Changing Trace Thickness Reason - Page 1
Forum section: electronics / projects

author: Str1ker
author_rank: Contributor
timestamp: May 18, 2021, 03:48:34 pm
content: Hi, I bought myself a nixie tube clock kit from GRA&AFCH and on inspection of the PCB I noticed, that the trace thicknesses are changing (getting thicker near the pads). I have never seen such a design on other PCBs and was wondering if there is a good reason for doing so or if the PCB is just poorly designed... What is your opinion on this? Many Thanks!

author: penfold
author_rank: Frequent Contributor
timestamp: May 18, 2021, 04:03:33 pm
content: There are parts where it looks fairly logical, i.e. maximising the trace thickness where possible and reducing when you need to run a few close together... but places where it looks less logical.Where it meets a pad, it's typical to tear-drop or expand the trace width a little to avoid sharp corners on thin traces which are more likely to crack. Some historic problems with acid traps may have caused a tendency to design traces to be thicker at certain points over their length or at corners.

author: phil from seattle
author_rank: Super Contributor
timestamp: May 18, 2021, 09:42:30 pm
content: It is one thing to neck down to a narrower trace for a short run to squeeze between some things but fattening those traces for such a short distance makes no sense at all.

author: thm_w
author_rank: Super Contributor
timestamp: May 18, 2021, 09:52:01 pm
content: Quote from: phil from seattle on May 18, 2021, 09:42:30 pmAs penfold said it can help delay cracking, but yeah in this case not really necessary unless you expect the nixie tube to dance around.The one serious case of through hole cracking I've seen was on a keyboard, where the PCB is constantly being hammered upon and flexing. Most other cases of delam or cracking that I recall are SMD parts, connectors, or really heavy parts (transformers).

author: ejeffrey
author_rank: Super Contributor
timestamp: May 18, 2021, 09:56:41 pm
content: This just looks like amateurish PCB layout. There is nothing really wrong with it except that it is sloppy, but no good reason for it either, and I would prefer my PCBs not look sloppy because I don't know what else is done sloppy.

author: TimNJ
author_rank: Super Contributor
timestamp: May 19, 2021, 02:25:54 am
content: As others have said, maybe no good reason in this particular case. No reason to care about acid traps these days.To me, if there was a reason at all, it may be for better pad adhesion and to try to prevent pad "rip-out" during rework. For a through-hole lead, if the the annular ring is quite small, after a few attempts de-soldering, the pad might be gone. For a surface-mount pad, say on a QFP or similar, there's not much surface area holding the pad to the PCB, so a little extra area may keep the pad fixed to the board during rework.Similar to above, if you're designing a cheap single-sided board with crappy, low-grade resin (between copper and laminate material), adding some extra copper around the pad may give better mechanical strength. It is less likely for a through-hole lead to "push through" with some sort of mechanical stress or shock.

author: Wolfram
author_rank: Frequent Contributor
timestamp: May 19, 2021, 08:29:06 am
content: This is done to reduce the stress where the trace meets the pad. As far as I can see, these boards are made for mounting nixies via socket pins. Inserting the tubes into the sockets can take a lot of force, particularly if the pins are corroded or bent, which is not uncommon with new old stock tubes. If you have a single six or eight mil trace entering the pad, the stress of plugging and unplugging the tube can cause the trace to break right where it enters the pad.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 19, 2021, 10:25:47 am
content: Poor man's teardrop I guess?Reasons might include: increased heat dissipation, slightly increased strength, tapering trace impedance (on this scale, it would only be relevant to >10GHz designs), or uh, not much else I can think of, offhand?Teardrops are primarily used to connect to thru-holes, where the drill placement tolerance might reduce the pad (annular ring) to zero or negative (cutting entirely through the pad). When this occurs towards the trace, it can weaken or break the connection; the teardrop just adds a little extra meat around the trace to prevent that possibility.It's not really relevant for SMT pads, but I suppose it would increase strength slightly: tight inside corners are more prone to fatigue and tearing.Acute angles are also traditionally known to cause acid traps (trapping etchant chemicals, causing eventual corrosion and failure), but this isn't actually a problem on modern processes, AFAIK. Personally, I avoid doing it just because it looks ugly!Tim