DMIG as a matrix element

You can use a DMIG (Direct Matrix Import at Gridpoint) as a matrix element to represent a structure in matrix form, such as stiffness, mass, damping, or acoustic coupling. A DMIG provides a stiffness, mass, or damping representation of a structure, without exposing the details. When you use a DMIG, you can share a FEM without revealing proprietary or confidential information.

Each DMIG is stored in a mesh collector as a matrix element and can be used in an assembly FEM or a standalone FEM. For example, you can import a DMIG to use as a tire model with an automotive FEM, or as a satellite on a launch vehicle.

The element associated data contains the matrix. You can import, export, and use DMIGs, but not edit or create them directly in Simcenter 3D.

To create a DMIG, you must:

1. Convert a structural FEM into a .pch (Nastran PUNCH file) file using a superelement solution (SOL 103 Superelement).

2. Import the DMIG .pch file into Simcenter 3D to create a DMIG-based FEM.

3. Replace a structural component FEM with the DMIG-based FEM in an assembly FEM or in a standalone FEM.

You create a DOF Set to select a group of nodes and to specify the active degrees of freedom for each node. For each node in the set, you can set each degree of freedom to active or inactive. For more information, see DOF sets.

The DMIG matrix element is displayed with lines from each node in the DOF Set to the center of gravity of all the nodes. A letter M labels the element. If scalar points (SPOINTs) are included in the element, then the label MS is displayed.

For more information on SOL103 Superelement solution and SPOINTs, see Superelement analysis.

You control the conversion of DMIG matrices from the .pch file by using Simcenter Nastran case control. A DMIG represents the matrices in the bulk data file as the following:

Simcenter 3D	Nastran Case Control
Stiffness matrix	K2GG
Mass matrix	M2GG
Viscous damping matrix	B2GG
Structural damping matrix	K42GG
Acoustic fluid-structure coupling matrix	A2GG

When you use a DMIG representation, consider the following conditions:

• When you use all the structural modes for each superelement, using a DMIG gives the exact answer. However, typically you solve for the modes within a frequency range. In that case you introduce approximations to the solution. The number and location of boundary nodes that you choose for the DOF Set also affect the solution quality.

• If you do not choose the appropriate boundary degrees of freedom, you can compensate by using a large number of component modes. Likewise, if you do not calculate many component modes, proper selection of the boundary degrees of freedom can improve the accuracy.

• No standard method work bests for all problems. The default method of dynamic reduction (Craig-Bampton CMS) works well for most problems; however, there are always some problems for which it may not.

You can import a DMIG from:

• A Simcenter Nastran or MSC Nastran punch file (.pch) file.

• A Simcenter Nastran .op2 file generated with PARAM,OIBULK in the Bulk Data section.

• A Simcenter Nastran or MSC Nastran .op2 file generated without PARAM,OIBULK in the Bulk Data section.

For more information, see Create a DMIG-based FEM or the following:

Overview of Direct Matrix Input

DMIG Case Control User Interface

Defining Mass, Damping, and Stiffness through Direct Input Matrices

Complete assembly FEM with (1) satellite component FEM and (2) payload adapter component FEM	DMIG representation of satellite FEM

Satellite component FEM replaced with DMIG-based component FEM

How do I

Create a DMIG-based FEM

Replace a component FEM with a DMIG-based FEM

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

DMIG as a matrix element, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });