pcb design rules

Hi, I depends on mostly the PCB manufacturer. If you are going to produce mass productions ask some of the firms that you are working with I suggest. We have different types of PCB rules for different projects and different manufacturers. You may send your Gerber files to the manufacturers and they usually check whether it is proper or not before production. Engin

I always make track and gap equal (unless there's an electrical reason to do otherwise). I've found that decent PCB makers have no problem with

6 thou tracks/ gaps, but it helps to keep the minimum hole a bit up, say 0.4mm or 0.5mm, if you can.

Why by the way are tracks always in thou and holes in millimetres?

Paul Burke

In 'merica, we use mils (thou) for drill holes. Most decent PCB houses can deal with 5/5 mil rules. Below that, you need to find a good house and pay more. Any wanker PCB house can handle 10/10 rules. I routinely use 8 mil via holes for my crammed boards. The board house will be happier if your via holes are more like 13 to 20 mils. Before commiting to a PCB house, see if they can show you a sample of their work. Talk to the PCB houses and find out what rules you should follow, especially if you're trying to hit a price target.

--
Mark

That's quite common in the UK. I find them easy to visualise, for some reason.

Leon

He stated "always" and that isn't true. We do all our design in mils, traces, holes, pads, spacings. I think it is more of a use whatever works for you kinda' thing.

Jim

It would help to know what sort of board you are designing.

For simple boards using only through-hole components, I normally use

10 or 12 thou tracks and spaces, and 62 thou pads with 35 thou holes for most parts. Vias are usually 50 thou pads and 25 thou holes.

Holes for component leads are usually 5 - 10 thou larger in diameter than the leads, and pads 20 - 30 thou larger than holes (this leaves a

20 - 15 thou wide annular ring around the pad).

--
Peter Bennett, VE7CEI  
peterbb4 (at) interchange.ubc.ca  

What I am trying to understand is for a certain track and gap what via size I should use. Presumably the two go hand in hand so that if a design doesn't quite fit I would be able to reduce both for the same incremental rise in costs but all I find is "ideally use this" and "worst case we can cope with this" but the grey area between doesn't get a mention.

Colin

I use EAGLE for PCB design. All of my boards have been prototypes (2 layer and 4 layer). I typically use 10 mil (0.010") wide traces and

10 mil wide spaces. For power runs (i.e. 5v) I use 24 or 32 mil traces. For vias, I specify a 20 mil (0.020") drill. Eagle's standard via drill size is ~ 25 mils. To connect a heavy trace on one side to the corresponding heavy trace on the other side, I usually use 2 20 mil vias instead of 1 large via. HTH

-Dave Pollum

Maybe this link helps.

BTW, there is a worldwide shift to the metric system, according to IPC. The driving force is an EC regulative.

150 micrometres width and space is common for most professional board makers with vias as small as 0.3/0.7 mm final dimension. Minimum is 75 micrometres for larger production quantities with vias as small as 0.1/0.3 mm (bore/ring) - so called microvias. Only a few can do this. E.g. in Germany you might find around 5 PCB manufacturers doing this. Utmost minimum is 50 micrometres, but with a high count of unrectifiable rejects. I know one manufacturer. 200 micrometres with 0.4 mm bores is standard low cost. There is almost no exemption.

Greetings GerhartH

At some time in a previous century, the board shop charged extra because I had specified 24 thou vias instead of my usual 25 - this made me standardize on 25 thou. However, the board shops I use are now willing to go down to 16 thou or less at no extra charge - however, from habit, I still stick with 25 thou unless I really need to conserve space.

--
Peter Bennett, VE7CEI  
peterbb4 (at) interchange.ubc.ca