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 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.
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:
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.
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”.
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:
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.
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 …)
|