8 ms·
What's the deal with square traces on PCBs?
- abetusk 7y agoTLDR "conventional" wisdom about square traces having adverse effects on introducing noise for high frequency lines turns out to be negligible. Instead square traces were/are frowned on because of acid pooling from the etching process for making PCBs.
- deleted 7y ago[deleted]
- deleted 7y ago[deleted]
- Hendrikto 7y agoWhy does the author keep saying “square”, when what he actually means is “right angle”?
- OJFord 7y agohttps://en.wikipedia.org/wiki/Try_square https://en.wikipedia.org/wiki/Try_square
- roland35 7y agoI think a few PCB layout tools refer to 90 degrees as square, but you are correct!
- alanbernstein 7y agoadjective having or forming one or more right angles or being at right angles to something According to https://www.dictionary.com/browse/square https://www.dictionary.com/browse/square, this is British usage, but I've often heard and used it in the US.
- compiler-guy 7y ago"Square" is used all the time in manufacturing and crafts to mean a right angle. https://en.wikipedia.org/wiki/Steel_square https://en.wikipedia.org/wiki/Steel_square
- kijin 7y agoThe image at the top of the article shows a number of traces that look like they're trying to climb a steep hill. I don't know much about PCB design, so my best guess is that those squiggles are trying to match a certain latency. But if 90-degree turns are so meticulously avoided in the industry, why is it okay to do multiple 180-degree turns in quick succession?
- DanBC 7y agoThe reason those traces are shaped like that is to keep them the same length as some other trace. This question has some answers: https://electronics.stackexchange.com/questions/74789/purpose-of-wave-shaped-pcb-traces https://electronics.stackexchange.com/questions/74789/purpos... Designers would say that none of those corners are right angled, and that they each have a bit of bevelling.
- bookofjoe 7y agoWhen I (non-techie) first read the title, I thought this post would be about strange shapes on chromatography results measuring pesticide residues.
- dillonmckay 7y agoThis made me laugh. PCBs can come from PCBs, though. It is a valid interpretation.
- DanBC 7y agoYou can fit more in if you avoid 90 degree corners. You have shorter traces too. Also, auto-routing exists so most people aren't handcrafting these corners.
- EmpirePhoenix 7y agoUm wait, the main reasons for I know about is, that square corners are a huge issue with higher currents, as they tend to burn from the inside out, due to the lower resistance in the corner and non equal flowing of electrons.
- SJSque 7y agoI don't know about PCB level, but on smaller scales you should avoid making right-angle turns in metal lines because of electromigration [1]. Energetic electrons flowing along the line will crash into the 'wall' at the turn, and will knock the atoms out of place a little bit. Over time, this will lead to 'erosion' of the corner. [1] https://en.wikipedia.org/wiki/Electromigration https://en.wikipedia.org/wiki/Electromigration
- ajross 7y ago> on smaller scales you should avoid making right-angle turns in metal lines because of electromigration Someone needs to tell the semiconductor industry that, then, because all traces inside a modern IC are at 90 degrees. The whole chip is just a big array of parallel lines in two orientation that get cut by photolithography to form circuits. The vias between levels are 90 degrees too, of course. It's certainly true that electromigration is going to concentrate more at tight bends. But in practice if it isn't killing your 7nm interconnect you're... probably going to be fine with that 1 mil trace that is a million times wider.
- jgeada 7y agoThe reason it isn't killing that 7nm interconnect is that those semiconductor physical implementation designers run lots of EM simulations to determine the reliability and lifetime of all traces, taking into account the trace dimensions, electrical properties and the expected current flows and the design is only signed off when those metrics meet or exceed the design requirements. Note also that specialized metals (tungsten, ruthenium) are used on really fine lower level traces of advanced nodes, due both to their resistance to EM as well their better compatibility with silicon (smaller passivation thickness).
- ajross 7y agoI think you missed the sarcasm. Electromigration is simply not an issue for PCB design, period. The relative scales of the devices are separated by many orders of magnitude. The effect wasn't even discovered until photolithography pushed scales to values much smaller than we see on even the tiniest printed circuit. Maybe, just maybe, there's a high current, high voltage board out there with tiny traces that was designed with some kind of trivial electromigration mitigation. But if there is, I've never heard of it. And electromigration is absolutely not a reason to avoid 90 degree turns on your digital logic board, don't be ridiculous.
- roland35 7y agoAnother important consideration is ease of routing signals during design. Using 45 degree corners in general produces pretty space-efficient routing that makes it easy to cluster signals together as well as move them if necessary during layout. One point the article left out is the risk of traces lifting off of the board. Having less sharp corners seems to reduce the risk of this happening with components that have a mechanical risk of coming off (like USB connectors, or large capacitors).
- femto 7y agoI avoid right angle turns on the theory that the sharp exterior corner increases the risk of the copper foil peeling away from the substrate.
- iamkroot 7y agoYeah this is the only explanation I've ever heard. It's the same reason why you avoid acute angles in the design.
- russdill 7y agoNearly every single pcb designer uses square pads with 90° corners.
- coryrc 7y agoPads are much longer than the width across the smallest corner, so if it gets rounded a little, there's no problem. But a 90° corner for the thinnest trace is vulnerable to being etched from all sides and getting too thin.
- taneq 7y agoThere are a lot of good technical arguments raised here but the real reason we don't use right-angle bends on the 90% of PCBs which aren't carrying serious current or running at GHz is that right angles look ugly.
- roland35 7y agoYou can't fix ugly! There is nothing better looking than a beautifully laid out PCB
- cnvogel 7y agoHere's a paper that shows reflections (Fig. 3, "S11") and insertion loss (Fig. 4, "S12") on coplanar waveguides, when using a sharp 90° bend, a 90° bend with a champfer and the case where the bend is replaced by two successive 45° turns ("final design"). The frequency scale spans 10..90 GHz. http://tentzeris.ece.gatech.edu/ECTC09_Rida.pdf http://tentzeris.ece.gatech.edu/ECTC09_Rida.pdf
- scld 7y agoYah anyone who has done RF engineering knows that "just a little bit of capacitance" can be a lot of capacitance.
- baybal2 7y agoIf you are in RF, you may well be already using "cornerless" smooth traces. Google "topological router"
- superkuh 7y agoThat or using discontinuities in impedance intentionally. I've designed and had built a handful of successful UHF planar PCB filters using Sonnet. In a lot of them I use very small changes in trace width as the place to put resonating elements. ie, http://superkuh.com/stepped-impedance-bandstop-filter.html http://superkuh.com/stepped-impedance-bandstop-filter.html The difference between square corners and compensated is real. And it gets more real if you're working in generic FR4 with 1.6mm thickness and 2-3mm wide traces for the sweet spot between 50 and 75 ohms.
- ajnin 7y agoThe "final design" is the chamfered bend with additional vias, a design with two 45° bends was not studied in this paper. Page 2, second paragraph of section A : > The final design that includes both the chamfered bend and the vias
- IndrekR 7y agoYou can play around with this type of simulations quite easily. Have been using free version of Sonnet planar EM solver [1] for this over the years. Helpful in developing the industry standard magic RF intuition. [1] http://www.sonnetsoftware.com/products/lite/ http://www.sonnetsoftware.com/products/lite/
- srfilipek 7y agoFor simple and slow communication busses on hobbyist boards, sure it probably doesn't matter. But I really can't trust this very superficial attempt to prove a negative with regards to a very complex phenomenon that I do not think he understands, especially since he mentions nothing about inductance, reflections, or impedance changes. Hell, RF experts with decades of experience will still find new corner-cases and issues with PCB layouts when it comes to analog signals. In terms of "actual wisdom" regarding 90 degree traces: Some time ago at my job we had to actually scrap a PCB because of right-angle traces causing too much interference. The end effect was a comb filter on the signal and a ton of emitted RF interference. TLDR: Yes, the phenomenon is real. Do not trust these hand-wavy attempts to dismiss it.
- everybodyknows 7y agoFirst sign of the author's confusion: >a square of copper two millimeters on a side has the same resistance as a square of copper ten millimeters on a side. It’s counter-intuitive. The phenomenon is perfectly intuitive for anyone who understands DC resistance of metals, and the geometric assumptions of the "sheet resistance" thought experiment. Resistance is proportional to conducter length divided by cross-sectional area. For a sheet conductor, cross-sectional area is thickness times width. A necessary assumption, unstated in the article, is that the hypothetical test circuit somehow makes perfect, uniform electrical contact over the entirety of both of the sheet's chosen "width" edges.
- madengr 7y agoI take issue with this article. Electrons do bunch up on sharp corners, as far as high voltage design is concerned. Sharp corners cause inductance when the current has to “turn the corner”. An infinitely sharp edge would have infinite inductance. Think of a charge having momentum, and the H field the result of that momentum. You can’t just change it. This is more troublesome at RF due to the currents crowding at the edges of the line, where the path length is now different for inside and outside radius, irrespective of lumped discontinuities. In the RF world we mitre the bends, and sometimes used swept bends. The swept bends supposedly radiate more than mitered, but have not proven that to myself. The case where you do want sharp, 90 degree bends are on electrically small monopole type antennas. The inductance will compensate for the high capacitive reactance of the antenna.
- aswanson 7y agoHave you ever done a design specifying molex connectors?
- madengr 7y agoMost have a Molex brand connector, though nothing > 50 VDC. I use a lot of the Molex Pico-Lock connectors, and similar sizes; all board level stuff. What I was revering to in the above post is the susceptibility to breakdown and corona discharge from sharp edges (example at link below). I have done some static E field modeling in CST for HV breakdown in potted modules. https://www.comsol.se/paper/modeling-of-avalanche-breakdown-in-silicon-and-gallium-nitride-high-voltage-diod-66642 https://www.comsol.se/paper/modeling-of-avalanche-breakdown-...
- markus92 7y agoWhat I've been taught during my EE studies, is that the main reason to avoid square traces is for EMC reasons, mainly due to reflections due to the hard boundaries. Interesting that the article doesn't touch on that. PCB design/layout is one of the more important factors influencing EMC. Taking it into account early in the PCB design phase saves you a lot of trouble during certification.
- krapht 7y agoThe article obliquely touches on it by mentioning how square bends affect the trace resistance and capacitance.
- crististm 7y agoYeah, it dances around the corners. Pun aside, signal reflections are the main reasons not to do it in high bandwidth circuits. Other circuits may have different reasons. I'm surprised about the hand-wavy way of ignoring a very well understood phenomenon.
- leetbulb 7y agoNot an EE by any stretch, but I've always thought this was the primary reason.
- russdill 7y agoReflections are caused by changes in impedance, not direction. The impedance at a 90° corner changes because there is more area which increases capacitance.
- krapht 7y agoHuh, article says not to worry about traces unless dealing with 100 MHz+ signal lines. Isn't that very common? Hell even the MSP430 is running at 25 MHz these days. And for all the other reasons listed in the article, you should avoid sharp corners. It's lazy to do otherwise when mitred 45 degree bends or curves are so easy to generate in a CAD tool. It's the hardware version of a code smell - the board house (compiler) might not care, but it should be fixed - don't give up freely obtained manufacturing slack because you couldn't set up a trace bend rule. I kind of feel like PCB layout ought to just be done by the antenna engineers for any serious product with wireless comms or high speed I/O.
- IshKebab 7y ago100 MHz in traces is very uncommon for typical DIY PCBs. The only place I can think you'd get that is in a microcontroller clock, but most people use modules or internal clocks.
- yetihehe 7y agoOr a 8mhz crystal and PLL in mcu.
- philpem 7y agoIt's not just the fundamental frequency that matters -- a square wave with fast edges will have harmonics which lead off to a surprisingly high frequency. Even on fairly slow signals they can be into the tens or hundreds of MHz.
- nitrogen 7y agoOr USB 2.0 if you are using a USB-capable microcontroller.
- IshKebab 7y agoUSB 2 High Speed support is still rare in microcontrollers. Most still only support Full Speed which is only 12 Mb/s. (If anyone is looking for this btw the best option I found is Atmel's SAM ARM microcontrollers, e.g. as used in the Arduino Due.)
- the-dude 7y agoMeanwhile, in Soviet Russia, traces square you : https://en.wikipedia.org/wiki/TopoR https://en.wikipedia.org/wiki/TopoR
- bcaa7f3a8bbc 7y agoHow do you ensure the proper requirements for routing analog circuits, high-speed digital circuits, or RF circuits are satisfied in a freestyle routing?
- fouronnes3 7y agoInteresting. I really enjoy manual routing though. For a small board it can be a fun game :)
- the-dude 7y agoI self taught PCB design a couple of years ago, settled for KiCAD and freerouting(.net). After the prototype revisions, it was very easy to move to 100% SMD and let the autorouter do its job ( design for manufacturing ).
- roland35 7y agoMy only problem with the auto router (in EAGLECAD at least) is that it ruined your undo/redo history! So basically if it screwed up you had to tear the entire thing up, or go back to an old save. It still is a huge time saver though!
- 7y ago
- gorio 7y agoSquare corners seems likely to be less space efficient, which is one consideration of pcb design. Why we don't use round corners or fluid traces might be a better question.
- roland35 7y agoRound corners are nice but the radius is constantly increasing so they do not stack as well as 45 degree corners. This is especially difficult when you have to move a group of signals together during design!
- philpem 7y agoAcid trap was the one I kept hearing, and proved true on my home-etched PCBs. The 90-degree traces would get undercut but the 45-degree ones were fine. To be fair it's less likely to be an issue with more advanced etching processes, but there are still limits. The thicker the copper layer, the wider your minimum track and gap widths become, otherwise the copper traces are excessively undercut.
- childintime 7y agoRelated: looking at the main image, there are lots of places where traces routinely deviate to go around a pad, with an extremely low clearance, needlessly so. The designer probably took a defensive approach: the traces have been routed to leave as much space as possible to easily allow additional traces in the same gap. So to me this pcb is a rough draft, an unoptimized initial version. The optimization obviously wasn't worth any time (and I agree with that), but I think an EDA tool worth its price should take such a design and optimize it. Such details really aren't the job of a designer, but still have the potential to significantly improve a layout.
- IndrekR 7y agoOn this board it looks like just a functionality/beauty thing and does not matter much. But depends on the target. While for the pads I agree, spacing can be optimised, then for the densely routed areas space is your friend. At higher frequencies (shallow skin depth) most energy is guided by the trace, but transferred in the space. Traces become bounds of transmission lines along what transverse electromagnetic waves are propagating. This is the reason why dielectric constant and dielectric loss matter a lot at higher frequencies; and why good impedance matching is needed for efficient energy transfer. EMC/EMI/RFI is mostly energy management issue.
- amelius 7y agoConclusion: > The reason we don’t see square traces in most PCB designs is simply due to aesthetic convention. If it looks wrong, it is wrong. There is no specific reason why every circuit board design should shy away from 90-degree angles on traces, it’s just something that you shouldn’t do because it looks wrong.
- jiveturkey 7y agoIt does matter for RF, as TFA says. So the tools do it for you. Since it's automatic and easily done with the tools, everyone just does it. Sure, you don't have to shy away from 90° but you also don't have to avoid it. I strongly disagree with "looks wrong". It's simply an aesthetic choice, there is no right or wrong about it. I wonder if they did this kind of optimization back in the day when traces were hand-taped. The sensitivity is to rise time, not actually frequency, so even for the slower designs of the day, maybe 45° or arced corners were still useful?