SolidWorks Intro Part 3

Dave Touretzky


  1. Start a new part.
  2. Create an Extruded Base on the front plane.
  3. Sketch a rectangle extending from the origin.
  4. Dimension the rectangle to be 1 inch high and 1.5 inches wide.
  5. Add a vertical centerline through the midpoints.
  6. Add a horizontal centerline as well.

    Making curves

  7. Select the spline tool
  8. Start a curve by clicking somewhere in the left half of the rectangle, near the top.
  9. Put the second point below and to the left of the first one; double click to end the curve, or hit escape to exit the curve tool.
    • If not selected, click on the curve to select it.
  10. Play with the control points:
    • The diamond changes the angle of the curve but not the length.
    • The arrowhead changes the length but not the angle.
    • The dot changes both length and angle.
  11. Snap the two endpoints to the vertical centerline.
  12. Adjust the control points to make half a heart shape.
  13. Click on the Mirror Entities tool and mirror the curve to make a heart.

  14. Click on Exit Sketch and set the extrusion depth to 1/8 inch.

  15. Add a 0.25 inch radius fillet to the corners of the piece.
  16. Save your file as HeartTile.SLDPRT

    Making puzzle connectors with trim

  17. Edit the sketch again, and go to a Normal View.
  18. Draw a small circle centered slightly outside the right edge of the rectangle, centered on the edge midpoint.
    • To do this, select the circle tool, put the mouse on the right edge (which makes the midpoint visible)
    • Slide it up until you reach the midpoint, then move slightly to the right.
  19. Draw a horizontal centerline connecting the circle to the right edge.
  20. Dimension the circle diameter to 0.2 inches (radius 0.1 inches).
  21. Dimension the centerline to 0.07 inches.
  22. Draw another small circle centered slightly INSIDE the left edge of the rectangle, on its midpoint.
  23. Select the circle, then shift-click to select the other circle.
  24. Add an Equal relation between the two circles.
  25. Draw a horizontal centerline connecting the new circle to the left edge.
    • Note: this will overlap the existing mid-point centerline.
  26. Click on the centerline, then right click and do "Select Other" to get the short one.
  27. Shift-click on the other horizontal centerline.
  28. Add an Equal relation between the two centerlines.
    • Notice that the sketch contains crossed lines (intersecting contours).
  29. Click on Exit Sketch and you'll get an error because of intersecting contours.
  30. Go back in and edit the sketch.
  31. Click on the Trim Entities tool.
  32. Click and drag across the line segments you want to delete, so no lines cross.
  33. Use control-Z to undo if you make a mistake.
  34. Now you have a puzzle piece
  35. Edit the sketch again.
  36. Change the arc radius to 0.3 inches.
    • Notice that both arcs changed at once.
  37. Then change the arc radius back to 0.1 inches.
    • Notice that the centerline endpoints are no longer aligned with the edge.
  38. Click on a centerline endpoint, then shift-click on the edge.
  39. Add a Coincident relation between them.
  40. Do the same for the other centerline endpoint.
  41. Now try resizing the arcs and note that the endpoints stay fixed.
  42. Repeat the same process to add top and bottom connectors to the puzzle piece.

    Assembly of Pieces

  43. Make a new assembly and insert four heart tiles.
  44. Color two of them red and two yellow.
  45. Mate them together as if they were puzzle pieces.
  46. Save your assembly as HeartMosaic.SLDPRT


Three ways to make a hole:

  • Closed contour in a sketch to be extruded.
  • Extruded cut.
  • The Hole Wizard:

Why you should use the hole wizard:

  • Correct sizing for standard fasteners (ANSI or metric).
  • Adjustable fit tolerances.
  • Proper symbology for machinist drawings.

Hole Wizard Example:

  1. Start with your HeartPiece part.
  2. Click on Hole Wizard in the Features tab.
  3. Click on "Hole" (third entry in the grid of hole types).
  4. Select "ANSI inch".
  5. Select "Screw clearance".
  6. Change the clearance type from "Normal" to "Close".
  7. Click on the "Positions" tab at the top of the dialog box.
  8. Click on the face of the part.
  9. Notice the mouse pointer changes to a point tool. Click to place a point, indicating a hole location.
  10. Click again to place another point.
  11. Click on the green checkmark to complete the hole dialog.
  12. To edit whole positions, open the "Clearance Hole" feature in the Feature Manager tree and edit the first sketch, which specifies the hole positions.
  13. The second sketch describes the shape of the hole; don't edit that.