A Remote Force is equivalent to a regular force load on a face or a force load on an edge, plus some moment.
A Remote Force can be used as an alternative to building a rigid part and applying a force load to it. The advantage of using a remote force load is that you can directly specify the location in space from which the force originates.

A Remote Force is classified as a remote boundary condition. Refer to the Remote Boundary Conditions section for a listing of all remote boundary conditions and their characteristics.
A Remote Force can be applied to a face, edge, or vertex of a 3D model, or to an edge or vertex of a 2D model.
Remote Force is available for the following analysis types:
This section describes the characteristics of the boundary condition, including the application requirements, support limitations, and loading definitions and values.
Dimensional Types
3D Simulation: Supported.
2D Simulation: Supported (not supported for Explicit Dynamics).
Geometry Types: Geometry types supported for the Remote Force boundary condition include:
Solid: Supported.
Surface/Shell: Supported.
Wire Body/Line Body/Beam: Supported.
Topology: The following topology selection options are supported for Remote Force.
Body: Not Supported.
Face: Supported 3D Only.
Edge: Supported.
Vertex: Supported.
Cannot be applied to a vertex scoped to an end release.
Vertex selections do not support the Behavior option.
Nodes: Supported.
Loading Types: The boundary condition’s loading is defined using one of the following options.
: Supported. While loads are associative with geometry changes, load directions are not. This applies to any load that requires a vector input.
The vector load definition displays in the Annotation legend with the label Components. The Magnitude and Direction entries, in any combination or sequence, define these displayed values. These are the values sent to the solver.
. Supported for Harmonic Response Analysis only.
: Supported.
. Supported for Harmonic Response Analysis only.
Loading Data Definition : Enter loading data using one of the following options.
Constant: Supported.
Tabular (Time Varying): Supported.
Tabular (Step Varying): Supported for Static Structural analysis only.
Tabular (Frequency Varying): Supported for Harmonic Response Analysis only.
By default, at least two frequency entries are required when defining a frequency dependent tabular load.
Tabular (Spatially Varying): Not Supported.
Function (Time Varying): Supported.
Function (Spatially Varying): Not Supported.
You apply a Remote Force as you would apply a force load except that the location of the load origin can be replaced anywhere in space either by picking or by entering the XYZ locations directly or by scoping a geometric entity using the Location property. Note that when you first define the properties of the Remote Force, the application automatically sets the default location of the Location property at the centroid of the scoped geometry selection(s). This setting is maintained even if you re-specify your geometry scoping. It is necessary to manually change the Location property's definition.
The location and the direction of a remote force can be defined in the global coordinate system or in a local coordinate system.
To apply a Remote Force:
On the Environment context toolbar: click Loads>. Or, right-click the Environment tree object or the Geometry window and select Insert>.
Define the Scoping Method.
Select geometric entities on your model.
Specify a coordinate system as needed. The default selection is the Global Coordinate System. You can also specify a user-defined or local coordinate system.
Select the method used to define the remote force: (default), , , or .
Define the Magnitude, Coordinate System directional loading, and/or Direction of the load based on the above selections.
For Harmonic analyses, specify a Phase Angle as needed.
Select the Behavior of the geometry.
As needed, enter a Pinball Region value. The default value is .
The selections available in the Details view are described below.
| Category | Fields/Options/Description |
|---|---|
| Scope |
Scoping Method, options include:
Coordinate System: Drop-down list of available coordinate systems. is the default. The following properties are used to define the location of the load’s origin:
Location: This property specifies the location of the load's origin. The default location is the centroid of your geometry selection(s). You can define this property manually using geometry entity selections as well as by making entries in the above coordinate properties. |
| Definition |
Type: Read-only field that displays boundary condition type - Remote Force. Define By, options include:
Note: Selection of a Coordinate System rotated out of the global Cartesian X-Y plane is not supported in a 2D analysis. Suppressed: Include ( - default) or exclude () the boundary condition. Behavior : This option dictates the behavior of the attached geometry. If the Scope Method property is set to , the boundary condition will then assume the Behavior defined in the referenced Remote Point as well as other related properties. Options include:
Material: This property is available when the Behavior property is set to . Select a material to define material properties for the beams used in the connection. Density is excluded from the material definition. Radius: This property is available when the Behavior property is set to . Specify a radius to define the cross section dimension of the circular beam used for the connection. Follower Load (Rigid Dynamics analysis only): When set to (default), the force direction doesn't change during the simulation. When set to , the force direction is updated with the underlying body. |
| Advanced |
Pinball Region: Modify the Pinball setting to reduce the
number of elements included in the solver. Note: The Pinball Region property is not supported for the Samcef and ABAQUS solvers. |