PCB Trace Width

[clubrulz]

I have now started using Express PCB to layout my own boards. The question I have is:

Is it better to have more copper or more space betwen traces. For example, I just layed out the Purple Plexi and used 1mm wide traces for all components. It looked like a lot of white space so I started to fill in the traces, leaving only about 1mm between some of the traces. My thought is to hvae more copper around the component holes to ensure I have a good connection between the comopnent and the copper on the board.
I figured we are dealing with mA and uA here so surely 1 mm between the traces should be good. Right?

[amptramp]

For signal traces, thin connectors have less capacitive coupling to other circuit elements, but the most important thing in a Purple Plexi is that it is based on an LM386, so the ground traces should be wide for less resistance and inductance.  The LM386 is a power amplifier IC and it can pull considerable current, so wide power and ground traces help with stability, especially the traces connecting the bypass capacitor across the power pins.  All signals are referenced to this ground since there is no Vcc/2 supply in this circuit.

[Seljer]

If you google for "pcb trace current" you'll find little calculator applets that'll help you to figure how wide of a trace you need to cover any thermal issues that may arise.
With the typical currents in stompboxes never being more than couple of 10mA on the power rails don't really have to worry much, the limiting factor is more how clean lines you can achieve with your chosen fabrication method (if you do the UV resist method or have a well set up CNC machine you can get some *really* fine traces). If I'm making the boards myself I also like to add some extra copper to all the pads (the restring feature in Eagle) so I can get away with larger tolerances when drilling.

A ground plane, besides providing a low impedance ground point also fill up all that blank space so it saves up etchant if you're making the PCBs yourself.

[karbomusic]

If I'm making the boards myself I also like to add some extra copper to all the pads (the restring feature in Eagle) so I can get away with larger tolerances when drilling.

Same here, that's a great feature. For the OP, I typically do 24mil traces, sometimes 16 to squeeze between IC pins with large pads. I've done 12mil but that is an exercise in extreme accuracy when using press and peel like I do. I usually use either 24 or 16 for isolation on the ground plane when I use one. I've gotten better at the iron on method as of late..

[R.G.]

I have now started using Express PCB to layout my own boards. The question I have is:

Is it better to have more copper or more space betwen traces. For example, I just layed out the Purple Plexi and used 1mm wide traces for all components. It looked like a lot of white space so I started to fill in the traces, leaving only about 1mm between some of the traces. My thought is to hvae more copper around the component holes to ensure I have a good connection between the comopnent and the copper on the board.
I figured we are dealing with mA and uA here so surely 1 mm between the traces should be good. Right?

It's a complex subject, but in general, for effects, trace widths 0.01"/0.25mm are fine, if a bit fragile. I habitually use 0.025"/ 0.635mm wide traces on a 0.025"/0.635mm grid, but my PCB software is set to alert me when conductors are nearer than 0.010"/0.254mm spacing, so this has the effect of putting traces 0.05"/1.27mm apart for most situations.  I also do not hesitate to drop to 0.012"/0.317mm traces when needed, with the same "warn me when spacing gets under 0.01"/0.25mm".

Power and ground traces should be no less than 0.025"/0.635mm wide, and wider is better.

So, for your question:
- 1mm wide traces for signal and general use is generous. If you can do it with this wide trace, it's fine. Don't hesitate to drop to 0.5mm or 0.3mm if you need to for signals.
- 1mm between traces is WAY generous. I use about 20 mil/0.5mm on average and don't worry until some spots get below 0.01"/0.254mm.
- the industry wants pads at least 0.020"/ 0.5mm bigger in diameter than the hole. That's very, very minimal. Use 0.062 minimum pads unless there is good reason not to.

[therecordingart]

double post

[Transmogrifox]

I found for home-made (etch resist and chemical) the wider the better, and also much larger pads than needed on through-hole parts for reasons mentioned above.

My biggest concern with a DIY board generally is the mechanical strength of things (how clumsy can I be and still not break traces).  Also I like having wide strong traces so the board can endure multiple cycles of changing components.  If it's a one-time build then this is less concern.

Just my own 2 cents.

[PRR]

> I figured we are dealing with mA and uA here so surely 1 mm between the traces should be good.

AMPS guide the *trace* width.

VOLTS guide the *between trace* width.

I would not hesitate to do 1mm trace-space in 300V work (different for the stuff from a wall-outlet). So all your 9V and 24V work, 1mm is overkill, and fine.

I'd have to look it up, but 1mm trace should be fine for an Amp, and no pedal has any 1-Amp traces.

But several Special Situations.

If you etch in a tray in the shed, you may want maximum copper and small bare spaces, so the etchant does not have to work so much. (If you send it out, that's the PCB-fab's problem and they don't charge extra for taking more copper off; they probably filter and re-charge their etchant at don't-care cost.)

As said, large copper is more robust against repeated (or clumsy) soldering.

I've never really cared about capacitive coupling on PCB. The main thing is to keep sensitive traces short, next keep them away from loud traces (outputs, power, clocks). PCB is generally much less capacitive coupling than tight hay-wire work, the way most early pedals were made.

If your technique is unrefined, either narrow traces or spaces is risky. Using Sharpy for resist, it may look like about 1mm, but ink-gaps can leave microscopic breaks in a trace, and ink-drift can leave hair-fine whiskers between traces.

Precision micro-screens can reliably produce traces and gaps the human eye can not see. This is key for modern micro-gizmos (cellfones, some digital pedals). A good PCB package will let you set such teeny lines/gaps. Occasionally it can be handy to sneak a trace between DIP pins. _Me_, I would not try that on shed-etch work (a jumper is more reliable than clever etching).