Procedure:

Start:

1- Open a new project, right click on this icon in taskbar

2- Load problem type Nastran. Follow the menu sequence below:

Data -> Problem type -> Nastran -> nastran

Appears a splash image and the name of the master window changes to NASTRAN Interface.

3- Change the view plane to XY:

View -> Rotate -> Plane XY (original)

Create geometry:

1-    Create line.

Geometry -> Create -> Line

Now insert in command line the coordinates of points to define the plate. Follow the order is very important.

   

    First point      -> 0,0

    Second point  -> 100,0

   

(Only it is necessary introduce points using two coordinates, the third coordinate Z is assume to 0 ).

Press escape or middle button of mouse.

Assign property and material:

1-    Define a new material.

Data -> Materials

Click on the following icon to create a new material:

Enter name for the new material alum.

Fill all statements like in the picture:

   

Click on the following icon to save the new material:

2-Define and assign the property for the surface.

Data -> Properties -> Property

If you don't close material window is possible get the property window clicking on the following icon  

and select option “property” in the menu.

Select from the top combo boxes the property “beam”.

Click on the following icon to create a new property:

Enter name for the new property cantilever.

Fill all statements like in the picture:

Look that in Composition Material there is selected the material created before.

Click on the following icon to save the new property:

Now click on Assign button, select the line.

To make a proof if the property is well assigned click on                 Draw button, select This property option.

Now in the NASTRAN Interface program window has to be an image like this:

Define Local Axes

2-    Assign Local Axes.

Data -> Properties -> Local Axes

Set statement Local Axes to Automatic (An automatic local will defined for all lines selected).

Select the line of the geometry.

Mesh the Geometry:

1-Create a mesh.

Meshing -> Generate

Now you are asked about the size of elements to be generate, leave default value (10)

Click on OK button

Appears a window with information about the mesh:

Num. of linear elements = 10

Num. of nodes = 11

Click on OK button.

Note: It is possible label mesh elements and nodes using this option:

-Press right button mouse to get the contextual menu.

-Select option “Label” and choose “All”.

Assign Constraints:

1- Assign prescribed displacements and rotation.

Data-> Boundary Conditions -> Constraints

Click on the following icon:  

To set the condition over points or nodes.

Show the labels of nodes using this option:

-Press right button mouse to get the contextual menu.

-Select option “Label” and choose “All in” and choose points.

Now in the NASTRAN Interface program window has to be an image like this:

 

 

Node 1

Check the following items:

X-Displacement

Y-Displacement

Z-Displacement

X-Rotation

Y-Rotation

Uncheck Z-Rotation.

Node 11

Check the following items:

Y-Displacement

Z-Displacement

X-Rotation

Y-Rotation

Uncheck X-Displacement and Z-Rotation.

Rest of nodes  (except node 1 and node 11)

Check the following items:

Z-Displacement

X-Rotation

Y-Rotation

Uncheck

X-Displacement

Y-Displacement

Z-Rotation.

To make a proof if the constraints are well assigned click on                 Draw button, select “Colors” option.

Now in the NASTRAN Interface program window has to be a image like this:

Perform the Analysis:

1-    Design Executive Control Section.

Data -> Problem Data -> Executive Control

Select type of NASTRAN will be use in the analysis.

Check MODES and leave all the other statements uncheck.

Leave the rest of statements with the default values.

Click on Accept data button.

2 - Design Case Control Section.

Data -> Problem Data -> Case Control

2.1.- Input data

        Leave all statements with default values.

2.2.- Output data

        Set Title to  “Modes_Analysis”

 

         Leave Subtitle, Label … and Post process with default values.

Check Displacements uncheck the rest of output requests.

In Output Design section leave the default values.

Note: If the user wants to post processing the results of the analysis with MI/NASTRAN Interface is mandatory that the output device has to set to PUNCH.

 

Click on Accept data button.

 3- Design Modes Extraction.

Data -> Problem Data -> Dynamics

In modes analysis tab:

Set the following values to the different statements:

    -Method of eigenvalues extraction = GIV.

    -First Frequency = 0.0

-Last Frequency = 350.0

    -Desired number = 3

    -Check Mass orthogonality test option.

    -Leave the default values for the rest of statements.

In Dynamic Design tab:

Set Mass formulation = Coupled

Click on Accept data button

4-    Set PARAM values.

Data -> Problem Data -> PARAM

In MI/NASTRAN tab set WTMASS to 0.00259

Leave the rest of statements with default values.

Click on Accept data button.

Obtain Input File for NASTRAN Code:

File -> Import/Export -> Write Calculation File

Appears a window to select in which folder and the name for save the file. It is very important write extension of the file in