I am confused about the meaning of “text” on the F.Cu layer.
The image shows the SCL text but indicates it is on layer F.Cu. I understand F.Silkscreen but what does F.Cu text mean in this context? Will the text get printed as copper etching? If not what is the function of this-- text notes for layout only? Thanks
I put “1”, “2”, “3”… on copper layers of multilayer PCBs with a window in the copper on all layers and resist so that I can inspect to see if the PCB stack up is correct. Long ago I had the manufactured layers messed up, one layer repeated and one missing. I have also seen one layer flipped. All scrapped boards.
Yes.
Plus a few characters.
You should try putting text in a mask layer. Because it’s a subtractive layer the effect is lettering in the selected Cu finish, e.g. HASL, ENIG, etc. Not all combinations make sense in normal situations but sometimes can be useful.
Maybe a spy could snuggle secrets out on an inner layer that would require X-rays to read. 
Snuggling is good, just not on a PCB. 
You don’t know the amorous lengths to which spies will go.
I once texted a friend about an Aldi special rice cooker sale. He texted back that his wife wouldn’t have use for a rice cooler. There are lots of hilarious but unprintable autocorrect alterations.
Seeing we’ve strayed off topic:
A female boss a couple of years ago left a message on my phone.
The message was “I have fill-ins for you, please phone me.”
The “smart” phone turned this to text which read: “I have feelings for you, please phone me.” 
Next time I’ll use a synonym that autocorrect will have difficulty mangling, like say exfiltrate.
In the screenshot it’s clearly information for the connector (pin header) pins. In this way the text will be copper, and the area around it will be bare. It’s just one way to print text on the board. There are three ways to add text: copper, mask, and silk. Each one can have text as absence or presence of material. There’s nothing weird in this, and it depends on the situation what is the best way. Usually copper and mask have better resolution than silk, so the text can be smaller. Silkscreen text gets quickly unreadable when going under 0.8 mm height (or something like that). Mask or copper may be readable with, IIRC, with 0.5 mm height or something like that. Actually I have used text so small it wasn’t readable with naked eye but was with microscope. Text on copper or mask may also look “cooler”, if you want that.
Excellent reply with a useful summary of options. Thanks to all for helping.
One more question related to text…
What is “mask text” (using F.Mask)? How is this different from F.Cu text? Tradeoffs? Thanks! Al
Here is an image of the board with all 3 text types
F.Cu text top then F.Silkscreen then F.Mask text bottom. In the 3D viewer the silkscreen text is “brightest” and the F.Cu text is lightest, I know this a 3D display choice but it mislead me at first.
It might have been mentioned above already, but text on F.Mask will open up the soldermask that covers the copper. So F.Mask text on a copper plane will have the same appearance / plating as the pads of for example SMD footprints.
Text on F.Cu will result in shaping the copper itself into text.
It can be covered with solder mask, or you can separately remove the solder mask around the text if you want.
Thanks!
It’s becoming clearer… So, F.Silkscreen and F.Cu text are positives (additive text) while F.Mask is a negative (subtractive text). True?
Does the F.Mask needs a “copper zone” to work? I can imagine removing copper from the zone resulting in readable text. Not certain about “SMD footprints” above since these are just copper rectangles and seem more like F.Cu text.
You should be able to see these effects in the gerbers. May be useful to generate them with a “test” design to better see the effects. Be sure to delete these gerbers after you view them (assuming they do not represent the final design). Else come time to collect files for PCB mfg they could get caught in the submitted files.
Yes, the silkscreen and copper layers define presence of material, i.e. any figure (graphics) in these layers mean that there is material in the corresponding manufactured board layer. Mask is negative: graphics means absence of material, i.e the mask substance which otherwise covers the board doesn’t exist where there is graphics in the design layer, either PCB Editor or the gerber file.
No, but you should consider readability. It depends on the needs. It’s hardly a good idea to put green mask text – either positive or negative – directly on the green board material if someone needs to read it easily. If you put mask text – either positive or negative – on copper, the result depends partly on the copper finishing if it’s applied to all bare copper.
Even though you are given only the choice of one colour for both the mask and board their colours differ slightly so you can with some difficulty make out mask text on bare board. If you look closely you can also make out the ridge due to the thickness of the mask layer.
Also we talk about text but it applies to any graphics.
In short what you get is the specified superposition of the layers.
As an example at PCB for DIN-rail case the terminal blocks are close to PCB edge - there is no enough room at top layer (were we have silkscreen) to place text identifying each pin. User will have it identified with texts at its case but during writing a software for it you have it without case. When you connect wires to it it would help you if you know what signal is expected at which pin. So I used text at bottom copper and the same text at bottom soldermask to get this pins signed in gold. Those PCBs were ordered without silkscreen at bottom.
Thanks, all very useful. Now I appreciate that the mask material, green, also can be used for text. Lots of combos and tradeoffs… Al
It is shown green in KiCad as default, but manufacturers have different colours (for example one makes the boards with purple mask), and often the manufacturers have several different couloured masks you can choose between (only one colour per board though).