17.6.2.6. Force

Force is specified based on the following topologies:

  • Vertex: Applies a Force vector to one or more vertices.

  • Edge: Distributes a Force vector along one or more straight or curved edges, resulting in uniform line load along the edge.

  • Face: Distributes a Force vector across one or more flat or curved faces, resulting in uniform traction across the face.

  • Node: Applies a Force to an individual node or a set of nodes. This scoping is the same as using an Nodal Force except that you scope the nodes directly (no Named Selection is required). As such, the Force is applied using the Mechanical APDL F command.

    Note:  Node-based scoping is not supported for Harmonic Response or Explicit Dynamics analyses.

  • Element Face: Distributes a Force across one or more element faces.

This page includes the following sections:

Analysis Types

Force is available for the following analysis types:
Dimensional Types

The supported dimensional types for the Force boundary condition include:

  • 3D Simulation

  • 2D Simulation: Not supported for 2D axisymmetric Explicit Dynamics analyses.

Geometry Types

The supported geometry types for the Force boundary condition include:

  • Solid

  • Surface/Shell

  • Wire Body/Line Body/Beam

Topology Selection Options

The supported topology selection options for Force include:

  • Face

    • 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

    • 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.

    Note:  You cannot apply a single Force load on multiple edges of different surface bodies, when the bodies include both a 3D surface body and a 2D surface body.

  • Vertex

    • 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 for 2D only.

  • Element Face: Supported for 3D only.

Define By Options

The supported Define By options for the Force boundary condition include:

  • Vector: Not supported for Node selection.

  • Components

  • Vector: Real - Imaginary: Supported for Harmonic Response analysis only.

  • Components: Real - Imaginary: Supported for Harmonic Response analysis only.

When using the Mechanical APDL solver, for all of the above Define By property options, the Force boundary condition also displays the Applied By property. This property has two options: Surface Effect (default for non-Mode Superposition) and Direct (Mode Superposition default).

The Surface Effect option applies Force using the surface effect elements created on the top of the scoped geometry. The Direct option applies Force directly onto the faces of solid or shell elements in 3D analyses. In 2D analyses, the Direct option applies pressure directly onto the edges of plane elements.

Note:

  • If you scope two Force objects to the same geometry, and specify the loads in the same direction, using the Direct option, the Forces do not produce a cumulative loading effect. The Force object that you specified last takes priority and is applied, and as a result, the application ignores the other Force object.

  • A Nodal Force and a Force applied using the Direct option share the same scoping and produce a resultant loading effect.

  • A Force applied using the Surface Effect option and a Force applied using the Direct option produce a resultant effect.

  • If your analysis includes some combination of a Pressure, a Force, and a Hydrostatic Pressure load, and 1) all are set to the Direct option, 2) share the same scoping, and 3) have the same Direction, whichever load was written to the input file last, overwrites all previous loads.

Important:  For the Mechanical APDL solver, note the following limitations when using the Direct option for Applied By property:

  • Not supported for vertices and edges of Solid bodies and Line bodies.

  • Not supported on bodies associated with General Axisymmetric and Condensed parts.

  • Not supported if the model has any cracks defined under the Fracture folder.

  • Not supported if the analysis includes a Nonlinear Adaptive Region object and 1) the Loaded Area property is set to Initial and 2) the Large Deflection property (Analysis Settings > Solver Controls) set to On.

  • In a multiple step analysis, if you define more than one load (Pressure, Force, or Hydrostatic Pressure) using the Direct option, and they share the same scoping, deactivation of a particular load step in one of these loads could delete all the other loads in that load step and following steps.

Magnitude Options

The supported Magnitude options for Force include the following:

  • Constant

  • 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 (Harmonic Index Varying): Supported only for a Harmonic Response (Full) analysis that includes a Cyclic Region object. By default, at least two harmonic index entries are required when defining a harmonic index dependent tabular load. The Force load for this analysis can be defined such that it is fully harmonic index dependent. That is, the magnitude of the load as well as the phase angle of the load can be dependent upon the harmonic index definitions.

  • Tabular (Sector Number): Supported for Harmonic Response (Full) analysis only when a Cyclic Region is defined. By default, at least two entries are required to define a dependent tabular load.

  • Function (Time Varying): Not supported for Harmonic Response analysis.

Applying a Force Boundary Condition

To apply a Force:

  1. Select the Force option from the Environment Context tab. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert>Force.

  2. Define the Scoping Method as either Geometry Selection or Named Selection and then specify the geometry.

  3. Select the method used to define the Force: Vector (default), Vector: Real - Imaginary, Components, or Components: Real - Imaginary.

  4. Specify the Applied By property: Surface Effect (non-Mode Superposition default) and Direct (Mode Superposition default).

  5. Define the Magnitude, Coordinate System directional loading, and/or Direction of the load based on the above selections.

    Note:

    • The Direction property is not associative and does not remain joined to the entity(s) selected for its specification. Therefore, this direction is not affected by geometry updates, part transformation, or the Configure tool (for joints).

    • 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.

  6. For Harmonic analyses, specify a Phase Angle as needed.

Details Pane Properties

The selections available in the Details pane are described below.

CategoryProperty/Options/Description
Scope

Scoping Method: This property specifies how you perform geometric entity selection. Options include Geometry Selection (default) and Named Selection.

Geometry Selection: Visible when the Scoping Method is set to Geometry Selection. Displays the type of geometry (Body, Face, etc.) and the number of geometric entities (for example: 1 Body, 2 Edges) to which the boundary has been applied using the selection tools.

Named Selection: Visible when the Scoping Method is set to Named Selection. This field provides a drop-down list of available user–defined Named Selections.

Definition

Type: Read-only field that describes the object - Force.

Define By: Options include:

  • Vector: A magnitude and direction (based on finite element selection). Requires the specification of the following inputs:

    Magnitude: Enter desired value.
    Direction: Specify using either the Node or Element Face selection option. When you select one Element Face, the Direction is normal to the selected face. When you select multiple Element Faces, the Direction is the average of the normals of all the faces. When you select two nodes (singular selection is not supported), the Direction is the direction along a line segment that includes both points. If you select three or more Nodes, the Direction calculation equals the surface normal of the first three nodes selected.
    Phase Angle (Harmonic analysis only)

  • Vector: Real - Imaginary (Harmonic analysis only): Real and imaginary magnitude and direction (based on selected geometry). Requires the specification of the following inputs:

    Magnitude - Real
    Magnitude - Imaginary
    Direction

  • Components: Option to define the loading type as Components (in the Global Coordinate System or local coordinate system, if applied). Requires the specification of at least one of the following inputs:

    Coordinate System: Drop-down list of available coordinate systems. Global Coordinate System is the default.
    X Component: Defines magnitude in the X direction.
    Y Component: Defines magnitude in the Y direction.
    Z Component: Defines magnitude in the Z direction.
    X Phase Angle (Harmonic analysis only)
    Y Phase Angle (Harmonic analysis only)
    Z Phase Angle (Harmonic analysis only)

    Note:  Selection of a Coordinate System rotated out of the global Cartesian X-Y plane is not supported in a 2D analysis.

  • Components: Real - Imaginary (Harmonic analysis only): Option to define the loading type as real and imaginary components (in the Global Coordinate System or local coordinate system, if applied). Requires the specification of at least one of the following inputs:

    Coordinate System: Drop-down list of available coordinate systems. Global Coordinate System is the default.
    X Component - Real: Defines magnitude (Real) in the X direction.
    X Component - Imaginary: Defines magnitude (Imaginary) in the X direction.
    Y Component - Real: Defines magnitude (Real) in the Y direction.
    Y Component - Imaginary: Defines magnitude (Imaginary) in the Y direction.
    Z Component - Real: Defines magnitude (Real) in the Z direction.
    Z Component - Imaginary: Defines (Imaginary) magnitude in the Z direction.

Divide Load by Nodes (visible for Node scoping only): 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.

Applied By: This property defines how the load is applied. Either by creating surface effect elements or by direct application on the scoped geometry. Options include:

  • Surface Effect: default option for all analyses except Mode Superposition analyses.

  • Direct: default option for Mode Superposition analyses.

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.

Important:  When you specify the load as Tabular, the Independent Variable property displays and is set to Harmonic Index by default. The Harmonic Index property is hidden as their values are entered in the table.

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. If you choose Tabular for the Magnitude property, you can then set the Independent Variable property to Sector Number and then specify your loading using the Tabular Data window.

Suppressed: Include (No - default) or exclude (Yes) the boundary condition.

Step Controls (Visible for Harmonic Response analysis with multiple load steps defined)

Step Varying: Options include No (default) and Yes. When you select No, the Remote Load is applicable at all defined steps. When set to Yes, only the load step selected in either the RPM Selection or Step Selection properties described below is applicable.

RPM Selection: This property displays when the Multiple Step Type property is set to RPM. Specify a Step Selection value from the values available in the RPM Value property of the Analysis Settings object to use for the Remote Load.

Step Selection: This property displays when the Multiple Step Type property of the Analysis Settings object is set to Load Step. Specify a Step Selection value from the values available in the Load Step Value property of the Analysis Settings object to use for the Remote Load.

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.

Mechanical APDL References and Notes

The following Mechanical APDL commands, element types, and considerations are applicable for this boundary condition.

  • When you set the Applied By property to Surface Effect, a Force is applied using the using the SFE ,,PRES command by creating the applicable elements as listed below.

  • Based on the selected topology, element types include:

    • SURF154 - 3D structural analyses for face selection.

    • SURF156 - 3D structural analyses for edge selection.

    • SURF153 - 2D structural analyses for edge selection.

    • FOLLW201 - 2D and 3D for vertex selection.

  • When you set the Applied By property to Direct, a Force is applied directly on to the element faces using the SFCONTROL and SFE ,,PRES commands. Refer to SFCONTROL command for a list of supported solid elements, shell elements, and plane-2D elements.

API Reference

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