Procedure:

Start:

1- Open a new project by clicking on the following icon in taskbar

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

Data -> Problem type -> Nastran(version number) -> nastran

If the problem type is correctly load a splash image appears and the name of the master window changes to GiD-NASTRAN Interface.

In case this thing doesn't happen, problem type is not correct installed.

Create geometry:

Create contour lines of the plate.

Geometry -> Create -> Line

Insert coordinates of points to the command line to define the plate (surface). It is important to follow the correct order of points.

POINT

X Coord.

Y Coord.

First point

0.0

0.0

Second point

5.0

0.0

Third point

5.0

2.0

Fourth point

0.0

2.0

Fifth point

0.0

0.0

        

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

Now you are asked if you want to join the first point and

the fifth point , select Join

Press escape or middle button of mouse.

Create surface.

Geometry -> Create -> NURBS Surface -> By contour

For faster surface creation click on the following icon:

Situated in the left vertical tool bar.

When the mouse pointer changes to  
, select the previously created lines to create the surface.

Press escape or middle button of mouse.

The NASTRAN Interface program window should look like this:

Assign properties and material:

Define a new material.

Data -> Materials

Click on the following icon to create a new material:

Enter name for the new material mat_1

Fill all statements like in the picture:

        

And set density, in Others page, to 0.282

Click on the following icon to save the new material:

Define and assign the properties for the plate.

Data -> Properties -> Property

You can go directly to the property window by clicking on this icon:   
without closing the material window and going back to the menu.

Select from the top combo box the property membrane.

Click on the following icon to create a new property:

Enter name for the new property property_1.

Fill all statements like in the picture:

You have to select the previously created material in Composition Material.

Click on the following icon to save the new property:

Now click on the Assign button, and the surface of the geometry.

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

The NASTRAN Interface program window should look like this:

Assign Constraints:

Assign prescribed displacements and rotation.

Data-> Boundary Conditions -> Constraints

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

Uncheck Z-Rotation and leave all other statements check.

Now click on Assign button and select the vertical line on the left side (line number 4).

Note: It is possible label geometry entities using this option:

-Press right button mouse to get the contextual menu.

-Select option Label and choose All.

Assign Dynamic Load

Define the table of interpolation values associate to dynamic load.

Data -> Loads -> Tables

Click on the following icon to create a new table:

Enter name for the new table freq_var.

Data Entry

Check Single Value

X= 0.0 and Y= 1.0

Click on Add button

X=1000 and Y= 1.0

Click on Add button

Click on the following icon to save the new table:

Click on Close button.

Assign dynamic load.

Data -> Loads -> Dynamics Loads

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

Select from the top combo box dynamic load Freq Dynamic Type1.

Fill all statements like in the picture:

Look that for Table Interpolation Values D[f] has value Table. Table is the default value for this statement is equal to a blank table, it means that D[f] is equal to zero function.

Click on the Assignbutton and select the right bottom point (point number 2).

Click on the Close button.

Mesh the Geometry:

1-Create a structured mesh.

Meshing -> Structured -> Surfaces

Select the surface of the geometry.

Press escape or middle button mouse.

Now you are asked for number of cells to assign to lines, set to 10.

Click the OK button and select lines 1 and 3, the large ones.

Press escape or middle button mouse.

Now you are asked again for number of cells to assign to lines, set to 4.

Click OK button and select lines 2 and 4, the short ones.

Press escape or middle button mouse.

Click on the Cancel button.

Generate the structured mesh.

Meshing -> Generate

Now you are asked about the size of elements to be generate, leave default value (0.54)

Click on the OK button

The following mesh information window appears when the mesh is created.

Num. of Quadrilateral elements = 40

Num. of nodes = 55

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.

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

Perform the Analysis:

Design Executive Control Section.

Data -> Problem Data -> Executive Control

Select type of NASTRAN you want to use for the analysis.

Check DIRECT FREQUENCY RESPONSE and leave all the other statements uncheck.

Leave the rest of statements with the default values.

Click on the Accept data button.

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 “Direct_frequency _Response”

 

Select which format file you want to use:

         - Small: Every file of a Bulk Data statement will use the 8-       characters definition.

         - Large: Every file of a Bulk Data statement will use the 16-     characters definition.

 

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

Check Displacements and Velocity, and uncheck the rest of output requests.

In Output Design section leave the default values.

Note: If the user wants to post process the results of MI/NASTRAN analysis with NASTRAN Interface, you have to set the output device to PUNCH.

 

Click on the Accept data button

Design Dynamic Analysis.

Data -> Problem Data -> Dynamics

Set these values to the different statements:

Solution Method = Direct

Domain of Solution = Frequency

Overall Structural Damping Coeff. = 0.06

Frequency Step

                   Initial step = 20

                   Frequency Increment = 20

                   Number of frequency increments = 49

Mass formulation = Coupled

Click on the Accept data button

Set Parameters values.

Data -> Problem Data -> Parameters

In Geometry tab set WTMASS to 0.00259

Leave the rest of statements with default values.

Click on the Accept data button.

Obtain Input File for NASTRAN Code:

File -> Import/Export -> Write Calculation File

Select a folder and file name to write the file. It is very important to write the correct extension of the NASTRAN input file (i.e. *nas, *.dat, *.nid …)