Moats, islands, cuts in the ground, isolated power planes, floating ground regions and a host of other intricate layout techniques are routinely used by digital engineers to reduce crosstalk, bolster EMI performance, and otherwise improve overall system operation. Yet I rarely encounter an engineer who can show me a clear before-and-after comparison demonstrating precisely what was the effect of the "improved" layout. Why not? The excuses most often given are: lack of time, money, and schedule for a separate test board. It's not that the testing process itself would be difficult. Given a test board, comparing the performance of two layouts is easy. The problem is that we don't usually have the test board.
We can improve this situation by taking advantage of the way PCB's are designed and manufactured. To see how this can be accomplished, let's first focus our attention on the interface between your layout shop (the people that route PCB traces) and the board fabrication shop (the people that make bare, printed circuit boards).
This is the point at which your board design crosses over into the realm of real-world manufacturing. It is also a point beyond which many of us digital engineers rarely dare to venture, and that is a real shame. If there is one thing I have learned over the years, it is that the more we know about manufacturing, the better our designs tend to be. I'd love to write a whole book on that subject. For now, let's turn our attention back towards the layout-to-board-fab interface. With a better understanding of how this interface works, you can learn to get 8 different prototype board designs fabricated for the price of one.
In most cases, information is transferred from layout to board fab in the form of Gerber files (see note). The standard Gerber file format is a rather primitive, but highly effective format for describing two-dimensional graphical information. It is well-suited for representing the two major components of a PCB image: lines and dots. To first order, you might think of each file in a Gerber file set as representing a picture of one layer in your printed circuit board stackup.
The layout house forwards to the fab house a set of Gerber files that completely represent every layer of your board.
Now, things get interesting
The first thing the fab shop does with your Gerber file artwork is to panelize it; that is, to step and repeat the artwork several times in order to fill up a standard fabrication panel.
Fab shops like to work with big sheets, or panels, of printed circuit board material. Typical panel sizes might be 12" x 18", 18" x 24", or even bigger. The bigger the panel, the lower their manufacturing costs. On a big panel, a fab shop might be able to panelize six or eight of your circuit cards, resulting in less handling of each individual card, and lower costs than if the boards had been individually fabricated.
On a typical prototype run for an EISA card, the fab shop takes in one copy of the Gerber files and panelizes it to create a new Gerber file set that shows maybe eight boards on one panel. Next, they make a set of panelized artwork masks from the new Gerber files, and shoot a couple of panels worth of boards. Then they chop the boards apart. You end up with a set of perhaps sixteen cards for their minimum prototype processing fee. That's probably more than you wanted.
If you want to get more out of the prototype fab cycle, try this: ask your layout house to "pre-panelize" the design. They will have to call the fab shop to get all the rules about panel sizes, minimum spacing between boards, placement of tooling holes, edge clearances, and the like, but it's well worth it.
The prepanelized design, like a regular design, results in a set of Gerber files. The difference is that the prepanelized design includes eight full copies of the same design, all laid out for fabrication on one big panel. Once you have the prepanelized Gerber files, this is where you get to have some fun. Have your layout person open up the Gerber file editor and just GO CRAZY!
Of the eight boards on your panel, try shorting out the moat on one, eliminate the guard traces on the next; just go ahead and do all those little modifications you always wanted to do but never seemed to have a chance to try.
Sure, there are limitations on what you can modify with a Gerber editor. Your layout person can explain them. It's not perfect, but it gives you a wonderful opportunity to really learn something about your design.
Best of all, the fab shop probably won't notice. They will just take your panelized Gerber files, make the artwork masks, and shoot some panels in the regular way. When the boards come back ready for assembly, you'll get back all the real boards you need, plus all of the test layouts. By piggybacking your test designs onto an existing fab cycle, the test boards will appear, like magic, right when you need them. They're almost free, and have very little impact on the whole schedule.
What's more, now you have a way to directly quantify the benefits of your layout tricks with an apples-to-apples comparison of like designs.