Start by finding the basic parameters required by the board house - trace width, copper spacing, hole sizes, soldermask clearance. (They aren’t necessarily the same for all board fabricators, or even for different pricing models at a single fabricator.) Enter these into PCBNew. Then get your design to the point where it goes through ERC and DRC with no squawks (either errors or warnings). The KiCAD DRC is still a work in progress - e.g., it doesn’t check for edge setback, and won’t detect silkscreen violations - but it is definitely your friend!
Find out how your fabricator wants the Gerber and drill files generated. Some want them named according to a particular syntax, there are options for the numerical format (systems of units, and precision), how the outline cuts should be handled, how to communicate special features such as cutouts or edge contacts.
Generate your set of Gerber files and open them in a Gerber viewing program. These are the files - not the KiCAD files, or what shows up on your computer display when running KiCAD - that tell the manufacturer how to make your boards. Does what you see make sense - i.e., do the copper, silkscreen, and soldermask layers seem to be what you want? Are there places where copper is missing, or copper that shouldn’t be there? At this stage, I’m usually looking at layers two at a time: top and bottom copper, for example, to check registration. Drill files versus copper and outline, for the same reason. Copper layers versus fab layer to make sure I didn’t put traces where they shouldn’t be. Top copper and top soldermask, to make sure that the pads (plus required clearance) aren’t covered, and everything else is. Top silkscreen (A.K.A. “legend”) and top copper, to make sure there’s no ink being placed on bare copper. Then, the same inspections on the bottom layer.
You’ll have to make some decisions about things outside of KiCAD’s scope. These include board thickness and material, soldermask color, copper thickness, silkscreen color, etc. Finally, prepare the package of files you’ll submit to the fabricator. There will almost certainly be top and bottom copper, top and bottom soldermask, drill file(s), and top silkscreen. Probably a separate outline file. Maybe a file showing the board’s critical dimensions, layer stackup, and fabrication notes. Possibly a “Readme” explaining what the files represent, how to contact you, special fabrication requirements, shipping and billing information.
This sounds like requirements imposed by an assembly house more than a bare board fabricator. You’ll have to contact them for details.
For a more comprehensive discussion of all the things you need to think about, get a copy of “PCB Design for Manufacture” from Seeed Studio (yes, three “e’s”). You can download it HERE.