Modal Simulation Tool

The Modal Simulation tool allows you to define a modal analysis (that is, solve for Eigenvalues) based upon modal solution options and constraint sets specified by a NASTRAN bulk data deck, ABAQUS input file, STL file, or a Mechanical model. You may also modify the following settings when requesting a Mechanical APDL command input file.

Imported File Requirements

The Mechanical application: the environment input into FE Modeler must be from a Modal analysis in order to display the modal options.

NASTRAN: require models to have SOL equal to 103 in the executive control to display the modal options.

ABAQUS: the *FREQUENCY keyword should be defined in the input deck in order to display the modal options.

Steps to Perform a Modal Analysis

Use the following procedure to perform a Modal analysis on an imported ABAQUS, NASTRAN, Mechanical, or Mechanical APDL archived file.

  1. Import a Mesh file into FE Modeler. FE Modeler displays the Import Summary.

  2. Select any object on the Outline tree and then select Insert>Modal Simulation or right-click the mouse and select Insert>Modal Simulation. The Modal Simulation object is placed in the tree and the Details View displays any modal analysis specifications associated with the imported file.


    Note:  If the input file does not contain modal analysis specifications, you must set new specifications for a modal analysis.


  3. Verify the contents of the following fields. If necessary, modify the values.

    • Number of Modes

    • Frequency Range

    • Mode Extraction Method

  4. Select a Constraint Set for the modal analysis. By default, a Free-Free configuration is defined and no constraints are written to the Mechanical APDL application input file.


    Note:  The following conditions apply:

    • Only one constraint set can be used to generate the Mechanical APDL application input.

    • For Mechanical models, only one constraint set (other than Free-Free) is available.

    • For ABAQUS and NASTRAN files, all constraint sets from the bulk data input are displayed in the Constraint Sets field.


  5. Select Generated Data in the Tree View section of the screen or the Export button in the Standard Toolbar. Modal analysis specifications are now included.

Verify Node Location

To verify the location of nodes contained in a constraint set or to verify the specific degrees of freedom that are constrained, use the Constraints View. This view displays the settings for each constraint set available. For example, if a Constraint Set from a NASTRAN model has a Set ID of nine (9), the Constraints View may display the following components:

SPC <SET:9, DOFS: 1,2,3,4,5,6, VALUE: 0>
SPC <SET:9, DOFS: 1,2,3,4,5,6, VALUE: 0>
SPC <SET:9, DOFS: 1 , VALUE : 0>
SPC <SET:9, DOFS: 2, 3, VALUE:0>

By selecting each of these components you can visualize the nodes that are constrained in all directions, as well as those constrained in direction 1(UX) , 2 (UY) and 3 (UZ) only. All of these values compose Constraint Set 9.


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