Changing trace width on a PCB after reaching component pad

Question

People advise not to change trace widths on a PCB because of the change in impedance of the trace and possible signal reflections for example. Does that still hold true when the trace reaches a component pad/pin (surface mount or through hole)? Or can I go from a 25 mil trace to a 50 mil trace without fear when the trace reaches the component pad (as if it were an "independent" trace)?

For example, if I have a power trace which, because of spatial constraint had to be small, can I make it bigger if space is available after reaching a certain component so that it may go to other components?

Answer 1

Does that still hold true when the trace reaches a component pad/pin (surface mount or through hole) ? Or can I go from a 25 mil trace to a 50 mil trace without fear when the trace reaches the component pad (as if it were an "independent" trace) ?

The presence or absence of the pad at the point where the trace width changes makes little difference. The signal propagating along the trace will reflect off of the discontinuity caused by changing the trace width.

If you're working with low frequency signals (the associated wavelength is more than 10x the total trace length) then the discontinuity and reflection aren't likely to have much effect at all (whether there's a pad or not).

If you're working with high frequencies (wavelength less than 10x the trace length) then the discontinuity and reflections are likely to have significant effects. In some cases this may be highly detrimental (for example, you just want to get the signal from one end of the trace to the other without disturbing the waveform). In others it may be unimportant or even desirable (for example the wider trace is part of a quarter-wave transformer you deliberately designed to match the impedance of the ultimate load at the end of the trace).

Answer 2

This is a broad question as it depends on various factors. You, as the designer, must ascertain if changing track width is feasible or necessary.

On controlled impedance tracks, changing width may cause signal integrity issues. Or, you may be required to change widths to maintain signal integrity as is done on some DRAM layouts.

For tracks that carry ho-hum signals (don't require controlled impedance, slow rise time signals, ...) adding teardrops to the pad-track interface is useful for improving mechanical integrity of the track-pad interface if that area of the PCB is flexed, e.g., areas where vibration or and/or connector removal/engagement can cause issues. I often use teardrops when going from small width tracks (<0.010 inches) to connector pads.

Teardrops are also useful in reducing trapped chemicals in sharp corners during the PCB manufacturing process (this was, may still be, an issue with silver plating). The trapped chemicals (acids used in the manufacturing process and/or assembly process) may cause failure of the track-pad interface over time.

You may need to neck down a trace to maintain clearance between features.

Answer 3

PCB pads for components need to be the size they need to be in order to mount the component.

And PCB tracks must be the size they need to be to have a specific controlled impedance.

So there must be a size change which is a discontinuity but chanses are with proper engineering the PCB pad effect can be mitigated somewhat to achieve good enough performance.

If the impedance change is small compared to signal speed then it does not matter much.

And power traces are rarely not considered as impedance controlled, you just need to worry about track being wide enough to have low enough resistance to pass enough current with low enough voltage drop, and wide enough to have low enough inductance so the chip can get the required current quickly enough when it needs it. And then there's bypass caps for local high frequency storage.