Tip #1: Keep It Simple
The best advice for anyone who has trouble in Sketcher: keep the sketch simple. Don’t try to make a single sketch that encompasses the entire model shape with all cuts and rounded edges. Instead, try to focus on creating multiple sketches that are simple and include fewer entities. When you make design changes, fewer entities are easier to control. Take this muffler model as an example:
The first solid geometry for this model started as this:
Followed by this:
And 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. This can make things a lot simpler.
Tip #2: Internal or External Sketches?
You can create both internal or external sketches in Creo.
An internal sketch is created internal to the feature that generates the resulting 3D geometry. For example, you can create a sketch that’s internal to an Extrude feature. The Extrude feature extrudes the 2D sketch geometry normal to the sketch plane. Internal sketches are only to be used by the feature they are internal to. While there are many benefits to internal sketches, a major benefit 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.
An external sketch is 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. Then, you are able to use that sketch for a Revolve feature later in the design process. A major benefit of external sketches is that you can use the same sketch for multiple features. For example, you could use an external sketch for an Extrude feature, and then use it again later for a different Extrude feature that cuts material away.
Tip #3: Know Your Design Intent
You’re constantly thinking to the future of the model and how it might have to change if design specifications change while you’re creating your sketches. This way of thinking helps you decide on the best way to specify your sketch’s design intent – which 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 various ways – no way is incorrect. However, you still have to determine the best design intent to use for your sketch so that it will update the way you want when modified.
Tip #4: No Weak Dimensions
When you are sketching geometry, the intent manager actively tries to help you capture design intent by enabling you to snap geometry vertically, horizontally, equal length, parallel, etc. Whenever you stop sketching, the intent manager automatically places light blue dimensions called weak dimensions, to maintain a fully dimensioned and constrained sketch at all times. You can choose whether you want to use these dimensions or not, depending on the design intent you want to capture. While adding your own dimensions and/or constraints, the intent manager removes the weak dimensions to maintain that fully dimensioned, constrained sketch.
You might reach a point where you have captured the design intent you desired, but few weak dimensions remain. Instead of leaving these dimensions weak, either continue adding additional dimensions/constraints to eliminate the weak dimensions, or convert the weak dimensions to strong dimensions.
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. Take full control of your design by converting all weak dimensions to strong dimensions.
Tip #5: “Flex” the Sketch
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 could assume 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. Maybe you think the angled lines on both sides of the sketch will move in equally the same amount? If you look again you’ll see the 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 want 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.