered for this command. The node list is to identify a surface and the Nlist field must contain a sufficient number of nodes to define an element surface. The loads are internally stored on element faces defined by the specified nodes. All nodes on an element face (including midside nodes, if any) must be specified for the face to be used, and the element must be selected.

If all nodes defining a face are shared by an adjacent face of another selected element, the face is not free and will not have a load applied. If more than one element can share the same nodes (for example, a surface element attached to a solid element), select the desired element type before issuing the SF command. The SF command applies only to area and volume elements.

For shell elements, if the specified nodes include face one (which is usually the bottom face) along with other faces (such as edges), only face one is used. Where faces cannot be uniquely determined from the nodes, or where the face does not fully describe the load application, use the SFE command. A load key of 1 (which is typically the first loading condition on the first face) is used if the face determination is not unique. A uniform load value is applied over the element face.

See the SFBEAM command for applying surface loads to beam elements. See the SFGRAD command for an alternate tapered load capability. See the SFFUN command for applying loads from a node vs. value function. Also see the SFE command for applying tapered loads on individual element faces. Use the SFDELE command to delete loads applied with this command. Use the SFCUM command to accumulate (add) surface loads applied with SF.

Tabular boundary conditions (VALUE = %tabname% and/or VALUE2 = %tabname%) are available for the following surface load labels (Lab) only:  PRES (real and/or imaginary components), CONV (film coefficient and/or bulk temperature) or HFLUX, DFLUX (diffusion flux), RAD (surface emissivity and ambient temperature), IMPD (resistance and reactance), SHLD (normal velocity and phase or acceleration), and ATTN (attenuation coefficient). Use the *DIM command to define a table.

This command is also valid in PREP7 and in the /MAP processor.

Product Restrictions

ANSYS Mechanical Enterprise SF,FSI and SF,FSIN are only available to the ANSYS Mechanical Enterprise family of products (ANSYS Mechanical Enterprise, ANSYS Mechanical Enterprise PrepPost, and ANSYS Mechanical Enterprise Solver).

Menu Paths

Main Menu>Preprocessor>Loads>Define Loads>Apply>Electric>Boundary>AppImped_E>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Electric>Boundary>AppShield>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Electric>Excitation>AppSurfChar>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Electric>Flag>AppInfinite>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Electric>Flag>AppMaxwell>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Field Surface Intr>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Fluid/ANSYS>Field Surface>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Fluid/ANSYS>Impedance>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Magnetic>Flag>AppInfinite>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Magnetic>Other>AppMaxwell>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Structural>Pressure>On Node Components
Main Menu>Preprocessor>Loads>Define Loads>Apply>Structural>Pressure>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Thermal>Convection>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Thermal>Heat Flux>On Nodes
Main Menu>Preprocessor>Loads>Define Loads>Apply>Thermal>Radiation>On Nodes
Main Menu>Solution>Define Loads>Apply>Electric>Boundary>AppImped_E>On Nodes
Main Menu>Solution>Define Loads>Apply>Electric>Boundary>AppShield>On Nodes
Main Menu>Solution>Define Loads>Apply>Electric>Excitation>AppSurfChar>On Nodes
Main Menu>Solution>Define Loads>Apply>Electric>Flag>AppInfinite>On Nodes
Main Menu>Solution>Define Loads>Apply>Electric>Flag>AppMaxwell>On Nodes
Main Menu>Solution>Define Loads>Apply>Field Surface Intr>On Nodes
Main Menu>Solution>Define Loads>Apply>Fluid/ANSYS>Field Surface>On Nodes
Main Menu>Solution>Define Loads>Apply>Fluid/ANSYS>Impedance>On Nodes
Main Menu>Solution>Define Loads>Apply>Magnetic>Flag>AppInfinite>On Nodes
Main Menu>Solution>Define Loads>Apply>Magnetic>Other>AppMaxwell>On Nodes
Main Menu>Solution>Define Loads>Apply>Structural>Pressure>On Node Components
Main Menu>Solution>Define Loads>Apply>Structural>Pressure>On Nodes
Main Menu>Solution>Define Loads>Apply>Thermal>Convection>On Nodes
Main Menu>Solution>Define Loads>Apply>Thermal>Heat Flux>On Nodes
Main Menu>Solution>Define Loads>Apply>Thermal>Radiation>On Nodes
The SF,,ATTN and SF,,RIGW commands cannot be accessed from a menu.

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