HyperWorks Solvers

FEA Setup and Modeling

FEA Setup and Modeling

 Previous topic Next topic Expand/collapse all hidden text  

FEA Setup and Modeling

 Previous topic Next topic JavaScript is required for expanding text JavaScript is required for the print function  
hmtoggle_plus1How can I apply multiple constraints or loads in a subcase?

OptiStruct can only accept one SPC and one LOAD component in a subcase, by default. There are two ways to apply multiple constraints and loads in a subcase.

1.Put multiple loads in one load collector, and include that one load collector in the subcase. The same method can be used in the case of multiple constraints.
2.Create load collectors for each and every load and constraint set. When you want to apply multiple loads in a subcase, a new load collector needs to be created with the LOAD card. Then, individual load collectors can be combined using the LOAD card. The LOAD card also enables you to associate an independent weighting factor to an individual load collector. In the case of applying multiple constraints, create a new load collector with the SPCADD card, and follow the same procedure as in the multiple load case. Once the combined load collectors are created, they can be applied in a subcase.
hmtoggle_plus1How can I specify an enforced displacement in a subcase (or loadstep) in an OptiStruct input deck?

There are two ways to do this:

1.Create a single SPC definition containing the enforced displacement information and reference this within the subcase (loadstep) definition.
2.Create an SPC, SPCD pair, with the SPC constraining the dof that is to have the enforced displacement and the SPCD defining the magnitude and dof of the enforced displacement. Both must be referenced in the subcase (loadstep) definition.
hmtoggle_plus1What kinds of checking does the check run perform?  What is the difference between the CHECK and the ANALYSIS card in the input deck?

The check run checks for syntax errors, input errors (missing LOAD or SPC card in subcase), and gives the recommended memory for the analysis or optimization run. All errors or warning messages will be output to the .out file.

If the CHECK card is included in the input file, chosen as a Run Option in HyperMesh, or added as a run option on the command line, OptiStruct will only perform the check run.

If the ANALYSIS card is included in the input deck, chosen as a Run Option in HyperMesh, or added as a run option on the command line, OptiStruct will perform only baseline analysis and no optimization.

Note:

A request for a check run always takes precedence over a request for an analysis run, and a request for an analysis run always takes precedence over an optimization.

hmtoggle_plus1How can I specify the temporary directory (where all the scratch files are written) to run OptiStruct jobs?

In an OptiStruct input, the complete path to the temporary directory (which has enough disk space for the scratch files) can be entered on the TMPDIR card. The TMPDIR card is available in HyperMesh in the control cards panel.

Also, note that when a temporary directory is specified, it is important to verify that the directory has correct read and write permissions.
hmtoggle_plus1What is the OptiStruct equivalent of the Nastran K6ROT parameter?

In Nastran, shell elements have five degrees of freedom per node, three displacements and two rotations. The K6ROT parameter provides an in-plane rotational stiffness (so-called drilling stiffness) accounting for the missing sixth degree of freedom. The absolute stiffness value provided by K6ROT is applied to all shell elements in the same manner. This way a singular stiffness matrix is avoided for shell models.

In OptiStruct, the shell elements have a built-in drilling stiffness. Each element’s drilling stiffness is calculated from the element properties using a shape function. This way, the shell elements in OptiStruct have six degrees of freedom per node, three displacements and three rotations. The OptiStruct approach is more accurate, since it derives the drilling stiffness from the structural properties of each element. This leads to somewhat different results between OptiStruct and Nastran for shell models.

An alternative shell element formulation is available in OptiStruct that matches more closely with the Nastran formulation. The primary difference with respect to the default OptiStruct shells is the absence of drilling stiffness. Some stabilization terms and other adjustments are added for reliable performance. The resulting elements are generally more flexible than the default OptiStruct shell elements, especially on curved geometries.

hmtoggle_plus1Is OptiStruct Benchmarked?

OptiStruct finite elements are benchmarked with the MacNeal-Harder tests, NAFEMS benchmarks, and some other problems posted by individuals and companies.

The NAFEMS benchmark problems and results are documented in the OptiStruct Verification Problems manual.