Natural Frequency - Modal - with Load Stiffening

Define Number of Frequencies/Modes to Solve

In the Parameters tab of 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 BCSLIB-EXT sparse solver is used (see Solver Options below), the results found can be further limited by entering a value for the Lower cut-off frequency and the Upper cut-off frequency. The modes between the lower and upper cut-off frequencies, up to the number of modes requested, is output by the processor.

If you have previously performed a natural frequency (modal) analysis on this model and want to start the load stiffening analysis from those results, activate the Begin with Linear Modal results check box.

Select Include rotational mass for beam elements when you expect torsional modes in your beam model. This 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.

Load Multipliers Section

There are four multipliers that control the magnitudes of various loads when they are applied to the model. These are located in the Load Multipliers section of the Parameters tab of the Analysis Parameters dialog box. The value in the Pressure multiplier field multiplies the magnitudes of any pressures or surface forces on the model. The value in the Acceleration multiplier field multiplies the magnitudes of any acceleration loads on the model. The value in the Displacement multiplier field multiplies the magnitudes of any displacement boundary elements applied to the model. The value in the Thermal multiplier field will multiply the thermal load in the model, where the thermal load is proportional to (coefficient of thermal expansion) * (nodal temperature - stress free reference temperature). The thermal multiplier does not multiply the applied temperatures.

Solver Options

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 solved for. Most of the time, the BCSLIB-EXT sparse solver is used. If multiple threads/cores are available on a system, the sparse solver uses all of them to solve the set of equations. The sparse solver is recommended for large models. The subspace solver uses an iterative solution and can be more efficient for simple models.

For the sparse solver, the Percent memory allocation 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. For the subspace solver, this controls how much of the available RAM is used to perform the entire analysis. This should be a relatively high number when using the subspace solver. (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 Stop after stiffness calculations check box can be activated to prevent the processor from performing the analysis after the stiffness matrix has been generated.  The Attempt to run despite errors check box can be activated it you want the processor to attempt to fix any negative diagonals that are encountered during the analysis. (Sometimes, a very small negative value (a value close to 0) can occur due to the element shape. Switching these stiffnesses to positive value allows the solution to proceed and generally has a negligible effect on the solution. However, this should not be used if negative value is a large value; in this case, fix the model instead.)

If the type of solver used is the Subspace solver, the subspace iteration algorithm terminates the calculation when the eigenvalue is accurate to the tolerance specified in the Convergence tolerance for Eigenvalue field. You can control how many iterations are allowed to be used to converge on this tolerance in the Maximum number of iterations field. It is important to make sure the Avoid bandwidth minimization check box is not activated. Deactivating this check box decreases the analysis runtime when using the Subspace solver. These three fields have no affect when using the BCSLIB-EXT sparse solver.

The Solver memory allocation field in the Sparse Solver section sets the amount of memory to use during the sparse matrix solution for the BCSLIB-EXT sparse solver. In general, allocating more memory should result in a faster analysis.

As listed above, some of the solvers take advantage of multiple threads/cores available on the computer. The drop-down Number of threads/cores control is enabled in such situations. You want to use all the threads/cores available for the fastest solution, but might choose to use fewer threads/cores if you need some computing power to run other applications at the same time as the analysis.

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. The following three options control the inclusion of text-type results...

• Displacement/eigenvector data
• Suppress stress data – Note that the stress data is included by default. Activate this checkbox to exclude the stress data from the output text.
• Equation numbers data

Text for the above three 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
• Nodal data
• Centrifugal load data

Use the following two options within the Output tab to control binary output (used for producing results contours viewable within the Results environment)...

• Normalized stress (binary)
• Normalized strain (binary) – Note that this option is only available if you first activate the preceding Normalized stress (binary) option.

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.

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 multi-point 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 Types of Contact page 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 10² to 10⁴ 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 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.