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.


Analysis Types

Nodal Force is available for the following analysis types:

Common Characteristics

The following section outlines the common boundary condition characteristics that include application requirements of the boundary condition, support limitations, as well as loading definitions and values.

Dimensional Types

Geometry Types: Geometry types supported for the Nodal Force boundary condition include:

Topology: The Nodal Force boundary condition is scoped via node-based Named Selections only. See the Specifying Named Selections by Direct Node Selection Help section for more information.


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.


Boundary Condition Application

To apply a Nodal Force:

  1. On the Environment toolbar, click Direct FE > Nodal Force. Or, right-click the Environment tree object or 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 View Properties

The Details View selections are described below.

CategoryFields/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: options include:

  • Yes: (default) the load value is normalized: it is divided by number of scoped nodes before application.

  • No: the load value applied directly to every scoped node.

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


Note:
  • 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 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.



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