Create a DMIG-based FEM

Creating a DMIG (Direct Matrix Input at Gridpoints) of a FEM file requires three main steps:

1. Create and solve a SOL103 superelement solution for the FEM file. The DMIG is output as a punch (.pch) file.

2. Edit the punch file so it can be read by Simcenter 3D.

3. Import the edited punch file to Simcenter 3D to create a new FEM. You will use this FEM, in which stiffness, mass, or damping are stored in matrix collectors, to replace a standalone FEM file or a component FEM in an assembly FEM.

Create and solve a SOL103 Superelement solution

1. Using the method you normally use, create or open a Simulation and FEM file, or import a Nastran input file that contains the model to be converted to a DMIG.For more information, see Creating new FEM and Simulation files or Importing Nastran data.

2. Create a SOL 103 Superelement solution. Specify the Solver as Simcenter Nastran, Analysis Type as Structural, and click OK.For more information, see Create or modify a solution.

3. In the Simulation Navigator, right-click Solver Sets and choose New→DOF Set to create a DOF set containing the nodes to define the superelement.These nodes should include selected free boundary nodes and nodes used to connect to other component FEMs. For more information see DOF sets .

4. In the DOF Set dialog box, select the nodes to include, select the Degrees of Freedom for those nodes, and click OK.

5. Right-click the solution name and choose Edit.

6. On the Case Control page, from the Superelement Options list, select an option and click Edit , or click Create Modeling Object to create a new one.

7. In the Superelement Options dialog box, do the following:Clear the Generate Assembly Process Bulk Data Entries and the Generate External Superelement Bulk Data Entries check boxes.Clearing these check boxes only creates DMIG-type matrices.From the File Format list, select DMIGPCH.In the External Superelement ID box, enter an integer number.You must create a unique ID number for the superelement.Click OK.

8. On the Case Control page, from the Output Requests list, select an output request and click Edit , or click Create Modeling Object to create a new one.

9. In the Structural Output Requests dialog box, do the following: Click Disable All.Click the Displacement page, and select the Enable DISPLACEMENT Request check box.(Optional) To limit the displacement output, from the Entity list, select Group and make the appropriate selections. For more information see Groups.When the SOL 103 Superelement solution computes the modes, displacements are computed for every node. To limit the .pch file size, especially for very large models, consider selecting only the nodes you have selected for the DOF Set. Click OK.

10. On the Case Control page, from the Lanczos Data list, select an option and click Edit , or click Create Modeling Object to create a new one.

11. In the Lanczos dialog box, do the following:In the Number of Desired Modes box, type the number of modes to solve.Selecting a large number of modes makes the DMIG valid for high frequencies and is a more accurate representation of the structure. One drawback is the large amount of displacement data that may result.Click OK.

12. On the Bulk Data page, from the Fixed Boundary (BSET) and Residual Vector (RVDOF) lists, select the DOF set you defined in step 4.

13. Click OK.

14. Solve the solution and save all the files.

Edit the punch (.pch) file

You must add case control information to the punch file so it can be imported.

1. Navigate to the punch file you created with the SOL 103 Superelement solution. Open the punch file (.pch) file with a text editor, such as Notepad.

2. At the first line of the punch file, enter these lines:TITLEK2GG = KAAXM2GG = MAAX****CENDIf your DMIG includes other results, such as viscous or structural damping, add these additional lines to the case control section:B2GG = BAAX****K42GG = KDMIG

3. Replace the line BEGIN SUPER 1 with BEGIN BULK.

4. After the last line in the file, type ENDDATA.

5. Save the file and exit the text editor.

Import the punch file to create a new FEM file based on the DMIG

1. In Simcenter 3D, create a temporary FEM file by choosing File→New.

2. Go to the Simulation tab, select Simcenter Nastran, and in the New File Name dialog box, type a new file name, such as my_workfile.fem, and click OK. The name is not important because this file is not saved.

3. Click OK.

4. In the New FEM dialog box, click OK.

5. Choose File→Import→Simulation.

6. In the Import dialog box, select Simcenter Nastran and click OK.

7. In the Import Simulation dialog box, do the following:Select ASCII as the file type and click Browse to navigate to the modified punch file. In the Select file to import dialog box, from the Files of type list, select PCH File (.pch).Browse or navigate to the punch file that you edited and click OK. Click OK to close the remaining dialog boxes.The software reads the punch file and creates a new FEM and Simulation file using the name of the punch file. The FEM file contains the DMIG matrices in a Matrix Collectors container.

8. (Optional) In the Simulation Navigator, make the FEM file the displayed part and examine the Matrix Collectors that contain the stiffness (K2GG) and mass (M2GG) matrix elements. The stiffness, mass, and damping matrices are stored in individual collectors.

9. To change the display of the matrix elements, right-click a matrix stiffness collector and choose Edit Display. Selecting the Text check box displays the matrix element label. The label is an M if it is a matrix element, and MS if the matrix element contains SPOINTs.

10. Save the FEM and Simulation files.

In the next step, you will replace a component FEM in an assembly FEM, or a standalone FEM, with the DMIG-based FEM. For more information, see Replace a component FEM with a DMIG-based FEM.

How do I

Replace a component FEM with a DMIG-based FEM

Learn more

DMIG as a matrix element

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Create a DMIG-based FEM, 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 } });