Sketch hide features????

You can use section view (view toolbar) You can hide bodies (go to the solid bodies folder) You can pick features from the tree and change colors to make them transparent, then remove the colors later. You can go work in wireframe You can change the color of part to make it somewhat or mostly transparent.

Those are the ones I use, sort of in order that I use them (I don't like working in wireframe... tooo slow)

-Ed

In addition to Ed's fine list here are a couple more things. Some are technique and some are settings.

Settings

1. In Tools/Sketch Settings turn off automatic relations.
2. In Tools/Options/Sketch turn off infer from model

Technique

1. Create your sketch off to the side and when you have it working the way you want attach it to the model with appropriate relations.
2. Don't work quite normal to the sketch plane so you can pick and choose underlying geometry when necessary.

Here's an additional tip for whether the part you are editing is open by itself or within an assembly:

Use the display of a section view (View/Display/Section View) to slice the component(s) in a plane position and direction which will provide a clear view "underneath" the visually obscuring solid features.

This, for example, makes it possible to more easily select an interior face on which to sketch and allows for cursor selection of any visible geometry (other than entities in the virtual section plane) for use in the sketch.

It's even possible to reposition and/or rotate the section view plane while the sketch in progress is kept active! Creating a keyboard shortcut key assignment is quite helpful for toggling the section view ON/OFF.

This I f> In addition to Ed's fine list here are a couple more things. Some are

That's what I was looking for. Thank you

Monty