Your fabricator (Oshpark) almost certainly has instructions on their web site regarding the files they require and some details about generating the gerber files. They may prefer a file-naming convention that uses the filename extension to indicate the file’s purpose (e.g., ".TOP for top copper, “*.BSM” for bottom solder mask, etc.). There are slight variations from one vendor to another, so be sure to read their instructions.
They definitely need top and bottom copper layers. They may have specific instructions about the data format within the gerber files (e.g., “4.5” versus “4.6” precision, imperial versus metric, etc). In many cases they will tolerate any current data format supported by Gerber, but they probably have one format that is preferred. They almost certainly want the “RS-274X” file format, NOT “RS-274D”.
They also need drill information, in Excellon format. Creating separate drill files for the plated holes, and unplated holes, is the most customary practice but some fabs may ask for a combined file. Ecellon also has options for data representation - ask the fabricator which they prefer.
A few fabs will produce “naked boards” - just copper layers; no silkscreen; no soldermask - at cheap prices and quick turnaround but usually we get soldermask (both top and bottom) and silkscreen. The long-running “standard” is silkscreen on top only but a few places will do silkscreen on both sides at no additional charge.
Pay attention to how they want the outline treated. Some ask for a separate outline (“EDGE.CUTS”) layer with absolutely NOTHING else on it; others will ask for the outline to show on EVERY layer; a few may ask for an outline included on a particular layer.
In the “good old days” (formerly known as “these difficult times”) the fabricator liked to have a dimensioned drawing of the board outline, perhaps showing locations of significant holes (e.g., mounting holes). I produce this (along with all the fabrication notes) on the “.DWGS.USER" layer; others use ".CMTS.USER” or one of the “*.FAB” layers.
Don’t include additional layers if they are not used - that creates an environment where confusion grows. The paste layers are used to make solder-paste stencils for assembling surface-mount boards. The adhesive layers are for placing glue that holds components into place during assembly (absolutely critical for SMT parts located on the bottom side of a two-sided board!). “CRTYD” layers are mostly to guide component placement during layout, to ensure there is enough “elbow room” around parts during assembly. Some users create assembly drawings in the “*.FAB” layers; others use them to send information to the raw board fabricator (much like I use DWGS.USER). “CMTS” and “ECO” layers typically have purposes specified by local administrivial processes or the designer’s personal workflow habits.