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 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.
2- 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:
1- 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 froms 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:
1- 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.
2- 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.
3- 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 Assignbutton and select the right bottom point (point number 2).
Click Close button.
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.
2- 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:
1- 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
3- 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
4- 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.
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.
|