While I was writing my question, I kept fiddling around and found a way. So I'll describe it to you. If you know of another simpler way, don't hesitate to take it back from me. If you can't find it, it will serve as a tutorial.
Preamble: Here's how I use drawings for an assembly. In the first sheet of a drawing, I place an assembly, and then describe the parts that make it up on the following sheets. A sheet for each piece. I don't do a drawing by rooms.
I want the name of the exposed room to be automatically displayed at the top on each sheet, so you need to create a background plan template with the file name wherever you want it.
The type $prpmodel and $prpview properties only work if the model is already in the sheet, so it is not necessary in the background.
So you have to go through the $PRPSHEET and then change the drawing to which the sheet properties refer.
So when creating each sheet, import the template (you won't find it in the list if you don't import it to your sheet first), and then right-click on the sheet in question in the featureManager creation tree, properties, and there, at the bottom, Select the template you just imported from "Use custom property values for the template shown in:". The name of your object appears at this time.
It doesn't seem like a very clean way of doing things to me, but it works.
Personally, I don't see much other method. At the very least, to limit the risk of error in the selection of the property donor view, you can make one mep per room and then group the meps by simple drag and drop.
Another solution that allows you to use the Type $PRPVIEW variables is to create annotations in the drawing template (e.g. Ref:$PRPVIEW:REFERENCE") and store them outside the graphical area of the sheet.
When drawing a part, simply copy/cut the annotation(s) you need and paste them into a view of the room for which you want to retrieve the information. Then we reposition the annotations or desired on the sheet.
The disadvantage of this method is that the annotations created in this way are not in the background of the plan but on the sheet.
Personally, I have a number of drawings in place that are used for both the assemblies and the parts.
To make everything work, I have parameters in my parts/assembly models that I use in the drawings.
There are 2 ways to use them: $PRPSHEET:"Description config" to use the 3D parameter (the part insert in the plan)
and $PRP:"Description config" which is a copy of the 3D setting when the drawing is created but which remains specific to the drawing. (i.e.: if you change the 3D parameter doesn't change).
Remember that there is the background plan and the drawing model.