4.1.1.1 Sketch mode

Create a Model with the name Sketcher according to the naming convention.

Choose Sketch (Home -> Sketch or Sketch -> Sketch).

Define the XY-Plane as your sketch plane by clicking it and confirming by clicking OK. If you accidentally rotate your view away from your sketch plane, you can re-adjust your view by clicking View -> Orient View to Sketch.

Now choose and draw a rectangle somewhere on your sketch plane. (figure "Sketch rectangle"). Measurements are automatically created, so-called Auto Dimensions (displayed purple or grey). You should now dimension the sketch on your own and replace Auto Dimensions. Measurements you created are displayed blue.

To do so, click "Geometric Constraints" (refer figure: "Sketch bar") and choose the desired constraint, in this case ("Collinear"). Now click the  Y-Axis, a green check appears in the window Geometric Constraints (figure "Geometric Constraints"). To select objects that you want to constrain to your first selection, choose "select object to constrain to" (you can also do this by pressing CMB) and, in this case, select the right side of your rectangle. 

Subsequently, one Auto Dimension less is displayed, since you replaced it with the function (figure "Sketch").

Disabling Auto Dimensions
You can disable the function Auto Dimension by clicking Continuous Auto Dimensioning within the drop-down menu "Display Auto Dimensions" in the sketch bar. Please note, that it is automatically turned on when restarting NX.

Now you can see your sketch within the Part Navigator . Double-click on Sketch (1) "Sketch_000" to open the sketch you just created. (figure "Sketch view"). Now you can edit your sketch and change parameters for example.