Analyzing a portion of a model using breakout modeling

Estimated time to complete: 10–20 minutes

In this tutorial, you will use the breakout modeling technique. First, you will analyze the overall structure using a coarse mesh, and solve for displacements. Next, you will create a smaller breakout model that uses a finer mesh. You will then map the displacement results from the overall model to the cut faces of the breakout model. Finally, you will solve the breakout model and evaluate stresses.

1: Setup

You will open a finite element model of the entire wheel, solve it, and then isolate one of the spokes for a more refined analysis.

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

  2. Click the link below:

    Download the part

  3. Extract the part files to your breakout folder.

  4. Start Simcenter 3D or NX.

  5. Open wheel_breakout_sim1.sim.

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: Solve the model

  Simulation Navigator

  •   Solution 1

  •   Solve

  • OK

     

  • Wait until the solve is complete.

  • No

     Review Results dialog box

  •   the Information window

  • Cancel

     Analysis Job Monitor dialog box

4: Display the displacement results

  Simulation Navigator

  •     Solution 1→Results

  •   Structural

 

Post Processing Navigator

  •     Solution 1→Structural→Displacement - Nodal

  •   Magnitude

  •  

  Return to Home (Context group)

5: Open the spoke FEM file

File

  Open

  • File name

    spoke_fem1.fem

  • OK

     

 

Note:

The mesh of the spoke is much finer than the mesh used to model the entire wheel.

6: Create a Simulation file for the spoke

Simulation Navigator

  •  

  •   spoke_fem1

  •   New Simulation

  • Name

    spoke_sim1.sim

  • Folder

    your part file folder name

  • OK

     New Part File dialog box

  • OK

     New Simulation dialog box

  •  

    Name

    Breakout Solution

  • Solver

    Simcenter Nastran

  • Analysis Type

    Structural

  • Solution Type

    SOL 101 Linear Statics – Global Constraints

  •  Element Iterative Solver

  • OK

     Solution dialog box

  Save

7: Export displacements to a table field

  Post Processing Navigator

  •    Solution 1→Structural→Displacement - Nodal

  •  Magnitude

 

Results

Edit Post View (Post View group)

  • Deformation

  • Deformation

  • OK

     

 

  Top (Top Border bar→Orient View list)

Identify Results (Tools group)

  • Nodal Results

    Pick from Model

  • Pick

    Box (All)

  • Drag a selection box around the spoke.

  •  

    Create Field (Identify dialog box)

  • Name

    Spoke Displacements

  • Independent Domain

    Cartesian

  • Dependent Domain

    Cartesian

  • OK

     Create Table Field dialog box

  • Close

     Identify dialog box

 

  Return to Model (Context group)

  Simulation Navigator

  •    Fields

  • Notice the Spoke Displacements field is listed.

8: Create an enforced displacement constraint

You will apply enforced displacements to the faces of the spoke where the spoke was split from the wheel. The software calculates the enforced displacements by interpolating the nodal displacements from the model of the entire wheel that you previously exported.

Home

  Enforced Displacement Constraint (Loads and Conditions group→ Constraint Type list)

  • Type

    Translational Components - Field

  • Type Filter (Top Border bar)

    Polygon Face

  •  

  •  

     

  • Magnitude

    Field

  • Specify Field

      Select Existing Field from List

  • Fields

    Spoke Displacements

  • OK

     all dialog boxes

  •  

9: Solve the spoke model

  Simulation Navigator

  •   Breakout Solution

  •   Solve

  • OK

     

  • Wait until the solution is complete.

  • No

     Review Results dialog box

  •   the Information window

  • Cancel

     Analysis Job Monitor dialog box

10: Display the results

  Simulation Navigator

  •     Breakout Solution→Results

  •   Structural

 

Post Processing Navigator

  •     spoke_sim1→Breakout Solution→Structural→Displacement - Nodal

  •   Magnitude

  •  

 

  Edit Postview (Post View group)

  • Display

  •  

  • Edges

    Feature

  • OK

     

  •  

 

Post Processing Navigator

  •   spoke_sim1→Breakout Solution→Structural→Stress - Element-Nodal

  •     Von-Mises

     

The calculated stress on boundaries where the enforced displacements are applied is sensitive to the interpolated displacements. To help avoid viewing aberrant stresses on these boundaries, create a contour plot with a layer of elements removed along these boundaries. To do this, create a group that includes all the elements on these boundaries. You can then exclude the group from the contour plot.

For this activity, the group Elements_on_Boundary has already been created for you.

 

  Post Processing Navigator

  •   Contour Plots→Post View 3→Groups

      Elements_on_Boundary

      Hide

 

  Save

File

  • Close→All Parts