Modal Analysis

 

The example model is 3D hexahedron model. This example creates mesh seed based on Hex8 contains eight nodes and meshed by CHEXA element with Number of element option. Material property set like as aluminum. It shows that when apply the DMAP command to the file generated from PATRAN

 

Figure 1  Target model

 

1.  To create MSC/NASTRAN, run Patran and create new database

 

     New database.

    Specify the working directory and file name.

 

Figure 2  New Database

 

1.  Create new geometric model

 

     Move to Geometric entity

     Geometric setting

    Action: Create, Object: Solid, Method: XYZ.

    Ref. Coordinate Frame: Coord0

    Vector Coordinates Lists: <1 1 1>

 

     Create

    After set the above items, click Apply. You can get the new model.

 

Figure 3  Creation of model

 

2.  Create Mesh seed on the model

 

     Move to Elements

     Mesh seed setting

    Action: Create, Object: Mesh seed, Type: Uniform.

    Number of Elements: 5.

    Curve list: Select all curves by dragging window

 

     Create

This method divides selected curves into Number of Element. It does not mean mesh. You can use another option that is Element Length to mesh seed.

 

Figure 4  Mesh Seed

 

3.  Mesh based on mesh seed

 

     Mesh options

    Action: Create, Object: Mesh, Type: Solid

    Mesher: IsoMesh

    Element Topology: Hex8

    Solid list: Solid1

 

     Mesh

Element Topology means a kind of elements that has different node number in the element and solid list means geometric entity that performed mesh seed. After select model, click Apply.

 

You can get the result windows.

Figure 5  Mesh

 

4.  Input Material properties

 

     Move to Material

     Material options

    Action: Create, Object: Isotropic, Method: Manual Input,

 

     Input material

    Elastic Modulus: 70e9

    Possion Ratio: 0.33

    Density: 2710

 

Figure 6  Material property

 

5.  Input element property

 

     Move to Property

     Element property options

    Action: Create, Object: 3D, Type: Solid.

    Property set name: cubic.

 

     Input Element properties

    Click Alumin and OK. (Alumin is material property that created in above step.)

    Select Members and Add. (Member is a set of created elements)

 

Figure 7  Element property

 

6.  Perform analysis to export MSC/NASTRAN Input file

 

     Move to analysis

     Analysis options

    Action: Analyze, Object: Entire Model, Method: Analysis Deck

    Enter the jobname

    After set the above options, select Solution Type

 

     Solution Type: Normal Modes

 

Figure 8  Export

 

7.  Edit exported file (jobname.bdf)

     Refer DMAP command editing in 2.2.2 MSC/NASTRAN Interface.

 

8.  Run MSC/NASTRAN

 

     Run MSC/NASTRAN with exported file

    Select Nastran Input file and open.

    Run

    You can get the punch file. (Jobname.pch).

    Punch file contains mass and stiffness matrix, mode vector and frequency.

 

Figure 9  Analysis with MSC/NASTRAN

 

Note

When you generate RecurDyn/Flex Input File (*.rfi) from Output file, you cannot include Stiffness matrix in option.