OptiStruct is a proven, modern structural solver with comprehensive, accurate and scalable solutions for linear and nonlinear
analyses across statics and dynamics, vibrations, acoustics, fatigue, heat transfer, and multiphysics disciplines.

Elements are a fundamental part of any finite element analysis, since they completely represent (to an acceptable
approximation), the geometry and variation in displacement based on the deformation of the structure.

The different material types provided by OptiStruct are: isotropic, orthotropic, and anisotropic materials. The material property definition cards are used to
define the properties for each of the materials used in a structural model.

High Performance Computing leverages computing power, in standalone or cluster form, with highly efficient software,
message passing interfaces, memory handling capabilities to allow solutions to improve scalability and minimize run
times.

Contact is an integral aspect of the analysis and optimization techniques that is utilized to understand, model, predict,
and optimize the behavior of physical structures and processes.

OptiStruct and AcuSolve are fully-integrated to perform a Direct Coupled Fluid-Structure Interaction (DC-FSI) Analysis based on a
partitioned staggered approach.

Aeroelastic analysis is the study of the deflection of flexible aircraft structures under aerodynamic loads, wherein
the deformation of aircraft structures in turn affect the airflow.

OptiStruct provides industry-leading capabilities and solutions for Powertrain applications. This section aims to highlight OptiStruct features for various applications in the Powertrain industry. Each section consists of a short introduction, followed
by the typical Objectives in the field for the corresponding analysis type.

This section provides an overview of the capabilities of OptiStruct for the electronics industry. Example problems pertaining to the electronics industry are covered and common solution
sequences (analysis techniques) are demonstrated.

Superelement or DMIG (Direct Matrix Input) approach is a known industry standard to efficiently reduce out the user-defined
components to the specified interface grids and this method helps improve the performance of finite element analysis
when used properly.

Preloaded or Prestressed Linear Analysis is any type of structural linear analysis performed on a structure under
prior loading (also termed preloading or prestressing).

Imperfection is used in large displacement nonlinear static analysis, for example, to solve post-buckling problems
combined with the arc-length method, among other techniques.

Cyclic symmetry is a type of symmetry in which a representative (or basic) segment, if patterned circularly about
an axis of symmetry would result in the full model.

OptiStruct generates output depending on various default settings and options. Additionally,
the output variables are available in a variety of output
formats, ranging from ASCII (for example, PCH) to binary files (for example,
H3D).

A semi-automated design interpretation software, facilitating the recovery of a modified geometry resulting from a
structural optimization, for further use in the design process and FEA reanalysis.

The OptiStruct Example Guide is a collection of solved examples for various solution sequences and optimization types and provides
you with examples of the real-world applications and capabilities of OptiStruct.

Superelement or DMIG (Direct Matrix Input) approach is a known industry standard to efficiently reduce out the user-defined
components to the specified interface grids and this method helps improve the performance of finite element analysis
when used properly.

Superelement or DMIG (Direct Matrix Input) approach is a known industry standard to
efficiently reduce out the user-defined components to the specified interface grids and this
method helps improve the performance of finite element analysis when used
properly.

Factorization of assembled matrices is computationally expensive for Implicit Finite
Element analysis. The cost is even higher if the factorization has to be repeated
multiple times such as for time domain or frequency domain dynamic analysis.

Standard Superelement versus Internal Superelement

The Standard superelement process consists of two steps:

DMIG generation run: the matrix reduction of components

Residual run: the final assembly run which uses DMIG

With the Internal superelement process, both DMIG generation run and residual run are
performed at the same time.

The main benefit of the Internal superelement process is to be able to retain the
model hierarchy, similar to the full model analysis (which does not use any DMIG)
and it is very easy to switch from the internal superelement process to full model
analysis.

Input Data

Internal superelements are defined using:

SUPER: Assigns a subcase(s) to a superelement or set of
superelements

SESET: Defines interior grids.

SEQSET: Assigning modal coordinate

SECSET: Defines the boundary degrees-of-freedom to be
free (c-set) during the calculations for the component mode synthesis

SETREE: Specifies the superelement reduction order

CSUPEXT: Assigns the exterior points to a
superelement

Define Superelements in OptiStruct

Consider an example involving four superelements. Before the analysis, all the
necessary superelements are created.

Each SUBCASE is created with a SUPER and a
METHOD card. The SUPER card provides
information about the individual superelement (SUPER refers to
SESET which defines the interior points for a given
superelement), while the dynamic modes for the reduction (Component mode synthesis)
are specified using the METHOD card. SUBCASE specific parameter
(PARAM,ORIGK4) may be used to replace all the material
damping coefficients.

With internal superelements, all the grids are by default, exterior points. The user
selects the proper interior points by
SESET for each superelement. For the given element, if the
part of grids is chosen as interior points, the rest of grids remain as exterior
points, as all the grids are exterior points by default (Figure 3).

Alternatively, you can explicitly pick certain grids as exterior points using
CSUPEXT. This can be used to ensure that the chosen grids
remain as the exterior points.

Review Superelements

Each Superelement is stored as a reduced matrix in the form of an
.h3d file in the working directory (Figure 4).

The interior and exterior grids for each Superelement can be reviewed from the
<filename>.intsup file created in the working directory
(Figure 5).

The exterior points which are created automatically and the interior points generated
by you can be visualized from the created sets in HyperMesh. This method can then be used as a verification for
the points that have been created.

Recovery of Results

The results from internal superelements can be recovered similar to standard
superelements (Figure 8 and Figure 9). However, in order to recover displacements,
PLOTEL elements must be created inside the internal
superelement. The PLOTEL elements would be automatically stored
in the same .h3d file, where the reduced matrices are present.
After the residual run, the displacement from the PLOTEL grid
would be recovered, if displacement output is requested for the
PLOTEL grids.

Multi-level Superelement Tree

The multi-level superelement tree is used to reduce the number of interface DoFs in
subsequent residual runs. It is performed by aggregating a few lower-level
components of the tree structure (Figure 10).

Comments

A job involving superelements will be skipped if the corresponding
.h3d files are already present in the working
directory. In such cases:

The .h3d files for specific superelements can
be deleted and the corresponding new superelements would be
re-generated by the job

PARAM,ISGENH3D,YES will initialize the
generation, even if the previously generated
.h3d files are present in the
directory

When the same Grid point is defined in SESET, as well as
in CSUPEXT, the Grid point in CSUPEXT
is considered.

Currently, optimization is not supported with internal superelements.