Creating a 2D mesh

Estimated time to complete: 15–25 minutes

In this tutorial, you will create a 2D mesh of a bracket.

1: Setup

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

  2. Click the link below:

    Download the part

  3. Extract the part file to your twod_meshing folder.

  4. Start Simcenter 3D or NX.

  5. Open bracket2.prt.

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: Create the FEM and Simulation files

  Simulation Navigator

  • bracket2.prt

  • New FEM and Simulation

  • Create Idealized Part

  • Solver

    Simcenter Nastran

  • Analysis Type

    Structural

  • OK

     all dialog boxes
4: Display the idealized part

  Simulation Navigator

  •  

  •  bracket2_fem1_i

  •   Make Displayed Part

  • OK

     Idealized Part Warning message box

5: Promote the bracket

Before you can modify the idealized part, you must place an associative copy of the master part file in the idealized part file. To do this, you can use the Promote command.

  Promote (Home tab→Start group)

  •   the bracket body

  • OK

     
6: Create a midsurface

Midsurface models are commonly used to simplify the analysis of thin-walled parts.

 Midsurface by Face Pairs (Geometry Preparation group)

  • the bracket body

  •  Automatically Create Face Pairs

  • OK

     
Note:

Midsurface by Face Pairs uses the average thickness of all faces in the pair. The thickness near the blend areas may contribute more.


7: Display the FEM file

Because you will generate the mesh on the midsurface and not on the original part, you will now hide the original polygon body.

  Simulation Navigator

  •  

  •   bracket2_fem1

  •   Make Displayed Part

  •   the Information window

  Simulation Navigator

  • Polygon Geometry

  • Polygon Body (1) (hide)

8: Create a mesh collector

Create the mesh collector that will define the associated physical property table and material for the mesh.

  Mesh Collector (Properties group)

  • Element Family

    2D

  • Collector Type

    Thin Shell

  • Name

    Bracket

  •  

    Create Physical (Shell Property)

  • Name

    Bracket

  •  

    Choose material (Material 1)

  • Materials

    Steel

  • OK

     Material List dialog box

  • Default Thickness

    10 mm

  • OK

     all dialog boxes 
9: Mesh the midsurface with 2D elements

 2D Mesh (Mesh group)

  •   Drag a box around the midsurface.

  • Type

    CQUAD4

  • Element Size

    10 mm

  •  

     

  • Automatic Creation

  • Mesh Collector

    Bracket

  • Note:

    Make sure that you clear the Automatic Creation check box and select the mesh collector that you created in the previous step.

  • Apply

     

    Apply generates the new mesh and keeps the 2D Mesh dialog box active.

  • OK

     message box

  •  

  •  

    Now refine the mesh in the fillets slightly by changing to a parabolic thin shell element and experimenting with the element size.

  • the mesh

  • Type

    CQUAD8

  • Apply

     to remesh the part

     

  • The elements conform much better to the fillet radius and the hole outlines.

  • Cancel

     2D Mesh dialog box

  Save

File

  • Close→All Parts