As in many CAD packages, you should first have an idea of a starting point for the design. I would then create an unattached flat wall (I'm new to Pro/E, this is how I would start). Use some basic parameters like material thickness, inside and outside bend radii, etc. At some point you need to make sure that it can actually be flattened and stamped on whatever machine will be doing this. If oyu're going to incorporate some special features like embosses or ribs or anything else, it might be a good idea to have some knowledge of what tools are in stock. One of the neat features that I have found in Pro/E is that I can model punches and dies and have them stored in a location that I can use later on other sheet metal pieces.
Hope this helps in getting started, I'm sure that there will be many responses from other more seasoned Pro/E users than me, but if you need more help, ask for it.
You have left your question very open and it is difficult to corner exactly what you are asking.
I usually start out by creating a flat first and running bends off of the fundamental geometry.
The commands generally run like any other model creation command
feature, create, flat
feature ,create, bend,
feature create , cut... etc.
You have to either convert standard geometry to sheet metal or switch over to sheet metal from standard pro-e however.
It might be recommended that you run through a tutorial to get a feel for the commands. Not sure what is meant by quality but in general , whatever you model will accurately translate to a sheet metal station(punch press, turret punch, lazer punch)
You might want to check with the sheetmetal vendor to see what they prefer to make the parts economical, bend radii, tolerance and tooling available. Most vendors have tooling lists available as well as design guidelines.
Bend deduction varies between vendors and tooling used as well as whether it is going against the grain or not so the default bend tables may not give you accurate results. Usually the vendor changes this parameter per his experience so you have to specify whether to use your flat or bend parameters.
Generally .01 tolerance and .03 inside radii is used commercially. You may have requirements for >thickness inside radii like they use in the aerospace industry.
Start with a primary wall, Flat or Extruded or Revolved as required. Optionally you can shell a solid and convert it to sheetmetal at the start. You can Copy Geometry from a part or assembly and use this to begin your walls.
I usually Set Geometry on the primary wall from the start but that is just the way I do it. This can be a flat surface or edge that is the fixed surface or reference to flatten the part from. I usually start with a flat or extruded wall and build walls off of that.
If you make a cut or hole thru all (multiple walls) do it before you flatten the part, otherwise it won't be in all locations when the flat pattern is made in the end.
Creating a flat state takes time to regenerate so do it as seldom as necessary, like once. If you flatten it just to see the results of a feature and not to create a feature you should delete that flat state in the model tree.
Many vendors will take your model to generate the machine tapes from, especially if it is to be laser cut.