Natural Frequency - Modal

Define the Number of Frequencies/Modes to Solve

In the Analysis Parameters dialog box, specify the number of frequencies/modes to solve for in the Number of frequencies/modes to calculate field. If the model is not sufficiently restrained to prevent rigid body motion (free body motion), then this input must also include the number of rigid body modes. Thus, the total number of modes includes x rigid body modes and y elastic modes. For example, if you want 5 modes and the model has 3 rigid body modes, then you should request 8 modes.

The Lower cut-off frequency field is not available, and will be grayed-out, when the Type of Solver option is set to Subspace-AMG under the Solution tab. When available, this field is used to skip the lowest natural frequencies of a model. The processor starts solving for the requested number of natural frequencies starting with the first natural frequency above this value. This can be used to reduce processing time if you know that your structure is not affected by frequencies below a certain level.

The Upper cut-off frequency field is not available, and will be grayed-out, when the Type of Solver option is set to Subspace-AMG under the Solution tab. When available, this field used to terminate computations if all eigenvalues below the specified frequency have been found. The calculation terminates when the nearest eigenvalue higher than the upper cut-off frequency has been determined. Only those modes whose frequencies are less than the upper cut-off frequency is used in subsequent dynamic restart analyses.

Account for Rigid Body Modes in Models

A rigid body mode occurs in a model if motion can occur in any of the six degrees of freedom. This is like linear static stress when the error message your model is not tied down enough appears. The mode shape processor can still solve the model if rigid body modes occur, but you must activate the Rigid body modes are expected check box in the General tab of the Analysis Parameters dialog box. For example, if you have a beam model with no constraints and you run a natural frequency analysis, most likely you encounter six rigid body modes because the model is in 3D space and there are six degrees of freedom. A rigid body mode in your model gives a natural frequency of zero or close to zero. You may want to account for this by solving for more frequencies.

Include rotational mass for beam elements

Select this option when you expect torsional modes in your beam model. The option approximates the rotational mass of beam elements. If you do not select this option, beam elements are represented as a lumped masses and torsional modes are not calculated. See Beam Elements for more information.

Solver Options

Solution Options Section

Use the Type of solver drop-down menu in the Solution tab of the Analysis Parameters dialog box to choose which type of solver to use for the analysis.

  • If the Automatic option is selected, the processor chooses the type of solver to use based on the size of the model and the number of frequencies to be found. For smaller models or for solutions of many eigenvalues, the Sparse solver is used. Conversely if the model is larger and you request a relatively small number of frequencies, then the Subspace-AMG solver is used. The equation for determining which solver to use is:

    If #DOF / #Freq > 10,000, then use the Subspace-AMG solver. Otherwise, use the Sparse solver.

    Where:

    • #DOF is the number of degrees of freedom (equations)
    • #Freq is the requested number of frequencies to be found

    Hence, for the default number of frequencies (5), models with greater than 500,000 degrees of freedom will use the Subspace-AMG solver.

  • Choosing the Sparse option forces the usage of this solver, regardless of model size or the requested number of modes.
  • Choosing the Subspace-AMG option forces the usage of this solver, regardless of the model size or number of modes.
Note: If multiple threads/cores are available on your computer system, both solvers use all of them to solve the set of equations. Also, both solvers will take advantage of 64-bit processing when available.

Percent memory allocation: For the sparse solver, this field controls how much of the available RAM is used to read the element data and to assemble the matrices. A small value is recommended when using the sparse solver. This input field is disabled for the Subspace-AMG solver. The value controls how much of the available RAM is used to perform the entire analysis. When the value is less than or equal to 100%, the available physical memory is used. When the value of this input is greater than 100%, the memory allocation uses available physical and virtual memory. The default value is 50%.

As listed above, the solvers take advantage of multiple threads/cores when available on the computer. The drop-down Number of threads/cores controls how many threads/cores are used. Use all of the threads/cores available for the fastest solution. Alternatively, choose to use fewer threads/cores if you need some computing power to run other applications at the same time as the analysis.

Subspace Iteration Section

The Subspace Iteration section is only applicable to and is only available if you are using the Subspace AMG solver.

  • The Maximum number of iterations field controls the number of iterations allowed in the attempt to reach the convergence tolerance. The default value is 32 and the processor uses a maximum of 100 if you enter a zero.
  • The option selected in the Accuracy of last frequency drop-down list is used to trade off solution speed versus solution accuracy for the highest modal frequency result. The choices are:
    • Fair (fast) – Use this setting for the quickest solution, when you are not as concerned about the accuracy of the last frequency as compared to the first few vibration modes.
    • Good – This setting balances performance and accuracy of the last frequency.
    • Better (slowest) – This setting provides the best accuracy of the last frequency result but also requires the greatest solution time.

Sparse Solver Section

If the sparse solver is chosen, then the Sparse Solver section is enabled. The inputs for this section are as follows:

  • The Type of sparse solver drop-down menu contains the choices Default and BCSLIB-EXT. Since there is only one sparse solver available currently, the action of either choice is identical:
    • Default uses the BCSLIB-EXT solver.
    • BCSLIB-EXT (Boeing sparse solver, supported on Windows and Linux): For Windows only, note that the BCSLIB-EXT solver may write temporary files to the folder specified by the environment variable USERPROFILE. By default, this variable is set to the folder %SYSTEMDRIVE%\Users\Username where %SYSTEMDRIVE% is the drive on which the operating system is installed, typically C:. The error numbers -701 or -804 returned from the BCSLIB-EXT solver means that it ran out of hard disk space for storing the temporary files. If this occurs, change the USERPROFILE variable to a folder on a drive that can provide sufficient hard disk space. (See the Windows Help and Support for documentation on changing environment variables.)
  • The Solver memory allocation field sets the amount of memory to use during the sparse matrix solution for the BCSLIB-EXT solver. In general, allocating more memory should result in a faster analysis. The default value is 100%.

Control Data in Text Output Files

After the analysis is complete, the analysis results can be output to a text file. The Output tab of the Analysis Parameters dialog box can be used to control the data that is output to this file. If the Matrices check box is activated, the stiffness and mass matrices is printed to the filename.mtx file. This output is in ASCII format. The format of this output is explained in Matrix Printout from Modal Analyses.

Normalized stress / Normalized strain outputs normalized stress and strain results. Normalized stresses and strains are not scaled to any specific structural load or excitation, and are only intended to demonstrate relative stress and strain distributions for the various mode shapes. The absolute magnitudes of these results are not meaningful.

Advanced Settings

Number of vectors in solution

The number of vectors to be used in the analysis can be specified in this field under the Advanced tab of the Analysis Parameters dialog box.

For the Subspace-AMG solver, if a zero is entered, then the processor automatically calculates this value to be the minimum of the following two choices:

  • Number of frequencies requested + 8, or
  • 2 * number of frequencies requested.

For the Sparse solver, if a 0 is entered, the processor calculates this value to be 2 * number of frequencies requested.

If you specify a positive, non-zero number of vectors, the processor will use the maximum of the following two choices for the number of vectors:

  • The requested number of vectors, or
  • The number of frequencies requested.

Frequency Shift

A frequency shift can be used when rigid body modes are present in cases when the solver encounters solution problems. For example, an analysis may give a negative diagonal warning. Apply a shift to adjust the rigid body modes to avoid the negative diagonal. An approximate shift value is the square of the first natural frequency (in radians/sec). This is specified in the Frequency shift field in the Advanced tab of the Analysis Parameters dialog box.

Do not save restart files

There are several analyses that can be performed after a natural frequency (modal) analysis that require files generated during the natural frequency (modal ) analysis. These include response spectrum, frequency response, random vibrations and transient stress. If you do not plan on performing these analyses, you can activate the Do not save restart files check box in the Advanced tab of the Analysis Parameters dialog box.

Stop after stiffness calculations

This check box can be activated to prevent the processor from performing the analysis after the stiffness matrix has been generated. The Attempt to correct matrix problems and continue check box can be activated if you want the processor to attempt to fix any negative diagonals that are encountered during the analysis.

Contact Settings

There are two methods of handling bonded connections. Which method is used depends in part on whether the nodes are matched between the two parts or not matched.

Activating the option Enable smart bonded/welded contact on the Contact tab uses multipoint constraint equations (MPCs) when necessary to bond the nodes on part A, surface B with the nearest nodes on part C, surface D. Shape functions interpolate the displacements at the nodes on surface B to the nodes on surface D. Therefore, the meshes do not need to match between the parts. The MPCs are used for all the nodes on the surface contact pair whenever any node does not match. If the meshes do match at all nodes, then node matching is used to bond the contact surface; the two vertices on the adjoining parts are collapsed to one node, and MPC equations are not used for the contacting surfaces. The options for the smart bonding drop-down are as follows:

  • None: Smart bonding is not used. Therefore, the nodes must match for parts to be bonded.
  • Coarse bonded to fine mesh: Smart bonding creates MPC equations that connect the nodes on the surface with the coarser mesh to the nodes on the surface with the finer mesh.
  • Fine bonded to coarse mesh: Smart bonding creates MPC equations that connect the nodes on the surface with the finer mesh to the nodes on the surface with the coarser mesh.

The smart bonding option applies to bonded contact and welded contact. See the page Meshing Overview: Creating Contact Pairs: Types of Contact for a discussion of defining contact and additional information about using smart bonding.

By default, smart bonding uses the condensation method to solve your analysis. If you find your analysis doesn't converge or is not performing as you expect, you can try a different Solution method to use with MPC equations (see Multi-Point Constraints). Click SetupLoadsMulti-Point Constraint and choose from the Solution method options. If you use the Penalty Method, the accuracy of the solution is controlled by the Penalty multiplier field. The Penalty multiplier, times the maximum diagonal stiffness in the model, is used during the penalty solution. A value in the range of 10 4 to 10 6 is recommended.

Note:
  • The solution method you select in the Define Multi-Point Constraints dialog box becomes the method used for all features that include MPCs. These features include, but are not limited to, cyclic symmetry, frictionless constraints, smart bonding, and user-defined MPCs. For example, if you want to use the Penalty Method to solve all your analyses involving smart bonding, you can override the default condensation method by selecting Penalty Method in the Define Multi-Point Constraints dialog box.
  • Smart bonding applied to contact between brick, 2D, membrane, and plate elements. Bonded contact involving other element types requires the nodes to match and are not affected by the smart bonding setting.

When the option Enable smart bonded/welded contact is not activated, the parts are bonded only if the nodes match between the parts.

Topics in this section
Parent topic: Analysis Parameters