Force load

Use the Force command to define the magnitude and direction of a force load.

You can define the magnitude of a force load as a constant value, an expression, or a field that defines how force load varies with time, frequency or temperature.

Define a force load on geometry or directly on nodes

You can define a force load on selected:

• Geometry (such as, curves, points, mesh points, polygon faces, or polygon edges).

• Nodes

If you define the force load on geometry, the software then maps the force loads to the corresponding nodes.

You can use the Type list in the Force dialog box to specify how you want to define the force load. The geometry or FE entities to which you can apply a force load depend on option you select from the Type list.

Defining a follower force in Nastran analyses

In the Simcenter Nastran and MSC Nastran structural environments, you can use the options in the Direction list in the Force dialog box to use nodes to define the direction in which the force acts. When you define the direction of a force by selecting nodes, the direction of that force can change as the model deforms. This means that the force becomes a follower force. A follower force depends on a structure’s geometry. As a structure deforms, a follower force changes in magnitude and direction.

• If you select Along 2 Nodes (FORCE1), the software uses the two nodes you select to define the vector that the force or moment acts along. With this option, the software creates a FORCE1 bulk data entry in your Nastran input file when you export or solve your model.

• If you select Normal to 4 Nodes (FORCE2), the software uses the four nodes you select nodes to define a plane normal. The force normal to that plane. With this option, the software creates a FORCE2 bulk data entry in your Nastran input file when you export or solve your model.

For more information, see FORCE1 or FORCE2 in the Simcenter Nastran Quick Reference Guide.

Defining a follower force in Abaqus analyses

In the Abaqus environment, you can use the Follower check box in the Follower Force Option group of the Force dialog box to specify that the direction of a concentrated force should rotate with the node to which you apply it. Use this option to include follower force or moment in your analysis.

You should define a follower force for large-displacement analyses and only at nodes with active rotational degrees of freedom, such as the nodes of beam and shell elements or tie nodes on a rigid body for Dynamic Explicit analyses. You should not use it with the reference node of generalized plane strain elements.

When you define a follower force for Dynamic Explicit and Static analyses, you should set the Specify Matrix Storage list to Unsymmetric Matrix in the General tab of the Step Solution dialog box. Eigenvalue analyses ignore the Unsymmetric Matrix option because the solver can only perform an eigenvalue extraction on symmetric matrices.

The Follower check box corresponds to the FOLLOWER parameter for the *CLOAD keyword. For more information, see *CLOAD in the Abaqus Keywords Reference Guide and Concentrated Loads in the Abaqus Analysis Guide.

Defining a force in a Nastran axisymmetric structural solution

If you apply a Force in a Nastran Axisymmetric Structural type solution, the force value you enter in the Force dialog box is treated by Nastran as:

• Force/2π, if you apply the force to the nodes of CTRAX3, CTRAX6, CQUADX4, or CQUADX8 elements.

• Total force around the circumference, if you apply the force to the nodes of CTRIAX6 elements.

The software distributes the force to the nodes according to the distribution strategy you select from the Method list in the Force dialog box but does not apply any additional scaling.

For more information, see CTRAX3, CTRAX6, CQUADX4, and CQUADX8 in the Simcenter Nastran Quick Reference Guide.

Where do I find it?

Application	Pre/Post
Prerequisite	A Simulation file as the work part and displayed part and an active solutionSimcenter Nastran, Abaqus, or ANSYS as the specified solver
Command Finder	Force
Simulation Navigator	Right-click Load Container→New Load→Force

How do I

Define a force or moment load using magnitude and a single direction

Define a force or moment load normal to the model

Define a force or moment load using components

Define a force or moment load on an edge

Define a force or moment using a node ID table

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Force load, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });