17.6.3.2. Displacement

Displacements are applied at the geometry level. They require that one or more flat or curved faces or edges or one or more vertices to displace relative to their original location by one or more components of a displacement vector in the Global Coordinate System or local coordinate system, if applied.

Important:  Due to an internal processing requirement, if you specify a user-defined (local) Coordinate System when defining this boundary condition, the nodal coordinate system axes may differ from the local Coordinate System axes. As needed, you can verify the actual nodal orientation in the Mechanical APDL application.

Also, for more information about how the application manages nodal DOF constraints, see the Converting Boundary Conditions to Nodal DOF Constraints (Mechanical APDL Solver) section.

Displacement as a Base Excitation

Displacement can also be defined as a base excitation during a Mode-Superposition (MSUP) Transient or a MSUP Harmonic Response analysis. You scope base excitations to a boundary condition. You can scope multiple base excitations to the same boundary condition, but the base excitations cannot have same direction specified (via the Direction property).

Important:  When duplicating an analysis within Mechanical that includes loads with the Base Excitation property set to Yes (Acceleration and/or Displacement), these loads will lose their scoping during the duplication process.

This page includes the following sections:

Analysis Types

Displacement is available for the following analysis types:
Dimensional Types

The supported dimensional types for the Displacement boundary condition include:

  • 3D Simulation. Displaces one or more faces, edges, or vertices.

  • 2D Simulation. Displaces one or more edges or vertices.

Geometry Types

The supported geometry types for the Displacement boundary condition include:

  • Solid

  • Surface/Shell

  • Wire Body/Line Body/Beam

Topology Selection Options

The supported topology selection options for Displacement include:

  • Body: Supported for rigid bodies in an Explicit analysis.

  • Face

    • Non-zero X-, Y-, and Z-components. The face retains its original shape but moves relative to its original location by the specified displacement vector. The enforced displacement of the face causes a model to deform.

    • For Zero Y-component, no part of the face can move, rotate, or deform in the Y-direction.

    • For blank (undefined) X- and Z-components, the surface is free to move, rotate, and deform in the XZ plane.

  • Edge

    • Enforced displacement of an edge is not realistic and leads to singular stresses (that is, stresses that approach infinity near the loaded edge). You should disregard stress and elastic strain values in the vicinity of the loaded edge.

    • Non-zero X-, Y-, and Z-components. The edge retains its original shape but moves relative to its original location by the specified displacement vector. The enforced displacement of the edge causes a model to deform.

    • For Zero Y-component, no part of the edge can move, rotate, or deform in the Y-direction.

    • For blank (undefined) X- and Z-components, the edge is free to move, rotate, and deform in the XZ plane.

  • Vertex

    • Non-zero X-, Y-, and Z-components. The vertex moves relative to its original location by the specified displacement vector. The enforced displacement of the vertex causes a model to deform.

    • For Zero Y-component, the vertex cannot move in the Y-direction.

    • For blank (undefined) X- and Z-components, the vertex is free to move in the XZ plane.

    • This boundary condition cannot be applied to a vertex scoped to an End Release.

  • Nodes

  • Element Face

Note:

  • Multiple surfaces, edges, or vertices can be selected.

  • Avoid using multiple Displacements on the same face/edge/vertex and on faces/edges/vertices having shared faces/edges/vertices.

Define By Options

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

  • Components

    • Entering a zero for a component prevents deformation in that direction.

    • Entering a blank for a component allows free deformation in that direction.

    • In a cylindrical coordinate system X, Y, and Z are used for R, Θ, and Z directions. When using a cylindrical coordinate system, non-zero Y displacements are interpreted as translational displacement quantities, ΔY = RΔΘ. Since they are treated as linear displacements it is a reasonable approximation only, for small values of angular motion ΔΘ.

    • For Explicit Dynamics analyses, when using a cylindrical coordinate system, the Y component (that is, Θ direction) of a displacement constraint is defined as a rotation.

  • Components: Real - Imaginary: Supported for Harmonic Response Analysis only. Define direct loading without Phase Angle.

  • Normal To: Supported for 3D Faces only.

  • Normal To: Real - Imaginary: Supported for Harmonic Response Analysis only. Define direct loading without Phase Angle.

  • Magnitude - Phase: Supported for Displacement as a Base Excitation during Harmonic Response analysis only.

  • Real - Imaginary: Supported for Displacement as a Base Excitation during Harmonic Response analysis only.

Magnitude Options

The supported Magnitude options for Displacement 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.

  • Tabular (Spatially Varying): Not supported for Explicit Dynamics and Harmonic Response analyses.

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

  • Function (Spatially Varying): Not supported for Explicit Dynamics and Harmonic Response analyses.

  • Free: Not supported for Displacement as a Base Excitation.

Note:   Solution Restarts are only supported for Tabular data modifications.

Applying a Displacement Boundary Condition

To apply a Displacement:

  1. On the Environment Context tab, select the Displacement option from the Structural group. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert>Displacement.

  2. Define the Scoping Method and select a geometric or mesh entity.

  3. Select the method used to define the Displacement: Components (default), Components: Real - Imaginary, Normal To, or Normal To: Real - Imaginary.

  4. Define the Coordinate System and axial displacements or the Distance, of the Displacement based on the above selections.

  5. As needed, set the Rev Dir for Inv Steps property to Yes. See the description below for requirements.

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

To apply Displacement as a Base Excitation when the Solver Type property is defined as Mode-Superposition during a Transient (default setting for a Transient configured to a Modal solution) or a MSUP Harmonic Response analysis:

  1. In the Definition category of the Details pane, set the Base Excitation property to Yes.

  2. The Boundary Condition property provides a drop-down list of the boundary conditions that correspond to the Displacement. Make a selection from this list. Valid boundary condition option for excitations include:

    • Fixed Support

    • All Fixed Supports

    • Displacement

    • Remote Displacement

    • Nodal Displacement

    • Spring: Body-to-Ground

  3. The Absolute Result property is set to Yes by default. As needed, change the value to No if you do not want to include enforced motion.

    Note:  If you apply more than one base excitation (either Displacement or Acceleration), the Absolute Result property needs to have the same setting, either Yes or No.

  4. To use complex definition entries, change the Define By property setting to Real - Imaginary from Magnitude - Phase (default).

  5. Define the loading inputs: Magnitude, Phase Angle (only in MSUP Harmonic Response), and Direction.

    Note:  You can scope Acceleration or Displacement as a base excitation to the same boundary condition, but the base excitations cannot have same direction specified (via the Direction property).

Details Pane Properties

The selections available in the Details pane are described below.

CategoryProperty/Options/Description
Scope

Scoping Method: Options include:

  • Geometry Selection: default setting, indicating that the boundary condition is applied to a geometry/geometries or mesh entity that are selected using a graphical selection tool.

    • Geometry: visible when the Scoping Method is set to Geometry Selection. Displays the type of geometry (Body, Face, etc.) or mesh entity (Element Face) and the number of geometric/mesh entities (for example: 1 Body, 11 Nodes) to which the boundary has been applied using the selection tools.

  • Named Selection: indicates that the geometry selection is defined by a Named Selection.

    • 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.

Boundary Condition (Displacement as a Base Excitation only): drop-down list of available boundary condition options for application.

Definition

Type: read-only field that describes the object - Displacement.

Base Excitation (Displacement as a Base Excitation only): No is the default setting. Set to Yes to specify the Displacement as a Base Excitation.

Absolute Result (Displacement as a Base Excitation only): This option allows you to include enforced motion with (Yes - default) or without (No) base motion.

Define By. options include:

  • Normal To: Requires entries for the following:

    • Distance. This is the distance of displacement, that is, a magnitude.

    • Phase Angle (Harmonic Analysis only)

  • Normal To: Real - Imaginary (Harmonic Analysis only): real and imaginary distance. Requires the specification of the following inputs:

    • Distance - Real

    • Distance - Imaginary

  • 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.

      Note:  If you apply a Displacement to mesh nodes, the Coordinate System property becomes read-only and is automatically set to Nodal Coordinate System.

    • 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.

  • Magnitude - Phase (Displacement as a Base Excitation for Harmonic Response only): Requires entries for the following:

    • Magnitude

    • Phase Angle (Harmonic Analysis only)

  • Real - Imaginary (Displacement as a Base Excitation for Harmonic Response only): real and imaginary magnitude. Requires the specification of the following inputs:

    • Magnitude - Real

    • Magnitude - Imaginary

Rev Dir for Inv Steps: This property is only available when the following Advanced Analysis Settings properties are defined:

  • Inverse Options property is set to Yes.

  • End Step equals the setting of the Number of Steps property.

Options include No (default) and Yes. Setting this property to Yes inverts the direction of your specified Displacement and is displayed by the change in direction of the displacement annotation in the Geometry 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.

Mechanical APDL References and Notes

The following Mechanical APDL commands and considerations are applicable when Displacement is defined as a base excitation in a Mode Superposition Transient analysis or a Mode Superposition Harmonic Response analysis.

  • Magnitude (constant or tabular) is always represented as a table in the input file.

  • Base excitation is defined using the D command under the Modal restart analysis (under Modal analysis in case of standalone Harmonic Response analysis).

  • Base excitation is applied using the DVAL command during a Mode Superposition Transient analysis or Mode Superposition Harmonic Response analysis.

Note:  Displacement can be defined as base excitation in a Modal linked Harmonic Response and Modal linked Transient analysis only when the upstream Modal analysis Solver Type is set to Program Controlled (provided program sets solver type internally to Direct or Supernode) or Direct or Supernode.

API Reference

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