Minimum trace width and spacing for 2oz copper

[HwAoRrDk]

I've been looking at designing a board that may need to use 2oz/70um copper for current-carrying capacity.

I have seen mentioned that when using 2oz copper, your minimum trace width and spacing must be larger compared to regular 1oz. Why is this?

And if so, what value would people recommend for minimum trace/space for 2oz? I usually go with 12 mil width and 10 mil clearance. Should I increase either?

[dave_k]

Check with your PCB manufacturer for what they recommend and what their capabilities are ..

[T3sl4co1l]

^^^

Minimum trace width and spacing must be several times the copper thickness, except for a few very special processes ($$$).  This doesn't usually affect 2oz proto boards (7/7 rule is usually acceptable).  3oz+ may need wider rules.

If you need finer, I've seen 4/4 available for 2oz, but you'll pay more for it (whether because of poor yields from a cheap source, or good yields from an expensive source).

Tim

[HwAoRrDk]

The only thing I could dig up from the websites of a couple of PCB manufacturers I've used before is a single line buried deep in a FAQ page from one of them, that says they recommend 10 mil trace/space for 2oz. But I don't know if this is a common figure.

If that's standard recommendation for many proto-grade services, then that's no problem for me.

Minimum trace width and spacing must be several times the copper thickness ...

So what is it about the etching process that requires this?

I would have imagined that thicker copper would allow the opposite: finer features, as you wouldn't be in as much danger of etching the copper away completely.

[T3sl4co1l]

Copper etches more or less uniformly, so that a trace, covered with positive resist, takes on a tapered (trapezoid) shape, thinner at the top than at the bottom (laminate surface).

This is reversed with negative resist (tin plate process), where the trace is plated up and mushrooms out instead.

AFAIK, typical proto boards are made with both steps.  As a result, the profile of a trace edge can be a little funky (having both undercut and overbite).  But in any case, the funkiness is exactly equal to the foil / plating height.  So that's where it comes from.

(There's one process that uses metallization in vacuum for the initial board copper, instead of foil lamination.  The initial layer is quite thin, a few microns.  The resist is negative, relatively thick, and happens to have straight sidewalls.  The exposed copper is plated up to the full trace thickness desired.  The resist acts like a mold, so the traces are straight sided, and can be very close together.  In the final steps, the resist is stripped, and the whole PCB is etched briefly: just a few microns, just enough to remove the initial layer that was hidden by resist.  The traces, being much thicker than this, are nearly unaffected.  IIRC, this process is unique, used by the company that happens to be the only PCB mfg in Australia.)

Tim

[GreggD]

I did some 6oz boards with 0603's and our shop wanted 18mil spacing. +&- 150V @ 35A

[T3sl4co1l]

I did some 6oz boards with 0603's and our shop wanted 18mil spacing. +&- 150V @ 35A

That sounds about right, and you'll just barely fit 0603s, SOICs and such on there.

Tim

[Warhawk]

I made 6/6 board with 2oz plating. However, not everyone can make it therefore it was expensive an I am not going to do that again

[Someone]

Copper etches more or less uniformly, so that a trace, covered with positive resist, takes on a tapered (trapezoid) shape, thinner at the top than at the bottom (laminate surface).

This is reversed with negative resist (tin plate process), where the trace is plated up and mushrooms out instead.

AFAIK, typical proto boards are made with both steps.  As a result, the profile of a trace edge can be a little funky (having both undercut and overbite).  But in any case, the funkiness is exactly equal to the foil / plating height.  So that's where it comes from.

(There's one process that uses metallization in vacuum for the initial board copper, instead of foil lamination.  The initial layer is quite thin, a few microns.  The resist is negative, relatively thick, and happens to have straight sidewalls.  The exposed copper is plated up to the full trace thickness desired.  The resist acts like a mold, so the traces are straight sided, and can be very close together.  In the final steps, the resist is stripped, and the whole PCB is etched briefly: just a few microns, just enough to remove the initial layer that was hidden by resist.  The traces, being much thicker than this, are nearly unaffected.  IIRC, this process is unique, used by the company that happens to be the only PCB mfg in Australia.)

Tim

Good details, most PCB manufacturers will scale the track/gap rules proportionally with the copper thickness.

The company doing copper deposition is Lintek: http://www.lintek.com.au
"Big Dollars" for the service but it can deliver some very fine/precise geometries, there is another Australian PCB manufacturer I know of:
http://www.pcbfast.com.au/techinfo/multi-design-panels/
Who answer the age old question of why manufactures don't like multiple designs (but it still doesn't add up to me, there is no extra charge for a wildly complex design that fills the panel size).

[KL27x]

Etching my own toner transfer boards, the difference is obvious. 10/10 is pushing it with 2 oz. I can just barely do ssop footprints. The lone traces will suffer some overetching by the time the tight pitch stuff is completely done. I might even have to scrape out tiny bridges in the ic footprints. And overall, everything is wavier and fuzzier around the edges.

With half oz or 1 oz, even 7/7 is easier and more consistent than 10/10 on a 2 oz board.

For the manufacturer, even if they can do x/x in 2 oz, their yield will be lower than the same in 1 oz. At some point they cant afford to do it at a given price.

*edit, and yes, the trapezoidal shape of the traces is very distinct and obvious under the microscope on the 2 oz boards!