PCB Power Trace Widths, Ground Planes, and Routing

It's just 4 layers. Where would you need more layers for? Most of the chips are surface mounted on one side. There is no sense in using more layers because you have no space to put the via's. If you look carefully at a modern motherboard, you'll find most of the signals are routed on the component side. This means the 2 inner layers and most of the solder side can be used for power.

--
Reply to nico@nctdevpuntnl (punt=.)
Bedrijven en winkels vindt U op www.adresboekje.nl

As far as I know, desktop type hardware is done on four layer boards.

I have personally worked on CompactPCI single-board computers that were 12 layers. IIRC, 14 layers is the maximum possible without violating a specification, and even so, it is kind of touch and go.

That is, the boards have to be physically within a certain thickness so that they fit in the card guides, and trace impedances are set down in the CompactPCI specification, too. If you go more than 14 layers on FR4, it is realistically impossible to simultaneously satisfy both specifications with achievable trace geometry.

These boards had Intel mobile processors, on-board ECC SDRAM (up to 18 SDRAM chips), C&T video, multiple ethernet MAC/PHY's and other junk I am probably forgetting right now. All of this on a 6U compactPCI card.

Oh yeah, one board had a dual fiber-channel controller. I think we went to

14 layers on that one.

--Mac

We only designed CompactPCI boards. CompactPCI is a spec put out by the PICMG

It specifies the thickness of all cards, regardless of whether they are master cards (like the ones I worked on) or peripheral cards.

Yeah, the cost wasn't a big issue. But we had an upper limit on trace impedance that was hard to meet with a 14-layer, 0.062" board. We had to use 4 mil traces on all the inner layers, IIRC.

--Mac

Did this once. Worked great until it came to EMI susceptibility. Never got as far as emissions. The board was mounted in a fiberglass enclosure and that didn't help, but neither did all the conductive spray paint and rf-gasket we could stuff into the blighter. Went to 4-layers, just added Vcc and gnd planes with thermal reliefs to the power vias, and it worked a charm.

FWIW, I would advise some caution if you are planning a grid ground plane on a 2-sided board with a real (not an 8051...) processor.

2-sided PC & AT motherboards were common on Taiwanese clones.

--
Nicholas O. Lindan, Cleveland, Ohio
Consulting Engineer:  Electronics; Informatics; Photonics.
Remove spaces etc. to reply: n o lindan at net com dot com
psst.. want to buy an f-stop timer? nolindan.com/da/fstop/

Still a problem with the power on the 2 sided board I guess. I made quite some combined audio / digital PCBs. Never had problems while using 2 layer boards even when the CPU was running its software from external memory and have several microphone inputs on the same board.

--
Reply to nico@nctdevpuntnl (punt=.)
Bedrijven en winkels vindt U op www.adresboekje.nl

Very important. Ideally you want every signal trace to have a ground return parallel to it all the way, on the next layer down. You also want the power to be distributed without significant static or dynamic voltage drops.

4 layers achieve this more closely than ever you can with 2, but I've had very good success with the following approach:

Route good thick (0.1") power traces for VCC and ground in the form of grid patterns. Ensure plenty of decoupling caps, you may also want to insert ferrites in the supply to some very busy ICs.

Route your signals, bearing in mind what you will do with the next step.

Flood fill all the area that remains with ground.

Use vias to stitch together all the ground fill and tracks. Examine closely to optimise the connectivity of the ground "plane"- many routes are better than fewer.

Iterate over the last stages until you are fed up of the whole thing and want to get a life.

Paul Burke