www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS Workbench

A modal analysis determines the vibration characteristics (natural frequencies and mode shapes) of a structure or a machine component. It can also serve as a starting point for another, more detailed, dynamic analysis, such as a transient dynamic analysis, a harmonic response analysis, or a spectrum analysis. The natural frequencies and mode shapes are important parameters in the design of a structure for dynamic loading conditions.

You can also perform a modal analysis on a prestressed structure, such as a spinning turbine blade.

Only linear behavior is valid in a modal analysis.

Damping is ignored in a modal analysis.

Any applied loads are ignored.

Prestressed modal analysis requires performing a static structural analysis first. In the modal analysis you can use the

**Initial Condition**object to point to the**Static Structural**analysis to include prestress effects.

**Attach Geometry**

*Basic
general information about this topic*

**...
for this analysis type:**

There are no specific considerations for a modal analysis.

**Define Part Behavior**

*Basic
general information about this topic*

**...
for this analysis type:**

Material properties must be linear but can be isotropic or orthotropic, and constant or temperature-dependent. You must define stiffness in some form (for example, Young's modulus, hyperelastic coefficients, and so on) as well as mass (Density, remote mass) in some form. All nonlinear properties are ignored.

**Define Connections**

*Basic
general information about this topic*

**...
for this analysis type:**

Any nonlinear contact such as

Frictionalcontact retains the initial status throughout the modal analysis. The stiffness contribution from the contact is based on the initial status and never changes.Joints are supported for modal analysis if they act as supports to a constraint.

The stiffness of any spring is taken into account, however any damping specified is ignored.

**Apply Mesh Controls/Preview Mesh**

*Basic
general information about this topic*

**...
for this analysis type:**

There are no specific considerations for a modal analysis.

**Define Analysis Type**

*Basic
general information about this topic*

**...
for this analysis type:**

Choose

Modalas theNew Analysistype.

**Establish Analysis Settings**

*Basic
general information about this topic*

**...
for this analysis type:**

Number of Modes: You need to specify the number of frequencies of interest. The default is to extract the first 6 natural frequencies. The number of frequencies can be specified in two ways:

The first N frequencies (N > 0), or

The first N frequencies in a selected range of frequencies.

Solver Type: Typically you should let the program choose the type of solver appropriate for your model.

Output Controls: By default only mode shapes are calculated. You can request

StressandStrainresults to be calculated but note that “stress” results only show the relative distribution of stress in the structure and are not real stress values.Analysis Data Management settings enable you to save specific solution files from the

Modalanalysis for use in other analyses. You can setFuture Analysisfield toRandom Vibration Analysisif you intend to use the modal results in a subsequentModalorRandom Vibration(PSD) analysis. More details are available in the section Define Initial Condition.

**Define Initial Condition**

*Basic
general information about this topic*

**...
for this analysis type:**

You can point to a

Static Structuralanalysis in theInitial Conditionenvironment field if you want to include prestress effects. A typical example is the large tensile stress induced in a turbine blade under centrifugal load that can be captured by a static structural analysis. This causes significant stiffening of the blade. Including this prestress effect will result in much higher, realistic natural frequencies in a modal analysis.## Note

www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS Workbench

When you perform a prestressed modal analysis, the support conditions from the static analysis are used in the modal analysis. You cannot apply any new supports in the modal analysis portion of a prestressed modal analysis.

**Apply Loads and Supports**

*Basic
general information about this topic*

**...
for this analysis type:**

No loads are allowed in the modal analysis. All structural supports can be applied. Due to their nonlinear nature, compression only supports are not recommended in a modal analysis. Use of compression only supports may result in extraneous or missed natural frequencies.

## Note

www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS Workbench

Pre-stressed Modal Analysis:In a pre-stressed modal analysis any structural supports used in the static analysis persist. Therefore, you are not allowed to add new supports in the pre-stressed modal analysis.

**Solve**

*Basic
general information about this topic*

**...
for this analysis type:**

Solution Informationcontinuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis.

**Review Results**

*Basic
general information about this topic*

**...
for this analysis type:**

Highlight the

Solutionobject in the tree to view a bar chart of the frequencies obtained in the modal analysis. A tabular data grid is also displayed that shows the list of frequencies.You can choose to review the mode shapes corresponding to any of these natural frequencies by selecting the frequency from the bar chart or tabular data and using the context sensitive menu (right mouse click) to choose

Create Mode Shape Results. You can also view a range of mode shapes as illustrated in step 6 under the Example: Modal Analysis below.You can view the mode shape associated with a particular frequency as a contour plot. You can also animate the deformed shape. The contours represent relative displacement of the part as it vibrates.

Mode shape pictures are helpful in understanding how a part or an assembly vibrates, but do not represent actual displacements. If there are structural loads present in the environment, then the frequencies and mode shapes will depend on the loads and their magnitudes.

**Create Report (optional)**

*Basic
general information about this topic*

**...
for this analysis type:**

There are no specific considerations for a modal analysis.

The following example illustrates performing a modal analysis in Simulation.

Open the model in Simulation and set up a modal analysis.

Open the file

`Beam.dsdb`from one of the following locations:Windows platform:

`...\Program Files\ANSYS Inc\v110\AISOL\Samples\Simulation`Unix platform:

`.../ansys_inc/v110/aisol/Samples/Simulation`

Choose

**New Analysis> Modal**from the toolbar.

Specify 12 modes to extract.

**Analysis Settings**Details View: Set**Max Modes to Find**= 12.

Apply a fixed support to one end of the beam.

Select the end face, then choose

**Supports> Fixed Support**from the toolbar.

Solve the analysis without results.

Choose

**Solve**from the toolbar.

View a bar chart of frequencies.

Highlight

**Solution**object folder. Bar chart is displayed in**Timeline**window.

Create modal shape results for all frequencies or a subset of the frequencies.

Drag the mouse to highlight frequencies of interest in the

**Timeline**window or multi-select the frequencies in the**Tabular Data**window, then click the right mouse button and choose**Create Mode Shape Results**.

Evaluate results at each selected frequency.

Highlight the

**Solution**object folder, then click the right mouse button and choose**Evaluate All Results**.

Rename each result object to display associated frequency.

Highlight all result objects, then click the right mouse button and choose

**Rename Based on Definition**.

View result contours.

Highlight any result object. The associated result contour is displayed in the

**Geometry**window.