Activity 2: Create the shovel surfaces

In this activity, you create all the surfaces you need for the shovel, from the sketches. You

• Extrude the circle to create the shaft

• Revolve the line and arc near the shaft to create the shovel face

• Extend the shovel face to create the final shovel shape.

  

  Shovel sketches with handle (left), and shovel surfaces (right)

Prerequisites

• Activity 1 is complete.

Steps

1. Extrude the circular sketch toward, and as far as, the curved part of the handle, to create the shaft.

   1. Click (Design workspace > Surface tab > Create panel > Extrude) to open the Extrude dialog.
   2. In the canvas, click the sketch point at the center of the circle, to select it as the Profile.
   3. In the Extrude dialog, set the Extent to To Object.
   4. In the canvas, select the rounded part of the handle as the Object.
      
      
   5. Click OK to accept the tool and close the dialog.

2. Use the sketch profile near the shaft, and the Y-axis as the Revolve axis, to create the main body of the shovel.

   1. Click (Design workspace > Surface tab > Create panel > Revolve) to open the Revolve dialog.
   2. In the canvas, select the line and arc near the shaft as the Profile.
   3. In the Browser, click next to Origin, to show all the planes and axes.
   4. In the Revolve dialog, click Select associated with Axis to activate it, then click the green Y-axis in the canvas.
      
      
   5. Click OK to accept the tool and close the dialog.

3. Extend the front edges of the revolved section of the shovel body by 150 mm using the Tangent Extend Type, to create the tapering section.

   1. Click (Design workspace > Surface tab > Modify panel > Extend) to open the Extend dialog.
   2. In the canvas, select one front edge, then press `Ctrl` (Windows) or `Command` (MacOS), and select the second front edge.

      Notice that the first edge extends, and then retracts when you press `Ctrl` (Windows) or `Command` (MacOS). Then both edges extend when you select the second edge.

      
      
      
   3. In the Extend dialog, confirm the Extend Type is set to Tangent, and the Distance is 150 mm.
   4. Click OK to accept the tool and close the dialog.

Activity 2 summary

In this activity, you created all the surfaces you need for the shovel, using the sketches. You

• Extruded the circle to create the shaft
• Revolved the line and arc near the shaft to create the shovel face
• Extended the shovel face to create the final shovel shape.