SolidWorks Express | February 2001

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How to create sketches with Design Intent in mind

Level:	Intermediate
ID#:	10220512
Category:	Modeling, Sketch, Best Practice, Tech Tip
Products/Version :	SolidWorks 2006
Last revised:	10/22/05

Capturing design intent starts when you create the first sketch within a part. These sketches are the building blocks for your models. What happens in this stage of design will determine how intelligent, flexible, and robust your design will become. It is this stage in which careful thought should be given as to the design intent for the sketch.

Sketch Feature

The following factors should be considered when creating a sketch:

What information is known about the design? Often, you may not have all the information and your sketch should be flexible to accommodate change later within the design cycle.
What features are important to the overall design?
What features are interrelated?
What dimensions are to be inspected or placed on a drawing? Where possible use these dimensions to produce the sketch and re-use the sketch dimensions to produce the drawings.
Dimensions should either be created for reuse on the drawing or define a geometric construction method for the sketch geometry.

Sketches are made up of three parts; sketch entities, geometric relationships, and sketch dimensions. All three parts are combined to define a sketch. The key is to combine all three components to define the intent of the design. To make this process easier, use the following order when creating a sketch:

Draw the sketch geometry
Fully define any sketch relations
Add the dimensions that complete the fully defined sketch definition

Creating the sketch in this order makes creating a sketch easier due to the fact that one area is being completed at a time. If you place dimensions and then sketch relations, it can be difficult to determine what drives a sketch feature.

Create and test the geometric relations prior to adding the dimensions. By exercising the sketch, you can determine whether the geometry is created in a manner that is consistent with the designer's intent. To exercise a sketch, select sketch geometry and drag entities and see how the sketch geometry modifies. The sketch geometry will alter in the under-constrained degrees of freedom. Dimensions or additional geometric constraints can be added to define the remaining degrees of freedom.

While under-defined sketches can be useful early on in the design process, it is a good practice to fully constrain and place sketch geometry. This insures that the sketch will modify as intended. The color gives a visual as to the level of constraint:

Blue = Under-Constrained

Black = Fully-Constrained

Red = Over-Constrained

Use of Construction Geometry
Construction geometry can be an effective sketch tool. Use of construction geometry within a sketch can document design intent, reduce the number of dimensions required, minimize drawing cleanup, and make feature modification more predicable. Creating a sketch using extra dimensions to define the design is harder to modify and makes drawing cleanup more difficult.

Sketch Example Using Construction Geometry

Dimensioning
Dimensioning is one of the most important communication tools at your disposal. The creation and placement of dimensions determine how the part will be manufactured and inspected. The tolerances can be associated directly to the dimensions within the sketch. If the dimensions and tolerances are not created within the model, they have to be re-created within the drawing. This can be duplicate effort and then 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, for example, surface finish and geometric tolerances, can help define the key design characteristics. This is the best time to define the tolerance and geometric attributes for a design. The best time to think about and determine design intent is while the model is being created, not as an afterthought while the drawing is being finished.

One advantage to placing the dimensions within the model is that they can be reviewed and changed without a drawing. Otherwise, if the dimensions are created and tolerance only within the drawing, the model will not document the design intent. Since the tolerances and dimensions will be created, why not place them inside the model and display the dimensions in the drawing.

Sketch Tolerances and Model Annotations

Manufacturing or a tool vendor can use the full tolerance model earlier within the design phase. They do not have to wait for complete drawings to produce prototype parts and still understand the tolerances and key dimensions associated with the design.

The method used to insert dimensions can produce different results. This is not always evident due to existing geometric relationships. The example shown produces the same dimension and modifies the geometry in the same manner. This is due to the fact that Horizontal and Vertical relationships exist for the sketch lines. The first controls the length of the line, the second controls the distance between the two points, and the third controls the distance between the bottom line and the point. If there were no geometric relations, modifying the dimensions would produce different results.

Line Secleted

2 Points Selected

Line and Point Selected

Derived Sketches
A derived sketch can be used to copy existing sketch geometry. This allows one sketch to drive a number of identical part features. Using a derived sketch ties the features together. The new sketch is dependent on the parent sketch. Any changes to the parent sketch are shown in the derived sketch.

Original Sketch

Derived Sketch

If the original (parent) sketch is deleted, the derived sketches are also deleted. To break the relationship, select the sketch within the FeatureManager, press the right mouse button, and select Underive.

Sketches can be copied to a new location, by holding down the Ctrl key and dragging. This differs from a derived sketch in that the new feature is not tied to the original. A sketch can also be moved to a new location by selecting the sketch and dragging. Moving the feature will not violate geometric constraints that may be in place.

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