Critical Buckling Loads

Multipliers

There are four multipliers that controls the magnitudes of various loads when they are applied to the model. These are located in the Load Multipliers section of the Multipliers tab of the Analysis Parameters dialog box. The value in the Pressure multiplier field will multiply the magnitudes of all pressures and surface forces on the model. The value in the Acceleration multiplier field will multiply the magnitudes of any acceleration loads on the model. The value in the Displacement multiplier field will multiply the magnitudes of any displacement boundary elements applied to the model. The value in the Thermal multiplier field will multiply the thermal loads 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

Solution Options Section

There are two solvers available for a critical buckling load analysis. This can be specified in the Type of solver drop-down menu in the Solution tab of the Analysis Parameters dialog box.

  • The Automatic option will pick the optimum solver based on the model size.
  • The Sparse option is recommended for large models. The sparse solver also takes advantage of multiple threads/cores if available in the computer.
  • The Inverse option may provide a faster solution for small models. If the Avoid bandwidth minimization check box is activated, the bandwidth minimization will not be performed. This usually makes the analysis run longer.

The Percent memory allocation controls how much of the available RAM is used to read the element data and to assemble the matrices. (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 drop-down Number of threads/cores control is enabled when the solver is set to sparse.. 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.

Inverse Iteration Solver Section

If you are using the inverse solver, specify the convergence tolerance to be used in the Convergence tolerance for Eigenvalue field and specify how many iterations can be used to achieve this tolerance in the Maximum number of iterations field.

Sparse Solver Section

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

  • The Type of sparse solver drop-down menu contains the sparse solvers currently available. If you choose a solver that is not available on an operating system, the processor will use the best one for the operating system. The sparse solvers available are as follows:
    • Default: use BCSLIB-EXT on Windows and use inverse iterative solver on Linux.
    • BCSLIB-EXT (Windows only): use the Boeing solver. 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 C:\Documents and Settings\Username where C: is the drive on which the operating system is installed. 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 directory 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 other sparse solvers adjust the memory setting automatically; so no setting is required for them.
  • The Sophisticated usage option is turned on by default. This option provides a robust solution for most models. Users might deactivate this option to reduce the solution time. However, if the nature of the model is ill conditioned, the solver may fail during the solution.
  • The Number of buckling modes to calculate field sets the number of buckling modes to calculate. Usually, the first mode (the lowest buckling load) is of interest.
  • The Upper buckling load cutoff factor and Lower buckling load cutoff factor fields will limit what buckling load multipliers are calculated. The number of requested buckling modes will start with the first buckling mode with a load factor larger than the lower cutoff. The analysis will end once a buckling mode with a load factor larger than the cutoff is calculated. This capability is useful when the lowest buckling mode is not of interest. For example, the lowest theoretical mode may occur if the loads are reversed, but in some cases you know that the loads cannot be reversed. In this situation, a small negative number for the lower cutoff prevents the calculation of the negative buckling loads.

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.

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 will use 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 will not be used. Therefore, the nodes must match for parts to be bonded.
  • Coarse bonded to fine mesh Smart bonding will create 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 will create 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 2 to 10 4 is recommended.

Notes:
  • 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.

Parent topic: Analysis Parameters