Activity 2: Sketching to create round gear teeth

In this activity, you create round gear teeth inside a hollow cylinder. This requires you to:

• Sketch a smaller circle using a center point and a diameter.

• Apply a constraint and a dimension to the circle to control its size and position.

• Create a circular pattern from the original circle.

• Convert the cirlces in the circular pattern into 3D geometry.

  
  
  Completed round geer teeth inside the cylinder

Steps

1. Start sketching a circle, with a 4 mm diameter, on top of the base of the cylinder.

   1. Click Solid > Create > Create Sketch .
   2. Select the top of the base of the cylinder as the plane you want to sketch on.
      
      
   3. Click Sketch > Create > Center Diameter Circle .
   4. Click to select the center point of the circle.
      
      
   5. Drag the mouse to start creating a circle, and type 4 mm in the Diameter field.
      
      
      
      
   6. Press Enter twice to complete the circle.

2. Apply a Horizontal/Vertical constraint to the circle to align it to the center point of the face. This ensures that if the center of the face moves, the sketch moves with it.

   1. Click Sketch > Constraints > Horizontal/Vertical.
   2. Click the center point of the circle you just created, then click the center point of the face.
      
      
      
      This aligns the two points.
      
      
   3. Press Esc to finish applying the constraint.

3. Start sketching a circle, with a diameter of 25.4 mm, inside the hollow cylinder to use as the basis for the circular pattern.

   1. Click Sketch > Create > Sketch Dimension .
   2. Select the center of the circle, and then the center of the face, as the objects you want to dimension.
      
      
   3. Drag the mouse towards the right and click to place the dimension.
   4. Type 25.4 mm in the Dimension field.
      
      
   5. Press Enter.
      
      Note: The sketch 2D profile is shown in black to denote that it is fully defined; that is, it has been constrained and dimensioned.

4. Create a circular pattern of six circles from the circle you have sketched.

   1. Click Sketch > Create > Circular Pattern . This displays the Circular Pattern dialog.
   2. Click Select next to the Objects field on the Circular Pattern dialog and select the circle.
      
      
   3. Click Select next to the Center Point field and select the center point of the face.
      
      
   4. Type 6 in the Quantity field.
      
      
   5. Click OK on the Circular Pattern dialog to create the pattern.
   6. Click Sketch > Finish Sketch

5. Extrude the circles in the pattern by a distance of 6mm to convert them into 3D features.

   1. Click Modify > Press Pull. This displays the Press Pull dialog.
   2. Click Select on the Press Pull dialog and then click each circle in turn to select all six circles. Selected circles are displayed in blue.
      
      When you select a circle, the Extrude dialog is displayed.
   3. Type 6 mm in the Distance field,then Click OK on the Extrude dialog.
      
      
   4. Use the ViewCube to orient the view to display the extruded features inside the cylinder.
      
      

Activity 2 summary

In this activity, you sketched a circular pattern and converted the circles into cylinders to create round gear teeth inside a hollow cylinder. To do this, you:

• Sketched a smaller circle using a center point and a diameter.

• Applied a constraint and a dimension to the circle to control its size and position.

• Created a circular pattern of six circles from the original circle.

• Converted the cirlces in the circular pattern into 3D geometry.

  
  
  Completed round geer teeth inside the cylinder