In NX each part has 3 Reference sets (stored in the part itself).
Empty - This contains nothing
Entire Part - Contains ALL geometry of your part
Model - By default only contains 3D geometry or anything else you manually put in there
When you load a part in an assembly it will (by Default) use the Ref Set Model. So only your 3D geometry (or what you have put in there manually) will be shown in your assembly.
Easiest way to show your Datum plane in context of the assembly is to switch the Ref Set which is picked for your component. Right click on the component - Replace Reference Set and select Entire Part. Now your datum plane will be visible.
After you have placed your constraints you can switch the reference set back to Model (hiding all other geometry again).
You can also create your own Reference sets. This can come in handy when you want to hide certain geometry on Drawings or assemblies. For instance you can hide Weld preparations from your drawing by creating a second body (without the weld preparations) which you place in a Ref Set "For Drawing" (or any other name you choose). In context of the drawing you can show the component with the Ref Set "For Drawing" (only the body without weld preparations will be shown).
You can also hide components, or prevent them from loading in assemblies by setting them to Ref Set Empty in the assembly. This you do usually with components (subassembly) which have a raw material in 3D attached. The raw material will be loaded with Ref Set Empty as you don't want to see those in your assembly.
Keep in mind that Reference sets only work in context of an assembly and only one level up.