Layouts created using Notebook functionality are capable of driving design from a top level data set in the .lay file. You can declare the layout to parts and then use the parameters and relations from the layout to drive multiple children. The layout will allow for the creation of global parameters that can then be passed to multiple children to control common design intent across models. Once the layout exists you can declare it to a model and then all design intent in the layout is available for use in the model(s) you declare it to.
PTC has not really added much to this tool since it was first offered and I think they intend to use Mathcad to replace the layout tool in Creo. It is very useful but the interface/setup has not evolved. You will need to import graphical data as DXF and then create the parameters and relations needed in the layout to control your part models as intended. You can at any time decide to undeclare the layout so that it is not driving a model if you need to.
As long as you can write equations that capture your design intent then the layout should work for you but it will require up front planning and development.
The enclosed picture is an example of a layout used to design and control the geometry of the individual components of a 2 stroke internal combustion engine. The input parameters are entered in the layout and relations are used to compute the correct values needed to create the geometry that will realize the desired parameters in the individual parts.
The trouble with notebook and advanced assembly is that we don't have those particular modules. Probably won't ever have them for that matter. We already get lots of complaints about the cost of the licenses we do have.
That's why I use assemblies to handle this type of functionality. It's not a specific tool designed for the job, like part skeletons and the like, but it's available in even the most rudimentary of installations.
Ok, so I went ahead and started a new "Master" assembly. I created several simple sketches using the assembly datum planes as sketch references. With these sketches I have all the pertinent information to create all of my parts.
What I am wondering is, if I were you, what would you do next? Do I:
Create part > Empty > Extrude using sketch plane on assembly datums > project geometry from necessary Master sketches?
In the master I do Model -> Create and start with an empty part (or use one of your template parts as a start)
Then activate that part and start building features, like extrudes, revolves, etc. Use master datums as sketch planes, etc.
When you're done with the part you're working on, make the activate the assembly and go on to the next part.
Be careful when building parts, that you do not use any edges or such from the other parts. You always want to define everything using the master geometry. I usually hide parts as I go along to avoid this mistake.