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)
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.
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:
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 |
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.
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.
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.
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
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.
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
|