Activity 1: Sketching to create a hollow cylinder

In this activity, you use sketches as the foundation to create a hollow cylinder. This requires you to:

Steps

  1. Start sketching a circle, which will become the base of the cylinder, on the XZ plane.

    1. Click Solid > Create > Create Sketch create icon.
    2. Select the XZ plane to sketch on.

      select plane

      When you have selected the plane, you enter the Sketch contextual tab, which contains commonly used Sketch tools. The Sketch Palette is also available, which lists options relevant to your current task or the currently selected sketch entity.
    3. Click Sketch > Create > Center Diameter Circle center diameter circle icon.
    4. Hover over the origin (or center) of the sketch. The cursor snaps automatically to this location.

      select sketch origin
    5. Click once to begin placing the circle.
    6. Drag the mouse away from the center to start sketching a circle.

      sketch circle

      Tip: Don't worry about the exact size of the circle now, we'll apply exact dimensions later in this activity.
    7. Click again to complete the circle.

      complete circle sketch
  2. Add a dimension of 62 mm to control the size of the circle, then finish the sketch.

    1. Click Sketch > Create > Sketch Dimension.
    2. Click the edge of the circle to select it.
    3. Click again to place the dimension.
    4. Type 62 mm.

      apply a dimension
    5. Press Enter.

      complete a dimension
    6. Click Sketch > Finish Sketch to finish the sketch.

      complete circle sketch

      Tip: Click Home View next to the ViewCube to view the sketch at its original size and orientation.
  3. Extrude the circle you have just created, by 8 mm, to convert its 2D sketch profile into 3D geometry.

    1. Click Modify > Press Pull. This displays the Press Pull dialog.
    2. Select the area in the middle of the circle as the profile you want to extrude. This displays the Extrude dialog.

      select a plane
    3. Drag the blue arrow upwards 8 mm to set the depth of the cylinder.

      extrude a circle

      Tip: If you can't drag the mouse to exactly 8 mm, type 8 mm in the Distance field and press Enter.
    4. Click OK on the Extrude dialog.

      extrude a circle
  4. Sketch a circle, with a diameter of 56 mm, on top of the cylinder. This circle will become the sides of the hollow cylinder.

    1. Click Solid > Create > Create Sketch create icon.
    2. Select the top of the cylinder as the plane you want to sketch on.

      select sketch plane
    3. Click Sketch > Create > Center Diameter Circle center diameter circle icon.
    4. Position the cursor over the center point of the top face to use it as the origin of the sketch.

      select sketch origin
    5. Click and start dragging the mouse to display the current diameter of the circle, then type 56 mm in the Diameter field.

      sketch a circle
    6. Press Enter.
    7. Click Sketch > Finish Sketch to finish the sketch.

      circle sketch completed
  5. Extrude the outer ring of the cylinder, by 22 mm, to convert it into 3D geometry.

    1. Click Solid > Modify > Press Pull. This displays the Press Pull dialog.
    2. Click the outer ring to select it as the 2D profile you want to extrude.

      select profile

      This displays the Extrude dialog.
    3. Drag the blue arrow upwards 22 mm to set the depth.

      extrude circle

      Tip: If you can't drag the mouse to exactly 22mm, type 22mm in the Distance field and press Enter.
    4. Click OK on the Extrude dialog.

Activity 1 summary

In this activity, you created a hollow cylinder. To do this, you: