Transient Structural 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 linked setup allows the transient system to share resources such as engineering data, geometry, and boundary condition type definitions made in the Modal Analysis.

Linking the Modal Solution cell to the Transient Setup cell configures the Transient analysis so that the application selects, by default, the Mode-Superposition Solution Method.

The Samcef and ABAQUS solvers do not support a linked Modal/Transient Structural analysis. For additional support requirements and notes regarding this analysis configuration, see the references at the bottom of this section.


Note:
  • For a Mode-Superposition Transient Structural analysis, the Modal analysis can be pre-stressed by a Static Structural analysis.

  • When solving a linked MSUP transient 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 transient 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 Transient 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 Transient Structural template directly onto the Solution cell of Modal template.

Establish Analysis Settings

  Basic general information about this topic

  ... for this analysis type:

For a Transient Structural system linked to a Modal system, the basic Analysis Settings include:

Step Controls

This analysis is only compatible with constant time stepping. So, auto time stepping is turned off and will always be in read only mode. The user specified substep or time step value is applicable to all the load steps. All of the Step Controls settings applied to this analysis are not step aware. The time integration is turned on by default and will always be in read-only mode. A Time Step value that results in an integral number of sub steps over the load step must be selected.

Options

These controls enable you to turn on the property Include Residual Vector to execute the RESVEC command and calculate residual vectors.


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

  • Nodal Force

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

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


Output Controls

These controls enable you to request Stress, Strain, Nodal Force, Reaction, Velocity and Acceleration results to be calculated. To expand reaction forces in the modal solution, set the Nodal Force property to Yes or Constrained Nodes. The General Miscellaneous property needs to be set to Yes in order to apply a Beam Tool and/or to calculate Beam Results. In addition, this setting is required to correctly produce twisted beam shapes. For better performance, you can also choose to have these results expanded from transient or modal solutions. The Contact Miscellaneous option is not available.


Note:  Solver Controls, Restart Controls, Nonlinear Controls and Creep Controls are not applicable to the current analysis.


Define Initial Conditions

  Basic general information about this topic

  ... for this analysis type:

The Transient Structural 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 all modes that may contribute to the dynamic response.


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


Apply Loads and Supports

  Basic general information about this topic

  ... for this analysis type:

The following loads are allowed for the linked analysis:

Direct FE

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

Support Limitations

Note the following limitations:

Notes


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