Yes. And you have to load them all into the gerber viewer AND CHECK every square centimeter on your board to make sure EVERYTHING is correct.
And if you serve the fab a particular layer, serve them BOTH front and back for it.
They don’t have to guess if you missed the other and call you back or hold your job.
If the file is empty for the other layer, they will know that’s what you want and not ask.
absolute minimum you need:
[boardname]-F_Cu.gbl
[boardname]-B_Cu.gtl
[boardname].drl
…plus any copper layers between them, if you got internal ones.
The following are ‘optional’…
If you board has a certain outline (most cheap fabs will otherwise just draw a rectangle as big as your layout and call it a day):
[boardname]-Edge_Cuts.gbr or .gm1
If you want soldermask that covers everything sans the pads:
[boardname]-B_Mask.gbs
[boardname]-F_Mask.gts
If your board has got silkscreen printing on it:
[boardname]-B_SilkS.gbo
[boardname]-F_SilkS.gto
Now we are getting into advanced topics, that need more understanding on your part on how this all works:
If you want to order a stencil for SMD solder paste reflow:
[boardname]-B_Paste.gbp
[boardname]-F_Paste.gtp
If you want to have it populated (not visible in gerber!!, those are text files and their format highly depend on the fab you use):
[boardname]-top.pos
[boardname]-bottom.pos
[boardname]-bom.csv
…if your board is being produced with SMD components on both sides you will need the adhesive layers.
And we could keep on going - more than 2 layers, you might want to provide a stack file, to tell the fab the heights of the prepreg between the copper layers.
Then there are other substrates, like aluminium core or polyamide for flexible pcbs (or a mix of them) or buried vias or microvias. Etc. pp.
The gerbviewer that ships with KiCAD doesn’t stick with a certain color <> layer list. It just loads the layers and assigns colors as they come in his list.
You have to create and load the same layers every time (even if you don’t use them) to make the gerbviewer colors consistent.
That’s why I always plot the copper, mask, silk, drill, edge and stencil file, even when a board doesn’t need them - makes my gerber viewing consistent - and send them all to the fab.
And check the layers for top and bottom separately (below screenshot shows my layer selection for the bottom layer check)
Oh, and use the legacy mode - the layers will be see through (menu I show in the screenshot).
The OpenGL canvas can’t do that yet - harder to spot problems.