The lettering and graphics that identify part locations, trade marks etc. is called by many names and the one we use is legend. Some other common names for the legend layer are Silk, Silkscreen, Ident, ID, and Nomenclature. The reference to "Silk" comes from the method that is widely used to apply the ink, and that is via "silkscreen".
The silkscreen ink used in PCB fabrication is designed to withstand the heat of mass soldering systems with minimal pigmentation change. Standard inks will scorch or burn off completely when the board is heated to mass soldering temperatures. The legend ink we use is White LPI or liquid photo imageable epoxy ink. This type of application allows for excellent detail with fonts used identifying parts.
The minimum line width is .006"/ .15mm for surface adhesion. Line widths less than .006"/.15mm either completely wash away or appear faded and often accompanied with voids in the characters and patterns. When we detect smaller width lettering we will swell it to the minimum width when possible. The minimum height for legibility without magnification is around .030"/.76mm. You can go as small as needed up to the restriction of the .006"/.15mm width. Too small and the letter becomes an illegible blob under magnification.
The often green coating on circuit boards is called Solder Mask. It's widely known as solder mask, occasionally referenced as silkscreen, which can add confusion. We'd prefer it is referenced as solder-mask. Our application method is Heated Vacuum Lamination of Photo Imageable Dry Film. The film is Gloss Green and is 0.0015"/0.0381mm thick.
Add 0.003"/0.0762mm to the board thickness for solder mask. (2 sides x 0.0015"/0.0381mm).
The dry film is applied over bare copper. This process is referenced as SMOBC or Solder Mask Over Bare Copper. The dry film solder mask is similar in image resolution to the legend ink. A minimum .0065"/.165mm of material is required to adhere to the substrate surface or it washes away, or worse, leaves string like threads dangling or sticking on areas it shouldn't be present.
We prevent threads by swelling the pad gaps to form a complete block-out of the region. QFP's are often masked in this fashion. A shrink or swell of the mask layer pads is done to achieve a .002"/.051mm moat around the desired areas. If the resulting swell or shrinking of the mask pad creates a thread width under .0065/.165mm, the region is fully blocked as a preventative measure against downstream finish and HASL failures.
Caution: Please be aware that any drill hit or cutout which is open in the solder-mask on one side of the PCB must be opened on the opposite side. A 0.002" swell is the minimum oversize requirement. Our CAM team will edit as required to meet this production stipulation.
The reason the pads must be fully tented or fully exposed on both sides in solder-masking is due to the HASL process. Hot Air Solder Leveling is a combination of heat - the eutectic temperature of solder, and high pressure hot air. When a board contains a tented pad on one side which has an opening on the opposite the molten solder will trap in the hole. This is because there is no way for the hot air to pass through the hole - the mask blocks it. The hot-high-pressure air (130psi @ 450F) can also blow the mask off the tented side causing cosmetic defects and contamination the solder pot which contains about 400lbs of molten solder. Pieces of the mask blow off with a volcano effect, called de-lamination, this is when the mask material looses its bond from the substrate.
Bottom Line DON'T DO IT - both sides open or both sides closed.
Our in-house services use DFPI Gloss Green for solder mask and White LPI for legend.