PCB tracks as wide as possible or just as wide as needed?

Question

what is the best practice regarding the width of PCB tracks?

There are of course a few hard constraints :

• wide enough to keep voltage drop acceptable
• wide enough to prevent excessive heating
• at least as wide as the minimal width allowed by the manufacturer/manufacturing process chosen
• not wider than there is space on the PCB to route them

That gives a range, but often it is quite large, specially for low current tracks. So how best to chose within this "acceptable" range"?

There might be a few additional soft constraints :

• if one can avoid the smallest width everywhere, then it might be wise to do so (might be less expensive, or allow to switch more easily to another manufacturer with less precise process).
• for high current tracks, making them larger gives a lower resistance so a bit less energy loss (always nice)

But how to choose the width for signal tracks?

1. always the minimal width
2. always a little bit wider than the minimal width (to reduce the risk of defects on PCBs at manufacturing?)
3. always as large as possible (once everything placed and routed, just increase the width of each track as much as possible)
4. something else?

Well, basically, how to select the best track width when the hard constraints give a big range oof allowed widths?

Answer 1

PCB tracks as wide as possible or just as wide as needed?

The answer depends upon the use of the PCB tracks, and what is parallel to the tracks on the PCB.

PCB tracks with a ground plane parallel to them will have capacitance proportional to their area. In some cases, the components driving a signal will have a difficult time if the capacitance of their load is too great. In such cases, "as wide as possible" is NOT the right choice. Rather, the right choice is "just as wide as needed".

Similarly, if the PCB track is carrying a signal whose rising and falling edges are short enough, or whose frequency is high enough, the PCB track together with its return path (possibly through a ground plane or return track parallel to the track) will have a characteristic impedance. Changes to the tracks width will cause changes to the characteristic impedance. Each sudden change to characteristic impedance will cause signal reflections. Enough of these, or changes of sufficient size, and the signal will be degraded. In this case the right choice is NOT "as wide as possible", but "with a constant width".

However, if you are routing a DC voltage to some component, there is no harm in the route having significant capacitance, nor harm in variations of characteristic impedance. In fact, the trace capacitance may be beneficial, and the trace resistance detrimental. In these cases, the right choice may be "as wide as possible", rather than "only as wide as is strictly necessary"

Answer 2

It depends on the signals of course. You need to know what signals they are and what are their required properties.

If tracks are too close there will be too much capacitive coupling between them. If it is something that needs a specific impedance, then the trace width and distance between another tracks are highly important, and it might require specific PCB thickness from signal trace to ground plane to have the required impedance.