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  -> 30,0

    Third point     -> 60,0

    Fourth point   -> 120,0

   

(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 this icon

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, and select all lines of the geometry.

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:

Assign Constraints:

1- Assign prescribed displacements and rotation.

Data-> Boundary Conditions -> Constraints

Click on the following icon to set the condition over points:

Assign the following prescribed movements:

X-Displ

Y-Displ

Z-Displ

X-Rot

Y-Rot

Z-Rot

Point A

1

1

1

1

1

0

Point C

0

1

1

1

1

0

Point D

0

1

1

1

1

0

Define Local Axes

1-    Assign Local Axes.

Data -> Properties -> Local Axes

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

Select all lines of the geometry.

Connections

1-    Disconnect degree of freedom from point B.

Data -> Boundary Conditions -> Connections

Checks disconnect Z-Rotation statement.

Click on Assign button and select point B.

With this condition it is possible disconnect some degrees of freedom of the union points of some beams. In this case this condition creates a 2-D rotule in XY-plane.

Assign Static Loads

1-    Assign static punctual loads.

Data -> Loads -> Static Loads

Click on the following icon to set the condition over points:

Point A

Select from the top combo box static load Moment.

    (Mx-Force, My-Force, Mz-Force) = (0,0, -60)

   

    Click on Assign button and select point A.

Point B

Select from the top combo box static load Point-Force-Load.

    (X-Force, Y-Force, Z-Force) = (0, -20, 0)

   

    Click on Assign button and select point B.

2- Assign static distributed loads.

Data -> Loads -> Static Loads

Click on the following icon to set the condition over lines:

        Line from C to D

Select from the top combo box static load Line-Pressure-Load.

            Coord. System = BASIC

(X-Pressure, Y-Pressure, Z-Pressure)= (0, -40, 0)

Click on Assign button and select the line C to D.

Mesh the Geometry:

1-Create a mesh.

Meshing -> Generate

Now you are asked about the size of elements to be generated, change to value 6.

Click on OK button

Appears a window with information about the mesh:

Num. of linear elements = 20

Num. of nodes = 21

Perform the Analysis:

1-    Design Executive Control Section.

Data -> Problem Data -> Executive Control

Select type of NASTRAN will be use in the analysis.

Check STATICS 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  “Beam_example”

 

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

Check Displacements and constraint forces 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.

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