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%.

Output Controls

Certain results and input data can be output to a text file. Use the options within the Output tab of the Analysis Parameters dialog box to control the data that is output.

• Matrices – When this check box is activated, the stiffness and mass matrices are printed to an ASCII file named filename.mtx. The format of this output file is explained in Matrix Printout from Modal Analyses.

Other results available through text output options are...

• Displacement/eigenvector data and
• Equation numbers data

Text for these two options is included within the analysis Summary file, which is viewable from the Report environment.

Additionally, the following analysis input data can be optionally included within the Summary file...

• Element data and
• Nodal data

Use the following two options in the SimMech Stress/Strain section to control generation of optional binary output when using the native Simulation Mechanical solver. (The optional binary output is used to produce results contours viewable within the Results environment)...

• Normalized stress (binary): Activate this check box to enable viewing normalized stress contours in the Results environment.
• Normalized strain (binary): Activate this check box to enable viewing normalized strain contours in the Results environment. This option is only available if you first activate the preceding Normalized stress (binary) option.
Important: Normalized stresses and strains are not scaled to any specific structural load or excitation. They 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.