Create geometry to represent a flat rectangular plate. Create a finite elements model of plate. Use a dynamic frequency dependent load Write an input file for MI/NASTRAN to run dynamic analysis in direct formulation. Use post-processing tools to analysis results.
|
Purpose:
Create geometry to represent a flat rectangular plate.
Create a finite elements model of plate.
Use a dynamic frequency dependent load
Write an input file for MI/NASTRAN to run dynamic analysis in direct formulation.
Use post-processing tools to analysis results.
Description of Model:
Determine the frequency response of a 5x2 inch flat plate under frequency-varying excitation by using the direct formulation.
A unit load at a corner of the tip will excite the plate model.
A frequency step of 20Hz will be used for this analysis within the range of 20 and 100Hz.
Structural dumping will be set to 0,06.
Properties:
Length |
5 inch |
Weight |
2 inch |
Thickness |
0.1 inch |
Mass Density |
0.282 lbs/inch3 |
Young's Modulus |
30.0e+6 lbs/inch2 |
Poisson's Ratio |
0.3 |
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 contour lines of the plate.
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 -> 5,0
Third point -> 5,2
Fourth point -> 0,2
Fifth point -> 0,0
(Only it is necessary introduce points using two coordinates, the third coordinate Z is assume to 0 ).
Now you are asked if you want to join the first point and
the fifth point , select Join
Press escape or middle button of mouse.
- Create surface.
Geometry -> Create -> NURBS Surface -> By contour
Or a more quick option is click on the following icon:
Situated in right vertical tool bar.
Now the pointer of mouse change to this form
It means that now is possible select the four lines created before to create the surface.
Select the four lines in the screen.
Press escape or middle button of mouse.
Now in the NASTRAN Interface program window has to be geometry like this:
|
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
mat_1
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 the following icon
and select option "property" in the menu.
Select from the top combo box the property membrane
.
Click on the following icon to create a new property:
Enter name for the new property
property_1
.
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, choose Surfaces and
select the surface 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:
|
Assign Constraints:
- Assign prescribed displacements and rotation.
Data-> Boundary Conditions -> Constraints
Click on the following icon to set the condition over lines:
Uncheck Z-Rotation and leave all other statements check.
Now click on Assign
button and select the vertical line on the left side (line number 4).
Note: It is possible label geometry entities using this option:
-Press right button mouse to get the contextual menu.
-Select option Label and choose All.
Assign Dynamic Load
- Define the table of interpolation values associate to dynamic load.
Data -> Loads -> Tables
Click on the following icon to create a new table:
Enter name for the new table
freq_var
.
Data Entry
- Check Single Value
- X= 0.0 and Y= 1.0
- Click on Add button
- X=1000 and Y= 1.0
- Click on Add button
- Click on the following icon to save the new table:
- Click on Close button.
- Assign dynamic load.
Data -> Loads -> Dynamics Loads
Click on the following icon to set the condition over points:
Select from the top combo box dynamic load Freq Dynamic Type1
.
Fill all statements like in the picture:
|
Look that for Table Interpolation Values D[f] has value Table. Table
is the default value for this statement an is equal to a blank table, it means that D[f] is equal to zero function.
Now click on Assign button and select the right bottom point (point number 2).
Click Close
button.
Mesh the Geometry:
1-Create a structured mesh.
Meshing -> Structured -> Surfaces
Select the surface of the geometry.
Press escape or middle button mouse.
Now you are asked for number of cells to assign to lines, set to 10.
Click OK
button.
Select lines 1 and 3, the large ones.
Press escape or middle button mouse.
Now you are asked again for number of cells to assign to lines, set to 4.
Click OK
button.
Select lines 2 and 4, the short ones.
Press escape or middle button mouse.
Click Cancel
button.
- Generate the structured mesh.
Meshing -> Generate
Now you are asked about the size of elements to be generate, leave default value (0.54)
Click OK
button
Appears a window with information about the mesh:
|
Num. of Quadrilateral elements = 40
Num. of nodes = 55
Click 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.
Now in the NASTRAN Interface program window has to be an 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 STATICS and DIRECT FREQUENCY RESPONSE and leave all the other statements uncheck.
Leave the rest of statements with the default values.
Click 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
"Direct_frequency _Response"
Leave Subtitle, Label … and Post process with default values.
Check Displacements and Velocity, and 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 Accept data
button
- Design Dynamic Analysis.
Data -> Problem Data -> Dynamics
Set these values to the different statements:
Solution Method = Direct
Domain of Solution = Frequency
Overall Structural Damping Coeff. = 0.06
Frequency Step
Initial step = 20
Frequency Increment = 20
Number of frequency increments = 49
Mass formulation = Coupled
Click 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 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 the name.
Post process:
Click on the following icon to enter in the post process:
Import punch file:
- 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 one of the results displacements or velocity.
|
|
Contour Fill Z-Displacement Step 20Hz |
|
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 one of the results displacements or velocity.
Use trackball rotation to rotate the plate and see better the deformation.
Numerical results:
To see numerical results in nodes, click on this icon
and select in which nodes you want to see the current numerical results display in the screen.
For example:
Node 51 step 200Hz
Displacements
X= 1.28075e-19 |
Y= -4.89892e-20 |
Z= -0.00547175 |
Dis. |
=0.0547175 |
---|
Velocity
X= -1.23013e-19 |
Y= -5.22769e-19 |
Z= 0.467011 |
Vel. |
= 0.467011 |
---|
Create an Animation:
- Select which kind of results will be displayed
- Open Animation Window.
Windows -> Animate
- Click Play button.