Assuming you're using 'master model', then you need to either change the reference set from Solid, to say Entire Part, or create a uniques reference set containing the geometry you want to display in the drawing file.
Using the master model principal (seperate model and drawing files) In the model, click Format > Reference Set then when the menu appears, click the white sheet (new) to create a new refernce set. Give it a name like drafting for example, then click the + button and select the geometry you want to add to the drafting reference set and OK.
Then in the drawing right on the model in the assembly navigator, select ref set, then under the choice which pops up, select the reference set you created (drafting) and you geometry will now be displayed on the drawing (provided you have added a view that is!)
Another alternative would just be to sketch the ink print in drafting, if you're not actually using it in modeling. But that will depend on the version of NX you're running...and that wasn't specified.
You can in later versions sketch on to the drawing, but I'd remind you that this is not master model based. So whatever detail you're adding at that level isn't part of the model definition. Sometimes it is just a part of the division of labour between modellers and drafters, but occasionally certain seemingly trivial things in design when not visible in the context of your assemblies for review processes could mean that there are unintended consequences. If the feature you're adding should not be hidden or perhaps in contact with another part in the design then you probably do want to define it as part of the model.
Sometimes I can't be bothered with things that dissapear and re-appear based on a complex web of settings and reference sets, and require specific file formats for export (ie, iges instead of parasolid).
If its a simple enough closed outline, use divide face to imprint it in the surfaces. Now its a permanent part of the 3d geometry.
