Procedure:

Start:

1-     Open GiD file called staticgear.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

2-     Select meshing tab and set window entries to the following values:

Surface mesher: Rsurf

Mesh until end: Activated

Automatic correct sizes: Activated

Unstructured size transition: 0.6

Smoothing: High Angle

No mesh frozen layers: Activated

Allow automatic structured: Disable

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 element model.

Assign Properties:

1- Define and assign the properties 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 the Assign button, and select the unique volume of the geometry.

To see if the property is well assigned click on Draw button, select This property option.

The NASTRAN Interface program window should look like this:

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 you want to use for the analysis.

Check STATICS and leave all the other statements uncheck.

Leave the rest of statements with the default values.

Click on the 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: If you want to post process the results of MI/NASTRAN analysis with NASTRAN Interface, you have to set the output device to PUNCH.

 

Click on the Accept Data button.

Mesh the Geometry:

1-Create a mesh.

Meshing -> Generate

Now you are asked about the size of elements to be generated, set the value to 18.

Click on the OK button

The following mesh information window appears when the mesh is created:

Num. of Tetrahedra elements = 45100

Num. of nodes = 13728

Obtain Input File for NASTRAN Code:

Option 1:

Calculate -> Calculate

Option 2:

File -> Import/Export -> Write Calculation File

Select a folder and a file name to write the file. It is very important to write the correct extension of the NASTRAN input file (i.e. *.nas, *.dat, *.nid …).