Selects the element nodal force type for output.

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


Type of force to be associated with the force items:



Total forces (static, damping, and inertia).



Static forces.



Damping forces.



Inertia forces.

Command Default

Use the total forces.


FORCE selects the element nodal force type for output with the POST1 PRESOL, PLESOL, PRRFOR, NFORCE, FSUM, etc. commands, the POST26 ESOL command, and reaction force plotting [/PBC]. For example, FORCE,STATIC causes item F of the PRESOL command to be the static forces for the elements processed. Element member forces (such as those available for beams and shells and processed by Item and Sequence number) are not affected by this command. The SMISC records extract the static force.

In a non-spectrum analysis that includes either contact or pretension elements in the model, the PRRSOL command is valid with the FORCE command. Otherwise, the PRRSOL command is not valid with FORCE. Use the PRRFOR command, which provides the same functionality as PRRSOL, instead.

Use the FORCE command prior to any load case operations (LCOPER) to insure the correct element nodal force combinations.

In POST26, the ESOL data stored is based on the active FORCE specification at the time the data is stored. To store data at various specifications (for example, static and inertia forces), issue a STORE command before each new specification.

The FORCE command cannot be used to extract static, damping, and inertial forces for MPC184 joint elements.

To retrieve the different force types, use the *GET command with Entity=ELEM and Item1=EFOR.

The FORCE command is not supported in a spectrum analysis. You can specify the force type directly on the combination method commands (ForceType on the PSDCOM, SRSS, CQC, etc. commands).

The FORCE command is not supported in a modal analysis.

Menu Paths

Main Menu>General Postproc>Options for Outp
Main Menu>TimeHist Postpro>Define Variables
Main Menu>TimeHist Postpro>Elec&Mag>Circuit>Define Variables
Utility Menu>List>Results>Options

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