Importing CAE data

Estimated time to complete: 15–25 minutes

In this tutorial, you will import an I-deas FE model using an I-deas Universal file and also using a Simcenter Nastran bulk data file.

1: Setup

  1. On your desktop or the appropriate network drive, create a folder named import_ideas_model.

  2. Click the link below:

    Download the part.

  3. Extract the files to your import_ideas_model folder.

  4. Start Simcenter 3D or NX.

File

New

  • Model

  •  

  • Model

    Modeling

    Millimeters

  • Name

    fork.prt

  • Folder

    your part file folder name

  • OK

     
2: Reset dialog box memory

The options you select in dialog boxes are preserved for the next time you open the same dialog box within a given session. Restore the default settings to ensure that the dialog boxes are in the expected initial state for each step of the activity.

File

Preferences→User Interface

  • Options

  •   Reset Dialog Memory

  • OK

     
3: Import the I-deas Universal file

File

  • Import→Simulation

  • Select solver

    Ideas Unv

  • OK

     

  • Browse

     

    Navigate to your part file folder.

  • File name

    fork.unv

  • OK

     IDEAS UNV Import Selection dialog box

  • OK

     Import Simulation dialog box

  • Available FEMs

    IdeasFEModel

  • OK

     all dialog boxes

Leave the Information window open.

4: Examine the imported model

When the import is complete, the Information window displays the details of the import process:

  • A new FEM file was created (but no Simulation file).

  • Five beam sections were imported.

  • Eight physical property tables were created.

  • Three materials were created.

  • 8040 nodes were created.

  • 4485 elements were read, of which 4427 elements were created. There were 58 rigid elements, which cannot be imported using the UNV translator.

  • Two groups were created.

  • Beam associated data was also created.

To complete this model, you would need to add the 58 rigid elements and also create the Simulation file with the loads and boundary conditions.

  the Information window

The new FEM file appears.

5: Consolidate the 1D meshes

Examine the mesh collectors and meshes in the Simulation Navigator. Notice that several mesh collectors were created to store the 1D meshes.

 

Simulation Navigator

  • 1D Collectors

  • Linear Beam(1)

  • Edit

    Note the physical property table assigned to the mesh collector in the Linear Beam list: BEAM BY XSEC IDEAS PTABLE.

  • Cancel

     

The first four Linear Beam mesh collectors use the same BEAM BY XSEC IDEAS PTABLE physical property table. You can confirm this by examining all the 1D mesh collectors and noting the physical property tables assigned.

Because these four 1D meshes have the same physical properties, there is no need to have each of them in a separate mesh collector.

Simulation Navigator

  • 1d_mesh(2)

  • 1d_mesh(2) into the Linear Beam(1) collector 

  • Apply Defaults

      Move Mesh Display Settings box

  • the other two linear beam meshes into the Linear Beam(1) collector 

  • Delete the empty mesh collectors.

6: Consolidate the 2D meshes

Only one 3D mesh collector was created, so no consolidation is necessary for the 3D meshes.

Examine the 2D mesh collectors. You will see that the 2D meshes use three physical property tables:

  • SHELL 4MM IDEAS PTABLE

  • SHELL 3MM IDEAS PTABLE

  • SHELL 2MM IDEAS PTABLE

  • Rename the Thin Shell(1), Thin Shell(3), and Thin Shell(5) mesh collectors to 4mmShell, 3mmShell, and 2mmShell respectively.

  • Consolidate the 2D meshes into three collectors. Organize them according to their physical properties.

  • The consolidated meshes should look like this:

  • Delete the empty mesh collectors.

  • Save

7: Export the FE model to UNV

For situations in which your company has developed custom applications that accept FEM data in Universal file format, you may want to manipulate data in your new imported model and then export the model again to a Universal file.

File

  • Export→Simulation

  • Browse

     

  • File name

    fork1.unv

  • OK

     all dialog boxes

 

The Information window displays the details of the export process:

  • Three materials are exported. For each exported material, the Information window lists unsupported material properties.

  • 11 physical property tables are exported.

  • 4427 elements are exported.

  • Beam element associated data is exported.

  • Two groups are exported.

  the Information window

File

  • Close→All Parts

You could now import this UNV file into your custom application as needed.

Next, you will create a FEM and Simulation file by importing the Simcenter Nastran bulk data file.

8: Create an empty part file

File

New

  • Model

  •  

  • Model

    Modeling

    Millimeters

  • Name

    fork2.prt

  • Folder

    your part file folder name

  • OK

     
9: Import the Nastran bulk data file

File

  • Import→Simulation

  • Select solver

    Simcenter Nastran

  • OK

     Import dialog box

  • Browse (File Name)

  • Navigate to your part file folder.

  • File name

    fork.dat

  • OK

      all dialog boxes

Leave the Information window open for the next step.

10: Examine the imported model

When the import process is complete, the Information window displays this information:

  • The ANALYSIS OF BULK DATA section lists information about each Nastran bulk data entry recognized and the number of entities imported for each bulk data entry.

  • The SUMMARY OF BULK DATA section lists the number of nodes, coordinate systems, restraints, elements, physical properties, materials, loads, and modeling objects imported.

Notice that a Simulation file has been created and the loads and boundary conditions have been imported.

  the Information window

As you can see, importing the Simcenter Nastran bulk data file offers a more complete import of your I-deas model.

11: Solve the model

Simulation Navigator

  • fork

  • Solve

  • Edit Solution Attributes

     

  • Element Iterative Solver

  • OK

     both dialog boxes

  •  

    Wait until the solution is complete.

  • No

     Review Results dialog box

  •   the Information window

  • Cancel

     Analysis Job Monitor dialog box

12: Review the results

Simulation Navigator

  •     fork→Results

  • Structural

 

  Post Processing Navigator

  •    fork→Structural

  •    Stress - Element-Nodal

  • Plot

     

 

 Save

File

  • Close→All Parts