The sketch tools within SolidWorks® are very similar to those in other CAD and Parametric programs: line, circle, rectangle, polygon, slot, arc, etc. (Figure 2.10). Each command also has drop down options to allow you to have more control over how you specify a geometric element in a sketch. There are yet even more customizing options for each sketch tool in the property manager for that sketch tool.

As soon as you activate a sketch tool by left clicking on it from the CommandManager, the property manager for that sketch tool opens, usually with a set of illustrative directions for how to use the sketch tool.

These tools are going to be the most straightforward tools because they work the same across all platforms (for the most part). However, as you add sketch geometry to a sketch, often times sketch relations will be automatically added to the origin and the entities you are adding. We will discuss these more later in this chapter and how to use them but for now just be aware that you will see them appear on your sketch as green tiny boxes.

Design Intent in Sketching

SolidWorks called the Sketch tools “Sketch” for a reason: the intention behind parametric design is to do a rough sketch of what you want first, and then constrain it using dimensional (Smart Dimension) and geometric (Relations) constraints. This will allow you to model way faster than if you tried to get all the details right as you sketched. Sketching this way also ensures that you are modeling based on design intent, not putting any unnecessary constraints on the geometry that are not needed for the design to function. An example is shown below in figures 2.11, 2.12, and 2.13.

You will notice that the sketch in figure 2.11, 12, and 13 started out as blue and then, constraints were added, it turned black. When features/entities are blue in the sketch environment, they are under-defined. When features/entities are black in the sketch environment, they are fully defined. These states are known as sketch geometry status’.

When a sketch is fully defined, all the appropriate design criteria needed to manufacture the feature(s) has been specified by the designer. When a sketch is under defined, this means that there is not enough information, not enough design criteria specified in the sketch environment to manufacture the features drawn.

Look at Figure 2.11 again: without the dimensions on the geometry to specify the intended size and location for the drawing, how would manufacturing know what the design intent was for the part? Without the symmetry constraint on the two circles between the vertical center line, how would manufacturing know where one hole is supposed to be with respect to the rest of the part? Yes, the information is in the model, but there is variation in manufacturing processes no matter what process it is, so what do we compare the manufactured parts to if there is no design information in the model? Therefore, it is critical to make sketches fully defined before sending them downstream in the product design process.

Fully define all your sketches!

Line

When you activate a tool, such as the line tool, you specify the location of the base point with a left click and then the size and orientation with the second left click; to exit the line command, simply right click and select “Select” or click the green check mark (Figure 2.14). Many sketch creation tools have expanded options. The line command has a midpoint option where you can specify the midpoint of the line on your first mouse click as opposed to the first endpoint.

 

 

Rectangle and Circle

The rectangle tool also allows you to either specify rectangles using two corners, the center of the rectangle, or 3 corner points. Below is an example of using the center point of the rectangle as the base point:

The property managers of all the sketch creation tools have many options and instructions on how to use each option. All sketch tools allow you to convert the sketch entities into construction geometry (also known as reference geometry). The rectangle tool specifically has different options for how the construction lines that help constrain the rectangle are placed: at the corners or at the midpoints (Figure 2.16).

In Figure 2.16, you can see that in the rectangle type icons, there are number 1, 2, 3. These indicate the order in which you left click to specify those points indicated in the icons.

ARcs, Slots, Polygons and Ellipses

The other sketch commands work in a very similar fashion as the line and rectangle commands. It is important to practice each sketch command, study each property manager for each sketch command, and try different variations of using the sketch commands to build proficiency in them.

Fillet and Chamfer

Entity based sketch tools such as fillet and chamfer allow you to quickly add complex but common sketch entities by modifying sketch entities you have already created. For example, if you’ve already drawn a rectangle using the rectangle tool, you can activate the sketch fillet tool, specify a size in the property manager, then click the corners you want to add fillets to (Figure 2.19).