Acoustics and vibro-acoustics > Alternate component representations > Modal models

Mode sets

A mode set is an alternate component representation that you can use to replace a FEM file or a component FEM file with modal model results. A modal model is a reduced form of the dynamic characteristics of a structure with a fewer degrees of freedom. Solving an assembly FEM in which some component FEM files are represented in a reduced form as mode sets takes less time and requires fewer computer resources.

For example, an assembly FEM of an aircraft contains component FEM files that represent the fuselage, wings, engines, tail, and so on. In the Simulation Navigator, you can use the Edit Representation command to replace the FEM file for each wing with a mode set that contains modal results from a previous analysis for the wings. When you solve the assembly FEM, you can use the mode sets to efficiently investigate the effect of the wing structure on the more detailed FEM model of the fuselage. You can also create mode sets of different wing versions to investigate changes in structure or material, and then evaluate the effect on the assembly FEM.

Generating the modal model

Before you can create a mode set, you must first generate the modal model to use as the basis for the mode set. A mode set is comprised of:

The modal forced response results.
The nodes and elements on which those results were computed.

To generate the modal results for a mode set, you can, for example:

Solve a Nastran SOL 103 Real Eigenvalue solution as part of a structural or vibro-acoustic analysis.
Import Test.Lab modal measurement data.

Specifying the modal data and mesh

To create a mode set, select Mode Set from the Representation list in the FE Model Component Representation dialog box. You can then use the options in the Mode Set dialog box to define the contents of the mode set.

To define a mode set, you must specify the files that contain the results and mesh data. You can select a single file that contains both the results and the mesh data, or you can specify a file that contains the results data and specify a separate file that contains the mesh data. In the Mode Set dialog box:

Use the Data Source option to specify either:A results file that contains both mode shapes and mesh data.A file that contains mode data only. You can then use the Mesh Source option to separately specify the mesh data for the mode set.You can select results files from a number of different solvers as the data source for the set.Note: The software imports MSC Nastran files without modal mass values. If you select an MSC Nastran file as the Data Source for the mode set, you must use the Edit Modes command to apply modal mass values. For more information, see Editing modes or functions in mode sets and FRF sets.
To specify a different file to define the mesh data for the set, use the Mesh Source option to specify either a file, such as a Nastran .pch file, or a FEM file that contains the appropriate mesh. For example, you can select:A FEM file that contains a mesh.A file that contains nodes attached to Nastran PLOTEL 1D elements where there is no structural or acoustic mesh.A file that contains a reduced set of nodes and elements that represents a subset of the complete model.Mesh from data source file****Mesh from a mesh source file that contains a subset of nodes and elements

You can use the Mesh Creation Modeoptions in the Mode Set dialog box to control how the software creates the mesh to use in the mode set alternate representation. For more information, see Controlling mesh creation for mode sets.

Associating additional data sources with the primary data source

If you want to include additional modal data that is associated with the Data Source file, you can use the Companion Data Sources options to add that data to the set. Use the Companion Data Sources option to import modes that are stored in different files, or even in different file types, and combine them into a single mode set. For example, you may want to include companion data sources when you use piecewise constant properties to represent visco-elastic materials and request multiple output files, where each file contains modes in a different frequency range.

Primary and companion data sources must contain the same number of nodes and elements, and those nodes and elements must have the same the same ID values.
Both primary and companion data sources can contain meshes, but the primary data source must contain a mesh.
You can specify a Simcenter Testlab file as a companion data source only when the primary data source is also a Simcenter Testlab file. The software uses the mapping table in the primary source data file (node name – node label) to read the companion Simcenter Testlab file.

Exporting mode set data

When you export or solve a solution, the software writes out the mode set data to the solver input file as six multi-point constraint equations (MPCs) for each node in the mode set. You can use the Export Options to manage how the software writes the data out to improve the solve time.

Select the Binary Format check box to export the mode set data in binary format. The software processes binary data faster than ASCII data, which can reduce the solve time.
Clear the Binary Format check box to export the mode set data in ASCII format. You can use the Constraint Equations Formatting (MPC) list to control the nodes that the software includes in the mode set. This reduces the number of constraint equations that the software writes out, which creates a smaller solver input file that is faster to solve.

Connecting nodes in mode set to other components

After you replace a component FEM with the mode set, you can connect the nodes in the mode set to the other component FEMs in the assembly FEM file to perform an evaluation of a larger and more complex structure. You can use 1D elastic elements, such as springs or beams, to create these connections. You cannot use rigid elements, such as Nastran RBE2s, RBE3s, or MPCs, to connect a mode set to other component FEMs.

Note:

You do not need to create 1D connections if your complete structure is represented as a mode set in a vibro-acoustic simulation.

Performing subsequent analyses using a mode set

After you replace a FEM file with a mode set, you can then re-solve the FEM file or the assembly FEM file. For example:

To calculate modal or frequency responses, you solve the assembly FEM using a structural or vibro-acoustic analysis using SOL 108 solution with the standard FEM method or SOL 111 solution with the either standard FEM method or the FEM Adaptive Order (FEMAO) method.
To compute dynamic responses, such as transmissibility or a frequency response function (FRF), you can solve a SOL103 Real Eigenvalue solution and then a Response Dynamics analysis on an assembly FEM file that contains a mode set.

Working with mode sets in the Simulation Navigator

When you replace a FEM file or a component FEM file with a mode set, the software adds brackets to the FEM representation in the Simulation Navigator and displays the name of the mode set. The original name of the FEM file displays in parentheses.

The software stores mode sets in a Mode Sets folder in the Simulation Navigator. The name of the set appears in blue to indicate that it is used in the model.

After you create a mode set, you can use right-click commands in the Simulation Navigator to:

Edit the mode set, for example, to change the options that you used to create the set.
Use the Edit Modes dialog box to control which modes are active, or scale the viscous and structural damping values. For more information, see Editing modes or functions in mode sets and FRF sets.
Create a contour plot of the mode set data. For more information, see Plot mode, ATV, or VATV set contours.
Delete a set. When you delete a set, the software resets the representation of the FEM or component FEM file to its base FEM representation.

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area