# Internal Superelements

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:
1. DMIG generation run: the matrix reduction of components
2. 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).