Friday, February 24, 2012

Creating a Cylinder at an Angle to a Hemisphere



This article was written as a reply to a question asked by one of my blog readers. He wanted to know how to draw a cylinder at an angle to a hemisphere as shown below.

completed exercise

So this was the reply:


  1. Create a new part file. A new sketch should open by default.
  2. In the Sketch environment, sketch a circle (say diameter 100mm). Use the center of the sketch as the center of the circle.
  3. Immediately press E to initiate the Extrude tool. Extrude to a height (say 5mm).


  1. Press S to launch the Sketch tool immediately. Click the top face of the circular base as the sketch plane. Sketch a semicircle (say of diameter 80mm). You can use the Arc tool(Center Point option).
  2. Join the endpoints of the semicircle with a line. Constrain the line to pass horizontally through the center of the sketch. If necessary, use the Trim tool to clean up the sketch.
  3. Make the line a centerline geometry. You can do this by selecting the line and clicking on the Centerline tool on the Sketch Tab> Format Panel.
  4. Press R to launch the Revolve tool immediately. Set the angle of revolution to 180 degrees. Click Ok.


Now I'm assuming that you followed my procedure. By constraining the circle that was used to create the circular base to the center of Sketch1, I ensured that the feature is entered in the graphics area. So I can reuse some of my default work planes and work axes without creating unnecessary new ones.

  1. On the Model Browser, expand the Origin folder. Right click the XZ Plane and click Visibility to make the XZ plane visible.
  2. Repeat step 1 above to make the X Axis visible.
  3. Press ] to launch the Work Plane tool. Click the XZ Plane and the X Axis (they should be visible on the graphics area). You can also select them through the Model Browser. This technique is used to create a work plane at an angle to a plane about an axis.
  4. Now set the angle of rotation to say 125 degrees. Click OK. A work plane is created (let's call it Work Plane 1).

    Now we are going to create an offset work plane parallel to Work Plane 1.

  5. Press ] to launch the Work Plane tool. Click and drag Work Plane 1 upwards above the hemisphere. Set the distance to say 50mm(Check if the distance is +ve or -ve. Also ensure that the new work plane is slightly above the hemisphere to your desired distance). Click OK. A new work plane is created. (Let's call it Work Plane 2.)
  6. Now press S to launch the Sketch tool. Select Work Plane 2 as the sketch plane to use.
  7. Create a circle of say diameter 25mm at the center of the new sketch.
  8. Press E to launch the Extrude tool. On the Extrude dialog box > Shape tab > Extents Area, set the Extents to "To Next". Click Ok. A cylinder is created from the Work Plane 2 to the hemisphere.
  9. Save file.

I hope you learnt a lot from this lesson. If you have any questions, please drop a comment, and I will answer ASAP. Thank you.