Routing power lines on top or bottom plane?

[Aeternam]

Noobie question incoming.

On a 2 layer board with a ground plane on the bottom, where do I put my power tracks (VIN, fuse, regulator I/O,...)? Is it ok to put them on the bottom also? This would leave the top layer for signal tracks only and result in a MUCH nicer layout. It's a DC, low voltage, low frequency, low everything board, nothing fancy going on.

I have read Dave's design primer. He suggests that you reserve a layer for power tracks and one for the ground plane on 4 layer boards, but I'd very much like to keep it at 2 layers. This whole PCB thing is messy enough as it is 

Is this a good idea?

[ovnr]

If you can keep the bottom layer as close as possible to an uninterrupted ground plane, that's better.

I'd suggest routing them on the top layer as long as it doesn't result in a complete mess; and even if that happens, don't just move it all to the bottom layer.

[tszaboo]

If you cannot keep a relatively solid ground plane, then it is better to route the ground same as other signals, and add a fill later. I would put power supply on the signal layer. If the signals in the way, you can still, do via -> short trace on bottom -> via, as many time as you want. If you post picture (read as: JPG file) of the board, we can help.

[Aeternam]

Ok guys, thanks for the input. I'll post a pic of the board once I'm done with the routing.

[chota.sanjiv]

dont pour ground on the top and have a full soild gnd plane on the bottom, this will ensure no gnd loops and single return path below every signal.

[T3sl4co1l]

For N layers, use approximately N/2 planes.  Route all other signals and supplies as usual.  Assign power rails to planes by priority.

For a 2-layer board, you have only one plane available (not even an unbroken one, at that).  Ground is the first priority.  Thus, all supplies get routed with traces.  You'll use more bypass caps, because the trace inductance will be relatively high.

For 4 layers, GND takes priority, then VCC (for example, a conventional digital design where a 3.3 or 5V supply dominates).  Other supplies, and signals, get routed as normal.  If different sections require different supplies (e.g., a 12V analog section), the power plane can be split into zones, as needed.

For 8 layers, GND may again return to priority, so that you have 4 routing layers, 2 grounds and 2 supplies (maybe 3.3V VCCIO, and 1.8V or 2.5V for core or memory supply).  Good grounding is always top priority.

Supplies on planes have excellent power quality, so that very few bypass caps are necessary.  You certainly don't need a cap per pin, as some appnotes recommend.

If you like, the power supply network can be analyzed: simply convert trace lengths to inductances, capacitors to RLC series circuits (typically, an 0603 size 0.1uF capacitor, with two vias tying to internal planes, clocks in at 3nH ESL and 50mohm ESR), planes to (small) capacitors with little or no inductance, and so on.  Plug this into SPICE and manipulate cap values, and types, until the impedance is stable and doesn't exhibit ringing.

Back to 2 layer boards.  Note that you can't have an unbroken ground, in almost all cases.  You inevitably need to cross traces, and those crossings must be done opposite the routing layer.  Try to minimize crossings, and pour ground on top and bottom and stitch the pours liberally with vias, so that it all acts as one plane, that averages out as if it were a middle layer.  Do not leave unconnected islands (they're better to remove altogether), and try to use two or more vias per island so there is a current path through the copper.

Tim

[KL27x]

It's a DC, low voltage, low frequency, low everything board, nothing fancy going on.

In this case... do it any way you want. 

[lorth]

dont pour ground on the top and have a full soild gnd plane on the bottom, this will ensure no gnd loops and single return path below every signal.

Not totally true, that only happens when Freq > 100KHz. At lower frequencies, it's basically the shortest path.