Procedure:

Start:

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

2- Load problem type Nastran by following the menu sequence:

Data -> Problem type -> Nastran -> nastran

A splash image appears and the name of the master window changes to NASTRAN Interface.

Create geometry:

Create line.

Geometry -> Create -> Line

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

        

         First point     -> 0, 0

         Second point -> 100, 0

        

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

Press escape or middle button of mouse.

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 alum.

Fill all statements like in the following picture:

        

And set density, in Others page, to 0.101

Click on the following icon to save the new material:

Define and assign the properties for the surface.

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 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 following 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  select the line 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:

Define Local Axes

The model has been created related to a global axes system XYZ that is unique for the entire problem. But every beam must have its own local axes system X'Y'Z' in order to:

1.      Refer section properties like Inertia modulus or thickness and height to this system.

2.      Some of the loads (that have the prefix Local) are related also to this system.

3.      Strength results over the beam are referred to this local axes system.

The main property of this system is that the local X' axe must have the same direction than the beam.

 


The ways for defining local axes systems are:

1.     Default. The program assigns a different local axes system to every beam with the following criteria:

·         X' axe has the direction of the beam.

·         If X' axe has the same direction than global Z axe, Y' axe has the same direction than global X. If not, Y' axe is calculated so as to be horizontal (orthogonal to X' and Z).

·         Z' axe is the cross product of X' axe and Y' axe. It will try to point to the same sense than global Z (dot product of Z and Z' axes will be positive or zero).

Note: The intuitive idea is that vertical beams have the Y' axe in the direction of global X. All the other beams have the Y' axe horizontal and with the Z' axe pointing up.

2.     Automatic. Similar to the previous one but the local axes system is assigned automatically to the beam by GiD. The final orientation can be checked with the Draw Local Axes option in the GiD Conditions window.

3.     Automatic alt. Similar to the previous one but an alternative proposal of local axes is given. Typically, User should assign Automatic local axes and check them, after assigning, with the Draw local axes option. If a different local axes system is desired, normally rotated 90 degrees from the first one, then it is only necessary to assign again the same condition to the entities with the Automatic alt option selected.

4.     User defined. User can created different named local axes systems with the GiD command:

Data->Local axes->Define

and with the different methods that can be chosen there. The names of the defined local axes will be added to the menu where Local axes are chosen.

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 the OK button

Appears a window with information about the mesh created:

Num. of linear elements = 10

Num. of nodes = 11

Click on the 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:  

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.

The NASTRAN Interface program window should look like this:

Node

X-Disp.

Y-Disp.

Z-Disp.

X-Rot.

Y-Rot.

Z-Rot.

1

1

1

1

1

1

0

2-10

0

0

1

1

1

0

11

0

1

1

1

1

0

To see if the constraints are well assigned click on Draw button, select Colors option.

The NASTRAN Interface program window should look 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 MODES 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 “Modes_Analysis”

 

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

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.

Check Displacements uncheck the rest of output requests.

In Output Design section leave the default values.

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

 

Click on the Accept data button.

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 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 …)