Harmonic Response Analysis Using Linked Modal Analysis System

Preparing the Analysis

Create Analysis System

  Basic general information about this topic

  ... for this analysis type:

Because this analysis is linked to (or based on) modal responses, a Modal analysis is a prerequisite. This setup allows the two analysis systems to share resources such as engineering data, geometry and boundary condition type definitions made in modal analysis.


Note:
  • The Mode-Superposition harmonic is allowed to be linked to a pre-stressed modal analysis.

  • When solving a linked MSUP harmonic system database from a version prior to the most current version of Mechanical, it is possible to encounter incompatibility of the file file.full created by the modal system. This incompatibility can cause the harmonic system’s solution to fail. In the event you experience this issue, use the Clear Generated Data feature and resolve the modal system.

    Refer to the Obtain the Mode-Superposition Harmonic Solution section of the MAPDL Structural Analysis Guide for more information.


From the Toolbox, drag a Modal template to the Project Schematic. Then, drag a Harmonic Response template directly onto the Solution cell of the Modal template.

Establish Analysis Settings

  Basic general information about this topic

  ... for this analysis type:

For this analysis configuration, the basic Analysis Settings include:

Options

See the Harmonic Analysis Options Group section for a complete listing of the Details properties for a Harmonic Response analysis. Note that for a Harmonic Analysis Using Linked Modal Analysis System, only the Mode-Superposition option is applicable, and therefore is read-only. In addition, you can turn the Include Residual Vectors property On to execute the RESVEC command and calculate residual vectors. Also, Mode Frequency Range is not applicable because available modes are defined in the linked Modal system.


Note:  The following boundary conditions do not support residual vector calculations:

  • Nodal Force

  • Remote Force scoped to global a Remote Point (created via Model object)

  • Moment scoped to global a Remote Point (created via Model object)


Output Controls

This category enables you to request Stress, Strain, Nodal Force, and Reaction results to be calculated. For better performance, you can also choose to have these results expanded from Harmonic or Modal solutions. To expand reaction forces in the modal solution, set the Nodal Force property to Yes or Constrained Nodes.

Define Initial Conditions

  Basic general information about this topic

  ... for this analysis type:

The Harmonic analysis must point to a Modal analysis in the Modal (Initial Conditions) object. This object also indicates whether the upstream Modal analysis is pre-stressed. If it is a pre-stress analysis, the name of the pre-stress analysis system is displayed in the Pre-Stress Environment field, otherwise the field indicates None. The Modal Analysis must extract enough modes to cover the frequency range. A conservative rule of thumb is to extract enough modes to cover 1.5 times the maximum frequency in the excitation.


Note:
  • Command objects can be inserted into Initial Conditions object to execute a restart of the solution process for the Modal Analysis.

  • If displacement loading is defined with Displacement, Remote Displacement, or Bolt Pretension (specified as Lock, Adjustment, or Increment) loads in the Static Structural analysis, these loads become fixed boundary conditions for the Harmonic solution. This prevents the displacement loads from becoming a sinusoidal load during the Harmonic solution.


Apply Loads and Supports

  Basic general information about this topic

  ... for this analysis type:

The following loads are allowed for the linked analysis:

Inertial

Acceleration (Phase Angle not supported.)

Loads
Direct FE

The Direct FE option Nodal Force is supported for node-based Named Selection scoping and constant loading only.

Acceleration as a base excitation

Support Limitations

Note the following analysis requirements.

  • Remote Force is not supported for vertex scoping.

  • Moment is not supported for vertex scoping on 3D solid bodies because a beam entity is created for the load application.

  • During a linked MSUP Harmonic analysis, if a Remote Force or Moment scoped to an internal remote point is specified with the Behavior property set to Deformable, the boundary conditions cannot be scoped to the edges of line bodies such that all of their nodes in combination are collinear.


Release 18.2 - © ANSYS, Inc. All rights reserved.