Module 7 Modal Analysis

7. Modal Analysis Modal analysis is used to determine a structure’s vibration characteristics — natural frequencies and mode shapes. It is the most fundamental of all dynamic analysis types and is generally the starting point for other, more detailed dynamic analyses. In this chapter, we will describe how to do a basic modal analysis via the following topics: A. Procedure B. Workshop For details, refer to your Structural Analysis Guide or Dynamics Training Manual. October 30, 2001 Inventory #001571 7-2

Modal Analysis A. Procedure The steps to do a modal analysis are as follows: Preprocessing Geometry Meshing Solution Analysis Type and Options Loading Solve Postprocessing Review results October 30, 2001 Inventory #001571 7-3

Modal Analysis ...Procedure Geometry & Meshing Same considerations as a static analysis: Include as many details as necessary to sufficiently represent model geometry. A fine mesh will be needed to resolve complex mode shapes. Both Young’s modulus and density are required. Specify mass density instead of weight density when using British units. weight density (lb/in3)  g (in/sec2) = mass density (lb-sec2/in4) For example, density of steel = 0.283/386 = 7.3E-04 lb-sec2/in4 Linear elements and material properties only. Nonlinearities are ignored. October 30, 2001 Inventory #001571 7-4

Modal Analysis ...Procedure Analysis Type The analysis type is modal. Solution > -Analysis Type- New Analysis Or issue ANTYPE,MODAL October 30, 2001 Inventory #001571 7-5

Modal Analysis ...Procedure Analysis Options Mode extraction options MODOPT command or Solution > Analysis Options... Method: Block Lanczos is generally recommended. Number of modes: Specify the number of modes you want to extract. Mode expansion options MXPAND command or Solution > Analysis Options... Expanding modes allows you to view them in the postprocessor. Number of modes is usually the same as the number extracted. Prestress effects PSTRES command or Solution > Analysis Options... calculate mode shapes of a prestressed structure, such as a spinning turbine blade. Default settings are usually sufficient October 30, 2001 Inventory #001571 7-6

Modal Analysis ...Procedure Loading & Solve The only “loads” valid in a modal analysis are displacement constraints: Solution > -Loads- Apply > Displacement > Or use the D family of commands: D, DK, DL, DA, etc. If you don’t specify constraints, ANSYS will calculate rigid body modes (zero frequency). After all constraints have been specified, obtain the solution: First save the database (SAVE command or Toolbar > SAVE_DB). Then issue SOLVE (or Solution > -Solve- Current LS). October 30, 2001 Inventory #001571 7-7

Modal Analysis ...Procedure Review Results POST1 (the general postprocessor) is used to review modal analysis results. Typically, the first step is to list the natural frequencies: General Postproc > Results Summary Or issue SET,LIST Note that each mode is stored in a separate substep. October 30, 2001 Inventory #001571 7-8

Modal Analysis ...Procedure To plot a mode shape: First read results for that substep General Postproc > Results Summary... Or use the SET command Then plot the deformed shape General Postproc > Plot Results > Deformed Shape Or use the PLDISP command October 30, 2001 Inventory #001571 7-9

Modal Analysis ...Procedure You can also animate mode shapes: Utility Menu > PlotCtrls > Animate > Mode Shape Or use the ANMODE command Another option is to plot contours stresses and strains. Note, however, that displacement and stress values are simply relative numbers and have no real meaning. October 30, 2001 Inventory #001571 7-10

Modal Analysis B. Workshop This workshop consists of the following problem: W6. U-Bracket Please refer to your Workshop Supplement for instructions. October 30, 2001 Inventory #001571 7-11