Nastran tutorials : Static Analysis of a Gear

Create geometry to represent a gear with octagonal axis. Create a finite elements model of gear. Run static analysis of the gear.


Purpose:

Create geometry to represent a gear with octagonal axis. Create a finite elements model of gear. Run static analysis of the gear.

Description of the Model:

Determine different results of linear static analysis of a gear pinned at the ends of axis with a normal pressure on one tooth.


Procedure:

Start:


  1. Open GiD file called pieza.gid. This file is localized in the Examples folder in the GiD installation directory.

To get this file, use the Internet Retrieve option of GiD and download Nastran Examples.
Internet Retrieve option is available under:
Data ->Problem Type -> Internet Retrieve
For more information see GiD manuals.

Comment:

If you want to create the gear's CAD model manually without downloading it, see the Post-process Tutorial of GiD, which can be obtained from the GiD web page in Support section.

Preferences:


With the target to obtain a good mesh some changes in meshing preferences of GiD have to be made.

  1. Open Preferences window:


Utilities -> Preferences

  1. Select meshing tab and set window entries to the following values:

Surface mesher: Rsurf
Mesh until end
Automatic correct sizes
Unstructured size transition: 0.6
Smoothing: High Angle
No mesh frozen layers
Allow automatic structured
These settings will prevent the creation of tetrahedron elements with seek angle bigger than 80 degrees. Please note, that gear's CAD model is designed like unique volume to allow the creation of a correct finite elements model.

Assign Property:


1- Define and assign the property for the surface.
Data -> Properties -> Property
Select from the top combo boxes the property Tetrahedron .
Click on the following icon to create a new property: 
Enter name for the new property gear .
Fill all statements like in the picture:

Make sure, that a one of the default materials is defined in Composition Material.
Click on the following icon to save the new property: 
Now click on Assign button, and select the unique volume of the geometry.
To make a proof if the property is well assigned click on Draw button, select This property option.
The following image should display the chosen property. :


Assign Constraints:

1- Assign prescribed displacements and rotation.
Data-> Boundary Conditions -> Constraints
Click on the following icon to set the condition over surfaces:

The model has the two lids of octagonal axis pinned, which means that all degrees of freedom have to be prescribed.
To do this it is necessary to check all statements.
2- Select the two lids of octagonal cylinder (axis of the gear).


Assign Static Loads


Assign Normal distributed pressure over one tooth of the gear.
Data -> Loads -> Static Loads
Click on the following icon to set the condition over surfaces:

From the top combo box static load select Normal-Surface-Load.
Set the value of the load to 2e4 (positive sign means that
load is oriented inward to the surface) and select the three interior surfaces of one tooth of the gear, as stated in the following image:


Perform the Analysis:


Design Executive Control Section.
Data -> Problem Data -> Executive Control
Select the NASTRAN Type that will be used for the analysis .
Check STATICS and leave all the other statements uncheck or with default values.
Click on Accept Data button.
2 - Design Case Control Section.
Data -> Problem Data -> Case Control
2.1. - Input data
In this example we don't consider the acceleration due to the gravity. Leave all statements with default values.
2.2. - Output data
Set Title to "Gear_example"
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, constraints forces, elements forces and elements stresses, uncheck the rest of output requests.
    In Output Design section leave the default values.
    Note: The output device has to set to PUNCH for post-processing with MI/NASTRAN Interface.
    Click on Accept Data button.

    Obtain Input File for NASTRAN Code:


    Option 1:


    Calculate -> Calculate

    Option 2:


    File -> Import/Export -> Write Calculation File
    In the Save File window, select the filename and location. Please note, it is very important to use the appropriate NASTRAN file extension.

    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
    Select the *. pch file located in NASTRAN results folder.
    After the 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
    Select the *.neu file located in NASTRAN results folder.
    After the 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.

    Results visualization:

    Open View results window.
    Windows -> View Results

    Contour Fill

    In View results window:
    Set View to Contour Fill .
    Set Results to total translation
    Set Component to total translation modulus.
    Click on Apply button.

    Contour Fill

    Total Translation


    Display Vectors

    In View results window:
    Set View to Display Vectors .
    Set Results to total spc forces
    Set Component to total spc forces modulus.
    Click on Apply button.

    Display Vectors

    total spc forces


    Of course there are more results and more possible visualizations, user is invited to explore all possibilities of GiD.