Sorry, I forgot to mention that starting NX 11.0.1 you can set the default scope in sketcher to within active sketch only using a customer default. It is suddenly there, like we read your mind... Isn't that scary?
You can find it in Sketch/General/Session Settings/Use 'Within Active Sketch Only' Selection Scope.
Normally I would advise you to stick to the defaults we ship. The sketch customer defaults are mainly intended to keep older workflows working.
In this case I say: "Try it! "
Just found this after some googling, great to see this default available!
My reason for wanting this is for consistent behaviour. With shipped defaults, I was getting annoyed with NX continually changing the selection scope i.e. I would select "within active sketch" when dragging objects, then if I started a curve command this would remain, but starting dimensions or constraints would change it back to "within work part". It was all very microsoft word style behaviour.
I think it doesn't really matter what a default is, as long as it doesn't change on it's own when I change command. This will keep us older engineers working!
A way to "keep the sketch simple" is to NOT trim it to the boundary.
I find that a good way to create simple sketches is to visualize the basic shapes (Rectangles, Circles, Polygons) that make up a sketch, similar to how you would look at a solid and visualize what features you will use to create it.
Sketch the shapes using the appropriate shapes - don't just assume that you should sketch the outer boundary using Profile and then figure out how to constrain it. Using basic shapes, especially rectangles, automatically brings in appropriate inferred constraints, such as using perpendicular constraints in the corners of the rectangles. As mentioned earlier, these are preferred, because it will allow you to rotate the rectangle shape.
Then, resist the urge to use Quick Trim. Although it works very well, what can happen is that whenever you delete a piece out of the middle of any line or shape, NX must add constraints to make up for the missing geometry. This adds a lot of invisible complexity to the sketch. And then when you delete more things, your constraints can become complex and no longer intuitive.
The trick to NOT trimming is to use the Curve Rule of Region Boundary Curves when you use the sketch to Extrude or Revolve.
Here is an example, to create this model.
To sketch the boundary, would require a lot of constraining.
To sketch it using mostly centered rectangles, all the constraints for colinear, perpendicular, and symmetry are automatically inferred.
If you try to trim away the unnecessary centers of the rectangles, you will lose some of the midpoint constraints enforcing symmetry, and will need to add these constraints back using symmetry constraints. In most cases, NX will add the required constraints, but in a case like deleting the middle of a line supporting a midpoint constaint, you must manually re-constrain the sketch another way.
Trim makes the sketch look simpler, but in actuality is making it more complex by requiring more geometric constraints.
The trick is to design the sketch, planning to use Region Boundary Curves to select the regions.
When you create a sketch, and then before finishing the sketch, immediately click Extrude, Region Boundary Curves is used as the default.
Great tip Mark,
When you create an internal sketch from within extrude or revolve, region boundary curves is used as default, and it seems to be extremely good at selecting regions without any user input. Here I've just recreated your sketch but without changing curves to reference, and it worked fine.