How to create better sketches

Sketching skills are vital to the creation of flexible, robust designs. The following are a number of sketch tips that can be applied to create and better control sketches. The intelligence and flexibility built into your sketches will be well served throughout the design cycle. Inflexible sketches that do not impart the design intent can become a major problem late in the design cycle.

Example Sketch

Double Sketch Entities
When selecting an object and it appears thinner, this is indication that a problem may exist. An example would be two entities on top of one another, or three entities with a common end. This illustration shows how a double line will appear when selected. A single line appears with a solid highlight, and the double line is only half-highlighted.

Sketch Inferencing
When creating a sketch, there are times when you do not want to use the automatically created inference relationships. SolidWorks offers visual clues when these relationships are about to be created. For example, you may not want a horizontal relationship added even thought the sketch entity is horizontal, or more common is a coincident relation to an unwanted object.

To override the creation of these relationships, hold the Ctrl key down while creating the sketch entity. When the Ctrl key is held down, the inference no longer displays in the graphics area.

Cursor with Inference	Cursor without Inference (Ctrl)

Fully Defined Sketches
When creating sketch entities, SolidWorks gives the user visual clues as to state (Under, Fully, or Over Defined) of the entity. When creating a sketch, a fully defined sketch will insure the sketch behaves as desired. An under-defined sketch may not change in the intended manner.

Blue = Under-constrained or under-dimensioned sketch entity. This means the sketch entity does not have sufficient geometric (relations) or dimensional constraints to fully define the position and location of the object.

Under Defined Sketch Entity

Black = Fully constrained and dimensioned sketch entity. This means the sketch entity has sufficient geometric (relations) or dimensional constraints to fully define the position and location of the object.

Fully Defined Sketch Entity

Red = Over-constrained or dimensioned sketch entity. This means there are geometric (relations) or dimensional constraints that define the sketch feature more than one way. This creates a conflict and the user will be warned that the sketch is over-defined. The sketch should not be left in an over-defined state. Additional dimensional references can be made driven.

Over Defined Sketch Entity

Modify Dialog
The sketch can be used to modify the geometry without rolling back the feature. Double-clicking directly on the feature or sketch will display the Modify dialog box. The Rebuild button can be used to try different combinations without leaving the Modify dialog box.

When modifying a part within an assembly, the same method can be used to modify a part without going to Edit Part mode. The dimension value can be changed and after the Rebuild button is pressed the feature changes.

Modify Dialog Box

Using Sketch Relationships
Relationships can be used to define design intent. These relationships can reduce the dimensions required to fully constrain the sketch. The second sketch shown can be fully constrained with one dimension. This was done using an Equal relationship.

By adding the type of geometric relationships that are not automatically inserted (i.e., Equal, Parallel, Symmetric, Intersection, etc.) the design intent for the sketch can be defined clearly. Otherwise, the sketch will require many unnecessary dimensions that would also be displayed on the drawing, making drawing cleanup more difficult.

before	after

Defining the Sketch Origin
The sketch geometry should be defined and constrained to the appropriate model geometry. The origin of the sketch can be used as a means to tie the sketch geometry. By defining an origin for the sketch geometry, the sketch can be easily moved or re-oriented.

Sketch Origin not Constrained	Sketch Origin Constrained

Input Dimension Value
The option Input Dimension Value can be set to prompt the user for a dimension value as soon as the dimension is inserted. This can save selections because otherwise, the dimension is inserted and then the user would have to double-click on the dimension to change the value. It can be more efficient to input the value as the dimension is placed.

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