Simulation Training
January, 2006

NX Nastran 4

SOL 601 Large Displacement/Contact Workshop

Start

  • Open the file 'plug.prt' in NX4. This file contains a simple 2 body part that resembles a snap-in plug connector. In this workshop, you will set up a large displacement nonlinear solution to simulate the assembly of the connector.
  • This workshop illustrates:
    1. Contact definition
    2. Enforced motion definition via table based field
    3. NX Nastran SOL 601 analysis setup for a large displacement (geometric nonlinear) contact analysis.

Create FEM

  • Start Advanced Simulation and open the Simulation Navigator (you may want to pin this open). Right click on the part and create a new FEM named 'plug_fem.fem'.
  • Set units to mm
  • Associate to part
  • Create idealized part
  • Use all bodies
  • Solver is NX Nastran
  • Analysis Type is Structural

Create RBE2 to control plug motion

  • Use the Line toolbar and point to point line method to create a line from 0,0,0 to 0,0,56
  • Create a mesh point at the end of the line (at 0,0,56)
  • Define a 1D mesh to create a RBE2 element from the mesh point to the highlighted face. Set the Default Element Number to 3 to get 4 grids per curve segment

Mesh plug body

  • Create a 3d mesh on the polygon body representing the plug. Hit the 'lightning bolt' to calculate a suggested element size of 3.79 mm.

·        Notice that the default settings suppress an edge in the critical contact area:

·        Use Split Face/Split Face by Suppressed Edges to restore these edges. Note that you will also need to reduce the small feature tolerance to 0% before updating the mesh. If left at the default of 10%, these 4 edges will be suppressed again when the mesh is updated.

·        Updated Mesh:

Mesh socket

  • Create a 3D mesh on the second body representing the socket. Use the suggested element length of 4.01

Define materials

  • Modify the material of both 3D meshes to the Nylon material found in the Plastics category of the material library.

Create Sim

  • Create a new Simulation file named plug_sim.sim on plug_fem.fem. Set the solution type to Advanced Nonlinear 601,106

  • Settings:

1.      Parameters

a.       Large Displacements

2.      Time Steps

a.       20 steps of 0.05 seconds

3.      Contact Parameters

a.       Continuous Segment Normals – Not Used

4.      Strategy Parameters

a.       Automatic Incrementation Scheme – ATS

b.      Maximum Iterations per Time Step – 30

c.       RBE2 Elements Option - Rigid

Define Contact

  • Create two surface to surface contact objects.
    • Coefficient of friction :0.1
    • Set 1:
      • Source: Dark blue faces on plug (4 total)
      • Target: Magenta faces on socket (5 total)
    • Set 2:
      • Source: Light blue faces on plug (4 total)
      • Target: Green faces on socket (5 total)

Define Constraints

  • Fix the base of the socket
  • Define enforced motion on the mesh point
    • Type = component
    • Tx = Ty = Rx = Ry = Rz = 0
    • Tz: Select ‘Link Existing Field on drop down menu

      • Create table based field

        • Name: Plug Motion
        • Insert independent variable
          1. Unit type: time
          2. Variable: time
          3. Units: sec
        • Insert dependent variable
          1. Unit type: length
          2. Variable: displacement
          3. Units: mm

        • Values: 0,0; 1,-21

Solve

  • Solution runs approx 12 minutes on desktop PC

Post Process

  • Set Deformed Options to 1x Results

  • Set animation to iterations

  • Select various output data in the Simulation Navigator
    • Stress, contact force, etc.

End of Workshop