5 Secrets to Mastering Sketches in Your CAD Software

Guest post from PTC University’s Matt Huybrecht and Katelyn Stevens

Are you frustrated that you can never seem to create a sketch quickly? Do you have trouble with sketches that fail? Does your model fail to update the way you think it should when you modify a dimension? If you answered yes to any of these questions, then follow the five hints below to create a robust sketch.

Tip #1: Keep It Simple!

The best advice for anyone who has trouble in Sketcher is to keep the sketch simple. Don't try and make a single sketch that encompasses the entire model shape with all cuts and rounded or chamfered edges. Rather, create multiple sketches that are simple, with fewer entities. Fewer entities are easier to control when you start making design changes. Take this muffler model, for example:

The first solid geometry for this model started as this:

Followed by this:

Then this:

Simple sketches of few entities were created, and the solid geometry started to take shape. The sketches should consist of small bites of geometry, not the whole shape at once.

Tip #2: Internal or External Sketches?

In Creo, you can create both internal and external sketches. Internal sketches are created internal to the feature that generates the resulting 3D geometry. For example, you can create a sketch that is internal to an Extrude feature. The Extrude feature extrudes the 2D sketch geometry normal to the sketch plane. Internal sketches can only be used by the feature they are internal to. The benefit of internal sketches is that you always know exactly where the Sketch feature is located in the model tree, and the new result is that there are fewer features in the model tree, resulting in a more compact model tree. In this figure, each Extrude feature was created with its own internal sketch.

External sketches are created external to the feature that generates the resulting 3D geometry. For example, you could create a Sketch feature as feature #5 in the model tree. You could then use that sketch for a Revolve feature much later in the design process. The benefit of an external sketch is that you can use the same sketch for multiple features. For example, you could use an external sketch for both an Extrude feature and then later on for a different Extrude feature that cuts material away. This figure shows an example of an external sketch called SKETCH_CRANK that was used a bit later on for feature Extrude 1.

Tip #3: Know Your Design Intent

As you create your sketches, you must constantly be thinking to the future of the model and how it might have to change if design specifications change. Thinking this way helps you determine the best way to specify your sketch’s design intent. Design intent is the method you choose to create, constrain, and dimension a sketch that causes it to update predictably if modified. The same sketch can be dimensioned and constrained in many different ways. No particular way may be incorrect, but you have to determine what is the best design intent to use for your sketch so that it will update the way you want if modified. In the following figures, the same sketch is dimensioned and constrained in three completely different ways. The geometry is identical, but the sketch will behave very differently if dimensions are modified.

Tip #4: Leave No Weak Dimensions

When you sketch geometry, the intent manager actively tries to help you capture your design intent by helping you snap geometry vertically, horizontally, equal length, parallel, and so on. When you stop sketching, the intent manager automatically places light blue dimensions called weak dimensions to maintain a fully dimensioned, fully constrained sketch at all times. You may choose to use these dimensions or not based on the design intent you wish to capture. As you add your own dimensions or constraints, the intent manager removes the weak dimensions to maintain that fully dimensioned, fully constrained sketch.

You may reach a point where you have captured the design intent you want for the sketch, but a weak dimension or two remains. DO NOT leave these dimensions as weak. Rather, either continue adding additional dimensions or constraints to eliminate the weak dimensions, or convert the weak dimensions to strong dimensions. In the figures below, the intent manager creates the light blue weak dimensions once you stop sketching geometry. As you capture your desired design intent, the weak dimensions are removed. Do not be tempted to leave weak dimensions. Take full control of your design by converting all weak dimensions to strong dimensions.

Tip #5: “Flex” the Sketch

Did you know you can actually test your sketch to see how it behaves when dimension changes are made to it? In the following figure, how do you think the sketch will behave if the 400 dimension is increased or decreased?

If the 400 dimension is decreased to 300, you might think that the entire sketch slides to the right with respect to the vertical reference. But if you look again you will notice the Symmetry constraint applied to the top, horizontal line endpoints. Perhaps you think the angled lines on both sides of the sketch will move in equally the same amount? But if you look again you will see that right endpoint is constrained to remain at a distance of 200 from the vertical reference. The way to verify this is to use the Modify option, located in the Editing group of the Sketcher ribbon. Then select the dimension you wish to modify.

You can then use the slider in the Modify Dimensions dialog box to dynamically increase or decrease the value, as shown here, to see how the sketch actually behaves.

If your desired design intent is such that the angled lines on both sides of the sketch move in and out equally, then you must apply the Symmetry constraint to the line endpoints and remove the lower 200 dimension.

If the same 400 dimension is added to the Modify Dimensions dialog box, the sketch now behaves as desired.

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