Finishing and optimizing the PCB

In this stage the designer must take care to various non-electrical layers and aspects which have to be performed in order to prepare the board for manufacturing.

For instance, the "silkscreen" layer, which is also known as the "component overlay" or "component layer", is the layer on the top of your board (and bottom if needed) that contains your component outlines, designators (C1, R1 etc), and free text. This is added to your board using a silkscreening process. White is a standard colour, but other colours are available upon request. You can even mix and match colours on the one board, but that usually costs extra.

When designing your board, make sure that you keep all your component designators the same text size, and oriented in the same direction. When laying out your own component footprints, were possible, make sure that you add a component overlay that reflects the actual size of your component. This way you will be able to tell at a glance how close you can physically position your components. Ensure that all polarised components are marked, and that pin 1 is identified.

Your silkscreen layer will be the most inaccurately aligned of all your layers, so don’t rely on it for any positional accuracy. Ensure that no part of the silkscreen overlaps a bare pad. There is no minimum width requirement for lines on the component overlay, so feel free to use smaller lines and text sizes to fit things in. If parts of the text or lines don’t turn out perfectly on your board then it does not affect your design, unlike tracks and pads. As a general rule, don’t put component values on the silkscreen, just the component designator.

Another important non-electrical layer is solder-mask. A solder mask is a thin polymer coating on your board which surrounds your pads to help prevent solder from bridging between pins. This is essential for surface mount and fine pitch devices. The solder mask typically covers everything except pads and vias. Your PCB program will automatically remove solder mask from pads and vias. The gap it leaves between the pad and the solder mask is known as the "mask expansion". The mask expansion should usually be set to at least a few thou. Be careful not to make it too big, or there might be no solder mask between very fine pitch devices.

The solder mask is displayed in PCB CAD systems as a negative image, just like the power plane. Under normal circumstances you don’t need to put anything on your solder mask layer. But if you want to leave the solder mask off a certain part of your board, you can place tracks and fills on your solder mask layer. It is often handy to remove a small square of solder mask from the top of your board, where there are no tracks underneath. This leaves a nice bare and visible part of your board to write something with a pen.

Solder masks come in two types, silkscreen, or "photo imageable". Photo imageable masks provide better resolution and alignment, and are preferred over silkscreened. You can get different colour solder masks, but the standard colour is green.

On most standard quality boards, the solder mask is laid directly over the bare copper tracks. This is known as Solder Mask Over Bare Copper, or SMOBC. You can get other coatings over your tracks in addition to the solder mask, but these are usually for fairly exotic applications.

You can have vias covered with solder mask if you wish, this is known a tenting. This is useful for close tolerance designs, to prevent solder from flowing into vias.