Create geometry to represent a beam with double T section. Create a finite elements model of beam. Run modal analysis of the beam.
|
Purpose:
Create geometry to represent a beam with double T section.
Create a finite elements model of beam.
Run modal analysis of the beam.
Description of Model:
Determine the first three modes of a beam whit double T section, using Givens method for eigenvalues extraction.
Properties:
Length |
100 inch |
Weight (Section) |
2 inch |
Width (Section) |
1 inch |
Thickness (Section) |
0.1 inch |
I1 |
0.229 inch4 |
I2 |
0.017 inch4 |
Procedure:
Start:
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
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)
Create geometry:
-
- 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 -> 100,0
(Only it is necessary introduce points using two coordinates, the third coordinate Z is assume to 0 ).
Press escape or middle button of mouse.
Assign property 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 picture:
|
And set density, in Others page, to 0.101
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 the following icon
and 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:
|
You have to select the previously created material in Composition Material.
Click on the following icon to save the new property:
Now click on Assign button, select the line.
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:
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:
- Refer section properties like Inertia modulus or thickness and height to this system.
- Some of the loads (that have the prefix Local ) are related also to this system.
- 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:
- 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.
- 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.
- 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.
- 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 Local Axes.
Data -> Properties -> Local Axes
Set statement Local Axes to Automatic (An automatic local will defined for all lines selected).
Select the line of the geometry.
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 OK button
Appears a window with information about the mesh:
|
Num. of linear elements = 10
Num. of nodes = 11
Click on 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.
Now in the NASTRAN Interface program window has to be an image like this:
|
Node 1
Check the following items:
X-Displacement
Y-Displacement
Z-Displacement
X-Rotation
Y-Rotation
Uncheck Z-Rotation.
Node 11
Check the following items:
Y-Displacement
Z-Displacement
X-Rotation
Y-Rotation
Uncheck X-Displacement and Z-Rotation.
Rest of nodes
(except node 1 and node 11)
Check the following items:
Z-Displacement
X-Rotation
Y-Rotation
Uncheck
X-Displacement
Y-Displacement
Z-Rotation.
To make a proof if the constraints are well assigned click on Draw
button, select "Colors"
option.
Now in the NASTRAN Interface program window has to be a image like this:
|
|
Perform the Analysis:
- Design Executive Control Section.
Data -> Problem Data -> Executive Control
Select type of NASTRAN will be use in the analysis.
Check MODES 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
"Modes_Analysis"
Leave Subtitle, Label … and Post process with default values.
Check Displacements 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.
3- 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 Accept data
button
- Set PARAM values.
Data -> Problem Data -> PARAM
In MI/NASTRAN tab set WTMASS to 0.00259
Leave the rest of statements with default values.
Click on Accept data
button.
Obtain Input File for NASTRAN Code:
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
Post process:
Click on the following icon to enter in the post process:
Import punch file:
1- Import the punch file (***.pch) obtained from NASTRAN.
File -> Import -> Import PUNCH
Appears a window to select the punch file located in NASTRAN results folder.
After importing process is finished close the window.
Import FEMAP ASCII neutral file:
- Import the FEMAP ASCII file (***.neu) obtained from NE/NASTRAN.
File -> Import -> FEMAP file
Appears a window to select the *.neu file located in NASTRAN results folder.
After importing process is finished close the window.
Note: To obtain a FEMAP ASCII file in NE/NASTRAN go to NASTRAN editor:
Setup -> Default Analysis Options
Selects RSLTFILETYPE and set to FEMAP ASCII in Output Control Directives
Visualization of results:
- Contour Fill.
View results -> Contour Fill
Select "Displacements"
|
|
Contour Fill Y-Displacement mode 22665.1 |
|
To change step of analysis use this menu sequence:
View results -> Default Analysis/Step -> 1
Select that step you want to see.
- Deformation.
View results -> Deformation
Select displacements.
|
|
Deformation mode 1.84e6 |
|
Numerical results:
To see numerical results in nodes, click on the following icon
Select in which nodes you want to see the current numerical results display in the screen.
Create an Animation:
- Select which kind of results will be displayed
- Open Animation Window.
Windows -> Animate
- Click on Play button.
Modes of beam
It is necessary edit the results file ***.F06 located in results folder of NASTRAN.
Here are the results with (MI/NASTRAN):
Modes no. |
EIGENVALUE |
CYCLIC FREQUENCY |
1 |
2.266509E+04 |
2.396066E+01 |
2 |
3.627142E+05 |
9.585227E+01 |
3 |
1.837810E+06 |
2.157598E+02 |