17.6.5.2. Nodal Force

Using a Nodal Force, you can apply a force to an individual node or a set of nodes. You must create a node-based Named Selection before you can apply a Nodal Force. The Nodal Force that you apply in Mechanical is represented as an F Command in the Mechanical APDL application.

Note:  A Nodal Force object may be added during Solution Restart without losing the restart points.

This page includes the following sections:

Analysis Types

Nodal Force is available for the following analysis types:
Dimensional Types

The supported dimensional types for the Nodal Force boundary condition include:

  • 3D Simulation

  • 2D Simulation

Geometry Types

The supported geometry types for the Nodal Force boundary condition include:

  • Solid

  • Surface/Shell

  • Wire Body/Line Body/Beam

Topology Selection Options

The Nodal Force boundary condition is scoped via node-based Named Selections only. For more information, see the Specifying Named Selections by Direct Node Selection Help section.

Note:  The Nodal Force boundary condition supports spatially varying loading on the scoped nodes for Static and Transient analyses only. For Harmonic Response and Eigenvalue Buckling analyses, only constant loading conditions are supported.

Applying a Nodal Force Boundary Condition

To apply a Nodal Force:

  1. On the Environment Context tab, click Direct FE > Nodal Force. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert>Nodal Force.

  2. Click the Named Selection drop-down list and then select the node-based Named Section to prescribe the scope of the Nodal Force.

  3. Enter a magnitude for the X, Y, and Z component to define the load.

Tip:  Define a Nodal Orientation for the Named Selection to control the Nodal Coordinate System.

Details Pane Properties

The Details pane selections are described below.

CategoryProperty/Options/Description
Scope

Scoping Method: A read-only field that displays scoping method - Named Selection.

Named Selection: A drop-down list of available node-based Named Selection.

Definition

Type: A read-only field that describes the node-based object - Force.

Coordinate System: A read-only field that displays the coordinate system - Nodal Coordinate System. The Nodal Coordinate System can be modified by applying Nodal Orientation objects.

X Component: Defines force in the X direction

Y Component: Defines force in the Y direction

Z Component: Defines force in the Z direction

You can define the Component values as a Constant, in Tabular form as a function of varying Time or varying Step (Static Structural only), or as a Function.

Divide Load by Nodes: Property options include Yes (default) and No. When set to Yes, the load value is normalized by dividing the Magnitude by number of scoped nodes. When set to No, the load value is applied directly to every scoped node.

Non-Cyclic Loading Type: This property is available for Full Harmonic Analysis when Cyclic Symmetry is present in the model. Options include:

  • No (default). The loading is purely cyclic. That is, the load applied to the base sector is applied to each and every sector.

  • Harmonic Index. The non-cyclic loading can be specified for one or more harmonic indices. This is also known as "engine-order loading" (or traveling wave excitation). A Harmonic Index entry is required.

  • Sector Number: This property enables you to select the desired Sector onto which you apply the non-cyclic load.

Harmonic Index: This property displays when the Non-Cyclic Loading Type property is set to Harmonic Index. Where NS is Number of Sectors, enter a value from:

1 to NS/2; if NS is even.
1 to (NS-1)/2; if NS is odd.

Sector Number: This property displays when the Non-Cyclic Loading Type property is set to Sector Number. You use this property to specify the desired sector onto which you want to apply the non-cyclic load.

Suppressed: includes or excludes the boundary condition in the analysis.

Load Vector Controls (Substructure Generation Analysis Only)

Load Vector Assignment: Options include Program Controlled (default) and Manual. When set to Manual, the Load Vector Number property displays.

Load Vector Number: Specify a Load Vector Number using any value greater than 1. A setting of 1 is reserved for a pre-stress Substructure Generation analysis. If multiple loads have the same Load Vector Number, the application groups these loads during the solution process to generate a single load vector that is the combined effect of all grouped loads.

Note:

  • If you have a Nodal Force and a Pressure, and/or Force, and/or Hydrostatic Pressure load that are 1) all are set to the Direct option and 2) share the same scoping, they will create a resultant loading effect.

  • When Divide Load by Nodes is set to Yes, the forces are evenly distributed across the nodes and do not result in a constant traction.

  • Two Nodal Force objects that have the same scoping do not produce a cumulative loading effect. The Nodal Force that was specified last takes priority and is applied, and as a result, the other Nodal Force is ignored. For Explicit Dynamics analyses, a resultant effect is always calculated if multiple loads are applied to a node (either by geometric entity or as a nodal force).

  • A load applied to a geometric entity and a Nodal Force produce a resultant effect.

API Reference

For specific scripting information, see the Nodal Force section of the ACT API Reference Guide.