I typically use 2 ounce copper as rule for all my PCBs. On a recent board I am using a 0.5mm pitch, relatively large micro, and noticed the pads aren't very flat. Assembly went fine with the protos, but I'm wondering if 1 once copper would provide for a flatter landing service. Does anyone have any experience with using 1 and 2 ounce copper with small pitch devices and/or any advice on assembly reliability related to copper thickness for such devices?
Unless you need high-current capability, 1 oz is the default thisckness. Line definition can be impaired with increased thickness, so only use when necessary.
1 oz (35 um) copper is much more suitable for SMD. Most board suppliers provide it as standard.
You don't seem to have a good reason to use the 2 oz copper ("I wish I had a good answer but basically because that's how we've always done it.") The main reason to use it is for high currents. If you don't have that, use 1 oz, it's the standard thickness and should be a lot cheaper than 2 oz.
I summarize PCB fab capabilities at the PCB manufacturers page. (You can help -- it's a wiki).
Capabilities are different for every PCB fab, but they often publish "preferred" capabilities that look something like
- 0.30 mm track/gap on 2 oz boards
- 0.15 mm track/gap on 1 oz boards
- 0.10 mm track/gap on 1/2 ounce copper boards
and "minimum" capabilities that are a bit tighter.
Thicker copper makes it more difficult to properly fabricate footprints for fine-pitch SMT components.
If you don't need lots of copper to provide a good heatsink or to handle high currents, you might be able to save a few dollars by using exactly the same board layout and specifying 1 oz or 1/2 oz copper instead of 2 oz copper -- especially if it results in the board being able to use one of their standard "preferred" processes rather than one of their more expensive "minimum" processes.
If you do need lots of copper to provide a good heatsink or to handle high currents, then a single PCB with 2 oz copper will likely to minimize your net costs. However, I've seen a few cases where designers were able to save a few dollars by re-designing the system to use 2 PCBs -- one small PCB with thin copper and narrow traces and multiple layers to support the fine-pitch SMT components, plugged into another PCB with one or two layers of thick copper and wide traces to handle high-current stuff.
If higher current handling is needed only in specific traces, I've often seen the use of a tin reinforcement on the copper. It seems to be quite effective, as explained here.