Design Intent
While creating sketches, you have the opportunity to document the important relationships within the design. These relationships will govern how the part can be modified, and maintain the dimensions, tolerances, geometric tolerances, and so on. Capturing design intent starts when you create the first sketch within a part. Design intent can include:

• the design's key elements;
• how the part features are related;
• the dimensions that will be inspected or placed on a drawing (where possible, reuse the sketch dimensions to produce drawings and add additional reference-dimensions within the sketch if the engineering intent does not match the inspection or manufacturing dimensions);
• the information known about the design (since you may not have all of it, your sketch should be flexible to accommodate changes later within the design cycle);
• functionally grouped sketches (this makes them easier to create and constrain, but don't include too many or unrelated details; instead, break these details into separate sketches/features);
• how the geometry is constrained--both geometrically and dimensionally (if the distance between two mounting holes is critical, a dimension should be placed between those holes);
• geometric constraints (let's you predictably modify geometry).

The advantage to capturing the intent at this phase is, you will be thinking about and defining the relationships. It would be redundant and cumbersome to add this intelligence back into the part or drawing later in order to document the design intent that you could have already placed within the sketches.

Creating Sketches
Sketches are made up of three parts: sketch entities, geometric relationships, and sketch dimensions. These components are combined to define a sketch. The key is to put them together so they define the design's intent. Using the following order makes this process much easier.

• First, create the sketch geometry. It should be the same shape as the final geometry, but make it slightly larger or smaller than the final form. Keep the sketch close to the final size, so, when the dimensions are added, it doesn't turn your 200mm arc into a 2mm one. This will let you see how it modifies when the dimensions are placed to fully constrain the sketch. Sketches should be grouped functionally. And remember: don't put too much detail into one sketch.
• Second, add any additional geometric relationships that were not automatically added.
• Third, locate the sketch to existing or reference geometry (such as planes, axes, and the like).
• Fourth, you exercise the sketch geometry to see if the origin and geometric relationships are defined per your intent.
• Fifth, add the dimensions to size the sketch entities.

Creating the sketch in this order makes the process easier because you complete one area at a time. It can be difficult to determine what drives a sketch feature if you place dimensions without first completing geometric constraints.

Geometric Constraints
A geometric constraint lets you add spatial or orientation intelligence to a sketch entity. When creating a sketch, define the geometric constraints prior to adding any dimensional constraints. By adding the geometric constraints first, you can determine how changing the dimensions will affect the geometry. For example, when drawing a rectangle, as shown in Figure 2, geometric constraints ensure that the sides stay horizontal, and that the vertical and lower left-hand corners are coincident with the origin. When dimensions are added later, the rectangle will resize predictably.

Figure 2. Geometric constraints ensure that the sides of this rectangle stay horizontal.

While under-defined sketches can be useful early in the design process, it is good practice to fully constrain and place (locate) sketch geometry. This ensures that the sketch will modify as intended, and the dimensions can be reused during the creation of drawings. Otherwise, SolidWorks will decide how to modify the under-constrained geometry in a way you may not have intended.

The color gives a visual clue as to whether a sketch entity is under, over, or fully constrained. When the color is blue, the sketch is under-constrained; black means fully-constrained; red equals over-constrained.

SolidWorks automatically adds several constraints to the sketch based on how you draw. The example in Figure 2 shows the cursor tips that SolidWorks provides to indicate that a relationship will be created. If you do not want to create this relationship, hold down < Ctrl> or turn off Automatic Relations from the Tools>Options>Sketch dialog box.

Figure 3. The geometry in these circles is kept fully constrained with only two dimensions.

The example in Figure 3 shows the power of geometric constraints. The geometry is fully constrained with only two dimensions. The sketch follows the design intent for this sketch, which is as follows:

• It is symmetric along the centerline (Symmetric).
• The two circles are of equal diameter (Equal).
• Both circles are coincident to the sketch origin (Horizontal).

The result is a simple sketch that can be modified with only a few dimensions, offers easier drawing clean up, is fully constrained, and documents the design intent.

Exercise the Geometry
One way to ensure you have added the desired level of geometric constraints is to test them prior to adding dimensions.

To exercise a sketch, select sketch geometry and drag the entities to see how the sketch geometry modifies. The sketch geometry will alter in the under-constrained degrees of freedom. Dimensions or geometric constraints can be added to define the remaining degrees of freedom.

Dimensional Constraints
The creation and placement of dimensions determines how the part will be manufactured and inspected. The tolerances can be directly associated with the dimensions within the sketch. If the dimensions and tolerances are not created within the model, they have to be re-created in the drawing. This duplicates efforts, and the tolerances will never be visible within the model. If the dimensions required for the drawing cannot be used to define the sketch geometry, use driven dimensions to define the extra dimensions.

Adding tolerances and other 3D annotations can help define key characteristics. This is when to define a design's tolerance and geometric attributes.

Another advantage to placing the dimensions within the model is, they can be reviewed and changed without a drawing. Otherwise, if the dimensions are created and toleranced only within the drawing, the model will not document the design intent.

Conclusion
By using the methods described above, you will produce better, more robust sketches. In turn, this will lead to more robust part designs.