17.6.1.1. Acceleration

The global Acceleration boundary condition defines a linear acceleration of a structure in each of the global Cartesian axis directions.

If desired, Acceleration can be used to simulate gravity (by using inertial effects) by accelerating a structure in the direction opposite of gravity (the natural phenomenon of). That is, accelerating a structure vertically upwards (+Y) at 9.80665 m/s2 (in metric units), applies a force on the structure in the opposite direction (-Y) inducing gravity (pushing the structure back towards earth). Units are length/time2.

Alternatively, you can use the Standard Earth Gravity load to produce the effect of gravity. Gravity and Acceleration are essentially the same type of load except they have opposite sign conventions and gravity has a fixed magnitude. For applied gravity, a body tends to move in the direction of gravity and for applied acceleration, a body tends to move in the direction opposite of the acceleration.

Acceleration as a Base Excitation

Acceleration can also be defined as a base excitation during a Mode Superposition Transient analysis or a Mode Superposition Harmonic Response analyses. 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

Acceleration is available for the following analysis types:

Dimensional Types

Acceleration applies a uniform load over all bodies. The supported dimensional types include:

  • 3D Simulation

  • 2D Simulation

Geometry Types and Topology Selection Options

By virtue of Acceleration's physical characteristics, this boundary condition is always applied to all bodies of a model.

Define By Options

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

  • Vector

    While loads are associative with geometry changes, load directions are not. This applies to any load that requires a vector input, such as Acceleration.

    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.

  • Components

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

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

Magnitude Options

The supported Magnitude options for Acceleration include the following:

  • Constant

  • Tabular (Time Varying)

  • Tabular (Step Varying): Supported for Static Structural and Rigid Dynamics analyses 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.

  • Function (Time Varying): Not supported for Explicit Dynamics or LS-DYNA analyses.

    For a Rigid Dynamics analysis, if the Acceleration is defined using an expression, you cannot also have a Standard Earth Gravity object.

Applying an Acceleration Boundary Condition

To apply an Acceleration:

  1. On the Environment Context tab, click Inertial>Acceleration. Alternatively, right-click the Environment object in the tree or in the Geometry window and select Insert>Acceleration.

  2. Select the method used to define the Acceleration: Options include Vector (default) or Components.

  3. Define the loading inputs: Magnitude, Coordinate System, and/or Direction of the Acceleration based on the above selections.

To apply Acceleration 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 Mode-Superposition Harmonic Response analysis:

  1. 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 Acceleration. Make a selection from this list. Valid boundary conditions 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. 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. As needed, set the Define By property to Real - Imaginary from Magnitude - Phase (default).

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

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

Details Pane Properties

The selections available in the Details pane are described below.

CategoryProperty/Options/Description
Scope Geometry: Read-only field indicating All Bodies.

Boundary Condition (Acceleration as a Base Excitation only): Drop-down list of available boundary conditions for application.

Definition

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

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

Define By: Options for this property include the following:

  • Vector: Requires the specification of the following inputs:

    • Magnitude

    • Phase Angle (Acceleration as a Base Excitation for MSUP Harmonic Response only).

    • Direction

  • Components: Requires the specification of the following inputs:

    • X Component

    • Y Component

    • Z Component

  • Coordinate System: Drop-down list of available coordinate systems. Global Coordinate System is the default. When using cyclic symmetry, the referenced coordinate system must match coordinate system used in the Cyclic Region. For a 2D axisymmetric model, the referenced coordinate system must be the Global Coordinate System. The referenced coordinate system must be Cartesian.

  • Magnitude - Phase (Acceleration as a Base Excitation for Harmonic Response analysis only): Requires the specification of the following inputs:

    • Magnitude

    • Phase Angle

  • Real - Imaginary (Acceleration as a Base Excitation for Harmonic Response analysis only): Requires the specification of the following inputs:

    • Magnitude - Real

    • Magnitude - Imaginary

Suppressed: Include (No) 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.

Note:  Step varying displacements can only be applied in one direction for all load steps, for a selected set of nodes.

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 and considerations are applicable for Acceleration:

  • Acceleration is applied using the ACEL command.

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

Note:

  • Should both an Acceleration and a Standard Earth Gravity boundary condition be specified, a composite vector addition of the two is delivered to the solver.

  • In a Mode-Superposition Transient analysis, Standard Earth Gravity is not allowed in conjunction with Acceleration.

Condensed Parts

Important:  When working with substructures, if the inertial acceleration is scoped to a Condensed Part, the nodes of the condensed part are not marked as the master degree of freedom. Instead, multiple super element load vectors are generated for each acceleration component via the substructure restart mechanism and scaled using SFE ,,SELV command. See the ANTYPE ,SUBSTR,RESTART command in the Mechanical APDL Command Reference. For additional information, see The CMS Generation Pass in the Substructuring Analysis Guide.

Limitation:  If your analysis includes a Condensed Part, the application does not support Acceleration when the Step Varying property is set to Yes.

Base Excitation

The following Mechanical APDL commands and considerations are applicable when Acceleration 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:  Acceleration 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, Supernode, or Subspace).

API Reference

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

Acceleration and Standard Earth Gravity Examples

The following illustrations compare how Acceleration and Gravity can be used to specify a gravitational load with the same result:

Global Acceleration Load Applied in the +Y Direction to Simulate Gravity and Deformation Result

Standard Earth Gravity Applied and Deformation Result