Procedure:

Start:

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

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

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:

1-     Create a line.

Geometry -> Create -> Line

Insert coordinates of points to the command line to define the beam (line). Command line is in the bottom of GiD master window.

1st point        -> 0,0

     2nd point        -> 30,0

     3rd point        -> 60,0

     4th point        -> 120,0

    

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

Press escape or middle button of mouse.

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.

Assign properties and material:

1-     Define a new material.

Data -> Materials

Click on the following icon to create a new material:

Enter a name for the new material 'alum'.

Fill all statements as in the following picture:

And set density, in Others page, to 0.101

Click on the following icon to save the new material:

2- Define and assign properties for the beam.

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 property beam from the top combo box.

Click on the following icon to create the new property:

Enter a name for the new property 'cantilever'.

Fill all statements as 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 the Assign button, and select all lines 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:

1- Assign prescribed displacements and rotation.

Data-> Boundary Conditions -> Constraints

Click on the following icon to set the conditions 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

Connections

1-     Disconnect degree of freedom from point B.

Data -> Boundary Conditions -> Connections

         Checks disconnect Z-Rotation statement.

         Click on the Assign button and select point B.

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

Assign Static Loads

1-     Assign static punctual loads.

Data -> Loads -> Static Loads

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

Point A

Select the static load Moment from the top combo box.

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

    

         Click on the Assign button and select point A.

Point B

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

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

    

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

                   Coordinate System = BASIC

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

Click on the 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, set the value to 6.

Click on the OK button

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

Num. of linear elements = 20

Num. of nodes = 21

Perform the Analysis:

1-     Design Executive Control Section.

Data -> Problem Data -> Executive Control

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

Check STATICS and leave all the other statements uncheck.

Leave the rest of statements with the default values.

Click on the 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”

 

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 constraint forces and uncheck the rest of output requests.

                   In the Output Design section leave the default values.

Note: If you want 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.

Obtain Input File for NASTRAN Code:

Option 1:

Calculate -> Calculate

Option 2:

File -> Export-> Write Calculation File

Select a folder and a 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 …).