Set up a large deflection, prestressed modal cyclic symmetry analysis

To calculate the frequencies and mode shapes of a deformed structure, you can perform a prestressed modal analysis (using the linear perturbation solution method) of cyclic structures after you perform a large-deflection nonlinear static analysis. The linear perturbation modal analysis procedure takes into account the prestress effects.

1. In the Simulation Navigator, right-click the Simulation file, and choose New Solution.

2. Create the nonlinear statics solution. In the Solution dialog box, do the following:Set the Solver list to ANSYS.Set the Analysis Type list to Structural. Set the Solution Type list to Nonlinear Statics.

3. On the General tab, select the Large Displacements check box.

4. On the Cyclic Symmetry tab, select or define the Cyclic Attributes (CYCLIC) and Cyclic Options (CYCOPT) modeling objects.

5. On the Restart Controls tab, select or define the Restart Controls (RESCONTROLS) modeling object. For example, you can specify the frequency with which ANSYS writes the results files.

6. Solve the Nonlinear Statics solution.

7. Create the modal solution. In the Solution dialog box, do the following:Set the Solver list to ANSYS.Set the Analysis Type list to Structural. Set the Solution Type list to Modal.

8. On the Cyclic Symmetry tab, select or define the Cyclic Options (CYCOPT) modeling object. You do not need to specify the Cyclic Attributes (CYCLIC) modeling object again.

9. On the Restart tab:Select the ANSYS Restarts check box.Specify the name of the results file from the previous Nonlinear Statics solution.Select or define the Linear Perturbation Options (PERTURB) modeling object. (Optional) Select or define the Contact Element KEYOPTS Modification (CNKMOD) modeling object to modify the behavior of individual contact pairs.

10. On the General tab, specify the appropriate options for the modal analysis.

11. Solve the Modal solution.In the Post Processing Navigator, the software associates the results from the restart solution (.rst file) with the original solution and not with the restarted solution. In this example, the results are stored with the original Nonlinear Statics solution and not with the Modal solution.

Learn more

ANSYS prestressed modal analyses with linear perturbation

Controlling how ANSYS writes restart files

Modifying the behavior of contact pairs

Specifying linear perturbation options

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Set up a large deflection, prestressed modal cyclic symmetry analysis, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });