SolidWorks Intro Part 4
- Start a new part with an extruded base on the front plane.
- Draw a rectangle.
- Dimension the width to 1.5 inches.
- Go to View -> Hide/Show and turn on Dimension Names.
- Dimension the height to 2/3 the width by typing the equation:
= [click on dimension D1] * (2/3)
- Change the width to 2 inches and watch the height change.
- Exit the sketch and set the extrude depth to 1/8 inch.
- Make a #4 screw hole near the left edge of the part.
- Right click on Equations in the Feature Manager Tree and select Manage Equations.
- Explore the four view buttons:
- Equation view
- Sketch equation view
- Dimension view
- Ordering view
- Define a global variable "Num Holes" and set it to 3.
Controlling a Linear Pattern:
- Suppose we want our holes to be evenly spaced across the part.
- Dimension the hole's distance from the left edge to be:
= [dimension D1] / [Global variable "Num Holes"] / 2
- Create a linear pattern feature to replicate the hole. Set
the number to 2 and the spacing to 1 inch.
- Go into the equation manager and select the Dimension view.
- Change the linear pattern parameters to "Num Holes" and make
the spacing equal to the part width divided by "Num Holes".
- 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.