SolidWorks Intro Part 4

Dave Touretzky


  1. Start a new part with an extruded base on the front plane.
  2. Draw a rectangle.
  3. Dimension the width to 1.5 inches.
  4. Go to View -> Hide/Show and turn on Dimension Names.
  5. Dimension the height to 2/3 the width by typing the equation:
    = [click on dimension D1] * (2/3)
  6. Change the width to 2 inches and watch the height change.
  7. Exit the sketch and set the extrude depth to 1/8 inch.
  8. Make a #4 screw hole near the left edge of the part.

    Equation Manager:

  9. Right click on Equations in the Feature Manager Tree and select Manage Equations.
  10. Explore the four view buttons:
    • Equation view
    • Sketch equation view
    • Dimension view
    • Ordering view
  11. Define a global variable "Num Holes" and set it to 3.

    Controlling a Linear Pattern:

  12. Suppose we want our holes to be evenly spaced across the part.
  13. Dimension the hole's distance from the left edge to be:
    = [dimension D1] / [Global variable "Num Holes"] / 2
  14. Create a linear pattern feature to replicate the hole. Set the number to 2 and the spacing to 1 inch.
  15. Go into the equation manager and select the Dimension view.
  16. Change the linear pattern parameters to "Num Holes" and make the spacing equal to the part width divided by "Num Holes".
  17. Change Num Holes from 3 to 4 and observe the effect.

Making Basic 3D Shapes

  • Method 1: Extruded base on an existing face of a part.

  • Method 2: Revolved base of a cross section. Sculpture example.

  • Many additional techniques: loft, shell, bend, etc.

  • Save the 3D part or assembly as an STL file, then import into your next tool.