PCB Design – Trace Distance from SMD Pads


Having followed a fabricator's DRC (this case being OSHPark), this distance between an SMD pad and a trace is considered acceptable (see attached images).

However, I wanted to inquire about what the accepted logic is behind the distances between traces and SMD pads, with and beyond manufacturing restrictions? My initial thought jumped to how exactly the SMD components are soldered, but am unsure what considerations to make in practice as I will be hand soldering them.

These examples are of SOT-23 transistor and a 0603 resistor respectively.

Example 1:

SMD / Trace distance

Example 2:

SMD / Trace distance

I've read through this question, which I think has pertinence.

Best Answer

There are really three levels of concern: Manufacturing (the blank PCBs), assembly (soldering components onto the board), and electrical (everything actually works as intended!).

  1. Manufacturing

    As long as you stay within the board house's constraints, they guarantee that the board can be made as you designed it. There are actually quite a few more constraints than OSHPark mentions on its website, but the ones listed are sufficient unless you are doing something with more stringent requirements.

    For example, here is the capabilities document from Advanced Circuits. Notice there are specs for everything(!), but you won't care about most of them :)

    Personally, I try not to push the limits of the board house unless I have to. OSHPark will give you 6-mil trace/space on a 2-layer board, but I'd use 10-mil or greater unless you're running out of space.

  1. Assembly

    If you use standard packages and footprints, you usually won't have to worry about solderability. The footprints will have soldermask which will help control the solder and minimize solder bridges.

    Once you dig into it, surface-mount footprints have a concept called "density", which is defined by IPC-7351 as "most", "nominal", and "least". These terms refer to how much copper is exposed for a given pad. If you need a really tight design, the pads shrink down and you can cram the parts closer. If you don't have space constraints, the pads can be bigger. This helps hand-soldering and it makes rework easier. It's hard to hand-solder a "least" footprint!

    If your tool gives you the options, "most" is really nice for hand-soldering. Many tools don't give you the options, but instead default to something close to "nominal". This should be fine.

    There is a free program, PCB Library Expert, which will construct footprints for you which conform to IPC-7351. It allows you to select different density levels, and works with many PCB software packages. The website is here. The free version has advertisements.

  1. Electrical Integrity

    This is a huge subject which can't be covered in a single question (or a single textbook). I've been doing boards for years and I keep learning new stuff. I'll mention just a few things to get you started:

    The very first level of concern is simply current-carrying capability. Thicker traces carry more current :) If you Google "trace width calculator" you'll find numerous free resources. There are other reasons to use thicker traces such as minimizing trace inductance, but they won't matter in many circuits.

    Also, the space between traces needs to increase as the voltages increase. Google "pcb creepage and clearance".

    Another thing to consider is cross-talk. Electrical fields created in one trace can couple into neighboring traces. This effect increases as the traces get closer together, and as the signalling rates increase. A good rule of thumb is to have 3*w space between traces, where "w" is the trace width.

    Cross-talk can easily minimized by putting a ground plane under all the traces on a different layer. Especially if you have a 4-layer board, you can fill an entire inner layer with copper which will give many types of benefits.

OK, that's enough! Good luck, and ask questions here as they come up :)