Force is specified based on the following topologies:
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. Force loads are not supported for 2D axisymmetric Explicit Dynamics analyses.
Geometry Types: Geometry types supported for the Force boundary condition include:
Solid: Supported.
Surface/Shell: Supported.
Wire Body/Line Body/Beam: Supported
Topology: The following topology selection options are supported for Force.
Body: Not Supported.
Face: Supported.
The force is applied by converting it to a pressure, based on the total area of all the selected faces.
If a face enlarges due to a change in CAD parameters, the total load magnitude applied to the face remains constant.
Edge: Supported.
If you select multiple edges when defining the force, the magnitude of the force is distributed evenly across all selected edges.
If an edge enlarges due to a change in CAD parameters, the total load magnitude applied to the edge remains constant.
Vertex: Supported.
If you select multiple vertices when defining the force, the magnitude of the force is distributed evenly across all selected vertices.
A force applied to a vertex is not realistic and leads to singular stresses (that is, stresses that approach infinity near the loaded vertex). You should disregard stress and elastic strain values in the vicinity of the loaded vertex.
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, such as a force.
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. Define direct loading without Phase Angle.
: Supported.
: Supported for Harmonic Response analysis only. Define direct loading without Phase Angle.
Loading Data Definition : Enter loading data using one of the following options.
Constant: Supported.
Tabular (Time Varying): Not supported for Harmonic Response Analysis.
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. The Force boundary condition in a Harmonic Response (Full, linked MSUP, or standalone) can be defined in such a way that it is fully frequency dependent. That is, the magnitude of the load as well as the Phase Angle of the load can be dependent upon the frequency definitions.
Tabular (Spatially Varying): Not Supported.
Function (Time Varying): Not supported for Harmonic Response Analysis.
Function (Spatially Varying): Not Supported.
To apply a 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 the method used to define the force: Vector (default), , Components, 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.
The selections available in the Details view are described below.
| Category | Fields/Options/Description |
|---|---|
| Scope |
Scoping Method, options include:
|
| Definition |
Type: Read-only field that describes the object - Force. Define By, options include:
Suppressed: Include ( - default) or exclude () the boundary condition. |
The following Mechanical APDL commands, element types, and considerations are applicable for this boundary condition.
Force is applied using the SFE,,PRES command.
Based on the selected topology, element types include: