Sketcher - tips, tricks and hotkeys

• You need to hold CTRL to snap to corners or other sketch entities
• select dimension(s) and Control+T will make the dimension strong.
• Select the sketch lines and press Control+G to make them Construction.

While in the sketch command hitting the RMB has many functions that is not available directly like locking the constraints, lengths, and many more.

Parametric sketches in models or the sketch tool in drawings, symbols, and formats?

If you need to add a reference while sketching, you can press Alt + select the needed reference then continue sketching

I also noticed yesterday something. If you select multiple arcs or circles, you can right click and select equal and all the selection will have the same dimension.

You can build relations in the sketch on the fly by typing the equation in the dimension.  I use "sd1/2" often to create symmetry while being able to display both dimensions on the print.

• Be mindful of your sketcher reference plane.  Not only does it allow you to control what H & V is, Creo will frequently pick a model surface rather than one of the default datums, creating another unnecessary parent child relationship.
• Always use surfaces for references rather than edges where possible.  They are much more robust.
• Get the right number and type of entities in when sketching, don't worry about placing them where they need to go.  In fact, I deliberately put them in the wrong place to avoid Creo assuming they should be aligned with something.
• Add "sketcher_starts_in_3D no" to your config to keep the model in 3D while sketching. Makes selecting references easier, especially when trying to pick surfaces vs. edges (see previous bullet)
• Don't worry about picking sketcher references ahead of time. Sketch first, then tie things to model geometry after.  It gives you more control over the constraints and references.
• Be very deliberate about your constraints and references.  I make sure every constraint, dim and reference is exactly the one I want.  These are what determine how your sketch will react to model changes, a little diligence here will pay big dividends later when things change.
• Watch for Creo over constraining with the H & V constraints.  It often will allow a line to be coincident with a planar surface and H or V.  If that surface changes angle, the sketch fails because it can no longer be H or V.