Defining nonlinear material properties

Estimated time to complete: 10–20 minutes

In this tutorial, you will define a material property using a table field.

1: Setup

Start Simcenter 3D or NX.

File

 New

  • Model

  •  

  • Units

    Inches

  • Model

    Modeling

    Inches

  • Note:

    Make sure that you use inches as the units.

  • Name

    nl_material.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: Create part geometry and start Pre/Post

Create a five-inch-long block with a one-inch square cross section.

  Block  (Home tab→Feature group→More list)

Note:

Block is visible only when Role is set to Advanced.

  • Type

    Origin and Edge Lengths

  •   the origin of the work coordinate system (WCS)

  • Length (XC)

    1

  • Width (YC)

    5

  • Height (ZC)

    1

  • OK

     

File

  • All Applications→Pre/Post

4: Create the FEM and Simulation files

  Simulation Navigator

  •   nl_material.prt

  •   New FEM and Simulation

  • Solver

    Simcenter Nastran

  • Analysis Type

    Structural

  • OK

     New FEM and Simulation dialog box

  • Name

    Material Nonlinear

  • Solution Type

    SOL 106 Nonlinear Statics – Global Constraints

  • Case Control

  •   Edit (Nonlinear Parameters)

  • Number of Increments

    20

  • OK

     all dialog boxes

 Save

5: Define nonlinear material properties

 Manage Materials (Properties group)

  • Materials

    Steel

  •    Copy

  •     (Young’s Modulus (E))

  •  Make Formula

  •  fd(“Young’s Modulus (E)”)

  • Note:

    You will replace the formula name with a constant value.

  • Young's Modulus (E)

    26.9E6 lbf/in²

  • Note:

    Make sure that you change the units to lbf/in².

  •     (Poisson’s Ratio (NU))

  •  Make Formula

  •  fd(“Poisson’s Ratio(NU)”)

  • Poisson's Ratio (NU)

    0.3

  •  

     

  •    (Stress-Strain (H))

  •  New Field→Table

  • Independent

    Strain

  •  

  • 0,0
    Note:

    Type this value in the unlabeled box at the bottom of the group.

  •   Accept Edit

  • Type the remaining values for the table, as listed below. Use commas or spaces to separate values in a row, and use semicolons to separate rows. Click Accept Edit to add values to the table.


  • 0.0013    34970
    0.005     40000
    0.01      43750
    0.015     46250
    0.02      50000
    0.03      52500
    0.04      55000

  • OK

      Table Field dialog box

  •  

    Initial Yield Point (LIMIT1)

    34970 lbf/in²

  • Note:

    Make sure that the units are lbf/in².

  • OK

      Isotropic Material dialog box

  •  

    Materials

    Steel_1

  •   Rename

  • Name

    Strain Hardening Steel

  • Enter

     

  • Close

      Manage Materials dialog box

 Save

At this point, you could mesh the part, add constraints, add a pressure load, use subcases to control load steps, and solve the model.

File

  • Close→All Parts