NO ! You don't need to worry about 90 degrees corner at PCB trace - Page 1
Forum section: electronics / general

author: BravoV
author_rank: Super Contributor
timestamp: March 02, 2013, 07:50:15 pm
content: ... unless you're going to play with a signal faster than 15 ps edge rates.Although this issue was asked by Dave and already clearly answered by Dr. Howard Johnson at TheAmpHour, also its mentioned in Howard's very popular book "High-Speed Digital Design: a Handbook of Black Magic".For those who do not have Mr. Johnson's book but still want to read some technical details related about this, there is another source of excellent paper regarding this matter.Book title : Right Angle Corners on Printed Circuit Board Traces, Time and Frequency Domain AnalysisAuthor : Mark I. MontroseThis paper is widely available in the net, just search it and you will got tons of links, and example link just in case you're lazy to google->HEREPS : Found this info while reading from one of Texas Instrument's recent app note on Stellaris system design guidelines.

author: free_electron
author_rank: Super Contributor
timestamp: March 02, 2013, 09:25:24 pm
content: YES, you need to worry about them. Sod those 'black magic experts !' They may know all the theory in the world an be able to solve Maxwell by hand, but they have never had to ETCH a board ...Sharp corners are acid traps and lead to underetching causing possible opens in traces. Especially on layers that are sparsely populated (large area's of copper that need to be removed with thin traces running over long lenghts)Of course they are right it doesn't matter for signal integrity, heck inside Ic's the traces are all routed using right angles.... Actually it does matter, if there is underetching you creat local impedance discontinuities... and those may impact.but signal integrity is only 1% of the entire board design... manufacturability weighs much heavier.what good is a perfect board signal integrity wise if noone can actually make it ? or if it has a yield of 1% ...by the way i have followed the course given by Montrose at UCSC ( university California Santa-Cruz) Passed with an A+ ..

author: Unknown
author_rank: Unknown
timestamp: March 02, 2013, 10:20:38 pm
content: I know this is a problem for hobbyists etching in their garage, but is it still a problem for the much more refined professional processes? I would expect them to have sufficient mixing to overcome this problem.

author: Marco
author_rank: Super Contributor
timestamp: March 02, 2013, 10:23:16 pm
content: AFAICS you certainly don't need 15 ps signals to see the effects.http://www.millertechinc.com/pdf_files/mti_tn063_microstrip_right_angle_bends.pdfLets say you use 3 right angle bends with microstrip on a 0.8 mm FR4 PCB ... that's around 5% reflection for a 100 ps risetime step signal.

author: AndyC_772
author_rank: Super Contributor
timestamp: March 02, 2013, 10:25:22 pm
content: Quote from: free_electron on March 02, 2013, 09:25:24 pmWhat good is a properly manufactured board which, by design, won't ever work correctly because the SI is inadequate?

author: JoeyP
author_rank: Frequent Contributor
timestamp: March 02, 2013, 11:22:34 pm
content: Quote from: alm on March 02, 2013, 10:20:38 pmYou're right. I've talked to PCB vendors about this, and they claim acid traps are a thing of the past due to improvements in modern processing. They told me not to worry about them at all.

author: MetraCollector
author_rank: Regular Contributor
timestamp: March 03, 2013, 12:03:32 am
content: All in all - are there any manufacturers nowadays that use acid etching ?Modern facilities use alkaline etching at all, this way of etching is not invasive and cover majority of PCB manufacturing.

author: Neganur
author_rank: Unknown
timestamp: March 03, 2013, 05:35:34 pm
content: Quote from: Marco on March 02, 2013, 10:23:16 pmI can't follow their paper. They claim on page 3 of the document you linked, that at 1 GHz "the skin effect is pushing the current to the outside edges of the microstrip" and illustrate it with a picture from a simulation. Why only the edges? The skin depth for copper @ 1 GHz is 0.0821 mil (2.085 µm) while the thickness of a trace for a 1 ounce copper-clad is 1.34 mil (34 µm). There is plenty of surface on that trace - not only at the edges at 1 GHz.The trace dimensions are weird. 8 mil trace width, 4 mil dielectric (uh what?) with a dielectric constant permittivity of 4.353 (apparently FR-4). I'm assuming 1 ounce per square foot copper since they don't mention it anywhere.Then that graph of S11 and S21, where it is said that "the reflection from a single right angle bend is less than 3% up to 15 GHz". Unless I'm mistaken, their graph shows an input port voltage reflection coefficient (S11) of about -50 dB at 1 GHz, which is about 0.3 % reflection. Why would three 90 degree bends be 5% ?

author: BravoV
author_rank: Super Contributor
timestamp: March 03, 2013, 06:14:29 pm
content: Neganur, thanks for the findings ! Learned new things here !

author: ddavidebor
author_rank: Super Contributor
timestamp: March 03, 2013, 06:33:26 pm
content: If fact, nobody kill you if you make a 90 degree tracesBUTWhy you have to? Is ugly and un-professional

author: free_electron
author_rank: Super Contributor
timestamp: March 03, 2013, 06:55:40 pm
content: Quote from: alm on March 02, 2013, 10:20:38 pmit is still a problem, especially when you get to geometries smaller than 4 mils and want to use thick copper ( 1 ounce)@andy_c ; you can at least start debugging....Note that this paper deals with both EMC and SI. But, you have to read it correctly.SI may not be impacted unless you use fast rise times , but things change when you have to do other elements.They investigate a single trace .. what about differential traces... where time-of-flight becomes important , like GDDR5 or DDr4 memories. you can't escape the rounded corners because you create a length imbalance..what about traces that are used to carry ANALOG signals ? what these guys have done is studied the impairment of a DIGITAL ( a fst rising edge) signal.... remeber that unobtainium oscilloscope i played with ? go take a look at the pictures of the hybrid used in that machine. it's all rounded traces , because you can't inject distortion! the scope would be unusable as it woudl falsify the signal.another thing is that these guys used striplines (transmission lines) with adequate rf return path... try this without return path and you are dead.things like crosstalk have not been studied. This paper deals with a single line above a ground plane. make that a 30 bit bus like for a fast memory and you end up in the pot with boiling water...You have to read this kind of paper and see it in its context.@metracollector. In the pcb industry all etching is done using Sodium or Ammonium Persulfate both of which are salts i believe and acidic in nature (ph)Howard Johnsons : High Speed Digital Design: A Handbook of Black MagicMontroses : Printed Circuit Board Design Techniques for EMC Compliance: A Handbook for DesignersLee Rithey : Right The first time : a practical handbook on PCB and system designespecially the last one is useful as it contains the practical ramification of the theory, and how to solve the problems arising with them.

author: Marco
author_rank: Super Contributor
timestamp: March 04, 2013, 09:25:26 pm
content: Quote from: Neganur on March 03, 2013, 05:35:34 pmThat was for 0.4mm dielectric thickness and it's about sinusoidal signals, I looked at the numbers on page 5 which concerns itself with step edges of a given rise time and looked at the numbers for 0.8mm dielectric thickness.

author: Smokey
author_rank: Super Contributor
timestamp: March 04, 2013, 11:37:28 pm
content: Thanks FE. "Right The first time" looks like a really good practical book. I'm seriously going to tear into that one later. I know I've been told a lot of PCB rules of thumb that probably won't hold up and it will be really good to get those myths busted by real data.The link to the free PDF for volume 1 is:http://www.thehighspeeddesignbook.com/PDF technical books like this are one of the reasons I'm thinking of getting a tablet. I do have to cringe at the thought of how long it is going to take to get through 639 pages though. It takes me a really long time to get through technical books with this much good info. I hope my lady friend doesn't want to see me much for the next couple months.

author: BravoV
author_rank: Super Contributor
timestamp: March 05, 2013, 09:15:20 am
content: Quote from: free_electron on March 03, 2013, 06:55:40 pmOk, since you mentioned this book, quotes from above Lee Ritchey's book at chapter 25 .....Right angle bends do not cause signal integrity problems at any practical edge speedRight angle bends also do not cause EMIRight angle bends areNOTacid trapThere is no good technical reason to prevent the use of right angle bends to route traces in a PCB."Vias used to route signal from one layer to another do not have a significant impact on signal quality even with 200 ps edges."PS : Not claiming an expert, its just these experts are very convincing don't you think ? And please don't shoot the messenger, I'm just quoting them.

author: Neganur
author_rank: Unknown
timestamp: March 05, 2013, 10:33:26 am
content: Quote from: Marco on March 04, 2013, 09:25:26 pmTwo points though:The graph is for rise times of digital signals, not sinusoids. You can apparently approximate the equivalent sine wave frequency of a digital signal by dividing 0.5 with the rise time, i.e. 0.5/100 ps = 5 GHz. Using this approximation, a 1 GHz sinusoid would correspond to a 500 ps rise time. Using their graph (between the 330 ps and 1 ns curve), I estimate the reflection at a dielectric thickness of 32.5 mil (~0.8 mm) to be approximately 0.01.A reflection of rho = 0.01 corresponds to a return loss of 40 dBm, which is incredibly good.Very interesting paper. I didn't realise they were referring to multilayer PCBs, which was why I was podering the thickness of the dielectric. The 4 mil dielectric thickness the paper refers to must be something like a 1.6 mm thick 12 layer PCB (5.1 mil FR-4, 4.67 mil pre-preg, 1.38 mil copper).But yes, according to your link you start to see reflections in 90 degree bends with 0.8 mm FR-4 and 100 ps rise time digital signals. I guess that's also a reason why multilayer boards are used so much today.EDIT: forgot to say where the 500 ps came from

author: ddavidebor
author_rank: Super Contributor
timestamp: March 06, 2013, 05:55:57 am
content: So if you don't need to worry all the engeneer that work on antenna in board application are all stupid?

author: Neganur
author_rank: Unknown
timestamp: March 06, 2013, 07:01:17 am
content: I don't understand your question, could you rephrase?

author: ddavidebor
author_rank: Super Contributor
timestamp: March 07, 2013, 09:19:48 am
content: All the datasheet that spoke about something that need hight frequency signal on a pcb had wrote "dont make any square trace for the signal part of the circuit"

author: BravoV
author_rank: Super Contributor
timestamp: March 07, 2013, 09:21:42 am
content: Quote from: ddavidebor on March 07, 2013, 09:19:48 amHow high ? All ?Give us one example, just one.

author: ddavidebor
author_rank: Super Contributor
timestamp: March 07, 2013, 09:37:51 am
content: Gps for example.

author: BravoV
author_rank: Super Contributor
timestamp: March 07, 2013, 09:39:37 am
content: Quote from: ddavidebor on March 07, 2013, 09:37:51 amWTF is that ? Just give us the link one of the datasheet you claimed, just one of MANY ..... how hard is that ?

author: ddavidebor
author_rank: Super Contributor
timestamp: March 07, 2013, 09:40:58 am
content: The first that came to my mind is ublox lea-XX gps module

author: westfw
author_rank: Super Contributor
timestamp: March 08, 2013, 07:42:35 am
content: QuoteQuoteWell, GPS is one of those 2.4GHz RF things. 2.4GHz is a period of 416ps, if I did my math right, so it may in fact have "edge rates" approaching the 15ps that the original article talks about. Go ahead and follow the suggestion for avoiding right-angle trace bends.But, pretty much ALL the time, I see hobbyists asking about their first PCB, using a 16MHz microcontroller or something, and people respond "get rid of those right angle bends." And that's a bit ridiculous...

author: lewis
author_rank: Frequent Contributor
timestamp: March 08, 2013, 10:20:20 am
content: Right angle traces look shit. Given the choice, why would you use them?

author: ddavidebor
author_rank: Super Contributor
timestamp: March 08, 2013, 04:10:22 pm
content: It's not ridiculous...

author: Tepe
author_rank: Frequent Contributor
timestamp: March 08, 2013, 04:34:25 pm
content: Quote from: ddavidebor on March 08, 2013, 04:10:22 pmAs a blanket statement it is cargo cult science. You need to qualify your claim.

author: ddavidebor
author_rank: Super Contributor
timestamp: March 08, 2013, 09:55:18 pm
content: Never a hobbist that learn to do thing in the better way is ridicolous...

author: jeroen74
author_rank: Frequent Contributor
timestamp: March 08, 2013, 10:05:54 pm
content: GPS is 1575.42 MHz and it's RF, not a digital signal with higher harmonics. The Ubloxhardware integration manualindeed mentions not to use Manhattan style routing.And, right angle bends just look ugly.

author: Unknown
author_rank: Unknown
timestamp: March 08, 2013, 10:19:39 pm
content: Quote from: ddavidebor on March 08, 2013, 09:55:18 pmShould we also tell them to use controlled impedance traces, since these provide better signal integrity and EMC at GHz frequencies?

author: ddavidebor
author_rank: Super Contributor
timestamp: March 09, 2013, 06:03:54 am
content: Teach him to di Fourier T. With only his mind.

author: BravoV
author_rank: Super Contributor
timestamp: March 09, 2013, 07:09:40 am
content: C'mon guys, thats ain't learning, just stop feeding the troll, clearly he is enjoying taken bait. Ignore list updated....Adolescente fastidioso e ritardato.

author: ddavidebor
author_rank: Super Contributor
timestamp: March 09, 2013, 11:37:10 am
content: The conclusion is in fact everytime the same90 degree traces are stupid thing to doEven for CC!

author: Zero999
author_rank: Super Contributor
timestamp: September 20, 2013, 12:01:47 pm
content: Quote from: MetraCollector on March 03, 2013, 12:03:32 amDoes it matter whether acids or alkaline substances are used? A corrosive substance is used to etch the PCB and right angles would have the same effect regardless of the pH.

author: SArepairman
author_rank: Frequent Contributor
timestamp: September 20, 2013, 05:02:12 pm
content: I will implement exclusively right angle design from this point forward. It looks better.

author: WarSim
author_rank: Frequent Contributor
timestamp: September 20, 2013, 06:15:31 pm
content: I am kinda surprised by how much of the real reasons have been lost in the "rule of thumbs" mentioned here.Every "rule of thumb" is a rule for a situation, some of the rules are quoted but very few situation. None of the "rules of thumb" are applicable in all situations.The 90deg rule situation factors are:PCB board manufacturing. (Not an issue with modern board shops, is an issue with DIY methods).Frequency/signal strength. With a direct energizer problematic frequency (around 2-5GHz) is much higher that without a direct energizer(around 1-3GHz). (Not an issue for almost all digital boards, they in general have direct energizers and under 500MHz)Frequency/signal integrity. Dependant of frequency spectrum. A simple frequency would have a higher frequency limit. (In general only an issue with low energy mixed composite signals)Frequency/strength/emissive. This is when the EMI effects are important. In all other cases other general "rules of thumbs" are used to compensate. The trace geometry is a significant factor for RF design.Signal integrity. If a design need matched traces and the differential limit is very low 90deg corners should be avoided or synchronized. This statement is due to pseudo angles calculations. For enterprise routers this is not an issue anymore because the software will perform the calculations for them (some require an extra RF design module/licence). For anyone else non-synchronized sharp angles become more difficult to calculate.These are "rules of thumb", yes there are exceptions. I could have missed a few that I don't use very often.

author: free_electron
author_rank: Super Contributor
timestamp: September 20, 2013, 06:47:08 pm
content: Quote from: WarSim on September 20, 2013, 06:15:31 pmYou obviously have never made a board for mass production using any kind of 'modern technology' like HDI interconnects or flex.Yes it is not a problem as long as you stay above 4 mil track and gap. once you go to high density and still want to maintain 1 ounce copper it becomes a problem again. Start working with fineline BGA (0.8mm ball pitch and below ) , flipchip and other modern technology and it does become problematic again.It's not only acid trapping. also the photoresist is problematic. the sharp corners peel off easier during scrubbing for example.As with a lot of things in electronics the only correct answer is 'it depends'.

author: WarSim
author_rank: Frequent Contributor
timestamp: September 22, 2013, 05:30:33 am
content: Quote from: free_electron on September 20, 2013, 06:47:08 pmI do agree with you. Yes my generalization did omit these factors. I considered a 4mil isolation and deep ratio geometry to be exceptions to my generalization.Feel free to point out the many exceptions to my generalizations. There are many exceptions and I would prefer not to explain all of them.I was just trying to give a starting point not supply a deaf to standard. I find that the answer of depends is not very helpful without a common starting point.

author: free_electron
author_rank: Super Contributor
timestamp: September 22, 2013, 07:22:46 am
content: The current state of miniaturisarion in electronics is moving is to a whole new playing field. Manufacturing rules that were applicable for a long time need to be revised as scale of geometries changes.An ipad logic board uses 2 mil traces.... There is not a lot of wiggle room there. Given it it as 10 or 12 layer board.... You do not want to mess it up so the rule is : no corners below 135 degrees . If a T junction is necessary the junction needs to be reinforced with a triangle. All trace to pad connections need teardropping and so on.There are documents availble specific for HDI board technology.Of course for a run of the mill home etch with 8 mil tracks it dont matter much. Go below and trouble starts.

author: BravoV
author_rank: Super Contributor
timestamp: September 22, 2013, 07:26:00 am
content: Quote from: free_electron on September 22, 2013, 07:22:46 amI don' deny that, the problem we always see is the arguments that the right angle affects "signal integrity" while talking at few measly Mhz level signal or worst at audiofool circuit, thats the reason I find its so annoying.

author: Mechatrommer
author_rank: Super Contributor
timestamp: September 22, 2013, 08:00:24 am
content: talking about manufacturibilty. why dont we just comply to whatever rule the manufacturer provides and STMITAFU?

author: free_electron
author_rank: Super Contributor
timestamp: September 22, 2013, 03:59:38 pm
content: Quote from: Mechatrommer on September 22, 2013, 08:00:24 amBingo.And for corners the manufacturer will only start specifying this for HDI (high density interconnect)

author: Nerull
author_rank: Frequent Contributor
timestamp: October 07, 2013, 09:55:39 pm
content: Quote from: ddavidebor on March 08, 2013, 09:55:18 pmIf you do something without knowing why you're doing it you haven't really learned anything at all.

author: WarSim
author_rank: Frequent Contributor
timestamp: October 08, 2013, 06:29:09 am
content: Quote from: Nerull on October 07, 2013, 09:55:39 pmVery true but very common.

author: itdontgo
author_rank: Regular Contributor
timestamp: January 24, 2016, 04:05:52 pm
content: I know this is an old topic but I thought I'd see what the internet's opinion of right angle traces is. I'm not buying the don't use right angles because of acid. Everytime your trace joins a pad there is a right angle unless you also use nice round pads (nobody uses round pads).Please see the picture!

author: Neganur
author_rank: Unknown
timestamp: January 24, 2016, 04:54:40 pm
content: The issue has a whole different dimension, it starts with 90 degree corners of your pcb outline...!!!On a serious note, it's not the fanout that was the issue being discussed but the trace bend. If you're worried about fanout there's this thing called tear-drops.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 24, 2016, 07:02:16 pm
content: Often, when a design goes into production, they'll ask about adding teardrops and send a check file. Automatic is usually fine. They know what they're doing.I do sh*t like this all the damn time:Officially speaking, it saves space, but as you can see, there's no space saving needed here. It's technically slightly worse for signal quality, because the tight grouping will increase coupling between traces (which isn't relevant in this location; this is also a 4 layer board, so the dielectric is thin and coupling is low). I just like the way it looks.Tim

author: CatalinaWOW
author_rank: Super Contributor
timestamp: January 24, 2016, 07:16:48 pm
content: I'll throw my hat into the it usually doesn't matter ring. But add another exception that requires some attention. If you have a very high current density and need long life, any discontinuity in the trace requires attention. Necks, bends, whatever. Obviously the best solution is to make the trace bigger so there isn't such high current density, but sometimes there are other alligators in the swamp.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 25, 2016, 03:35:31 am
content: I've seen induction heating coils where the inside corners burn out like that -- with seriously thick copper melting away, it's a nice graphic illustration of how strong the effect is. And it doesn't make itself better, only worse: once the inside corner melts, the metal beads up (or gets pushed out of the way by Lorenz force), making the inside corner even sharper, concentrating current further, and pretty soon you get a jagged burn path radiating out from the inside corner.For specifics: this is typically > 1/8" (3mm) copper, brazed together ("silver soldered", but not "silver bearing" (soft) solder), with water pipes nearby (usually no more than 1" (2.5cm) from the edges, where current flow concentrates). Frequencies 20kHz to 400kHz, currents of one to several thousand amperes.You'll notice skin effect is quite shallow in comparison (<< 10% of the thickness): the bulk of the metal is basically thermal only. A necessity for things this powerful!A typical bus bar for these sorts of things might be 2" wide, and nasty things like this were typical when the design engineer forgot to put a proper miter or curve on the joint.Tim

author: free_electron
author_rank: Super Contributor
timestamp: January 25, 2016, 04:36:15 am
content: Quote from: itdontgo on January 24, 2016, 04:05:52 pmHave you looked at the footprint requirements for DFN and likes ? IPC7351c explicitly calls to only use rounded rectangles or oblongs for pads.Teardropping mandatory. Sharp corners also have mechanical problems. When a oard is subject to vibration : that is where it will crack.As for rounded rectangle pads : the corner pullback is 12 to 20 %. The reason is the good wetting of solder. When dealing with very small pads solder does not flow in the corners.-

author: eetech00
author_rank: Regular Contributor
timestamp: February 05, 2016, 04:07:35 am
content: I don't know if its done anymore but back in the day right angle traces could cause solder bridges during flow soldering of the PCB.I imagine that any fab or assembly process that uses a liquid flow over the board might have trouble with right angle traces.Anyhow, its easy enough to not use right angle traces with today's modern PCB design tools so why even use them.just saying...

author: jwm_
author_rank: Frequent Contributor
timestamp: February 05, 2016, 07:25:02 am
content: Quote from: lewis on March 08, 2013, 10:20:20 amWhat? They have a fantastic retro look to them. All tron like. Bendy tracks are like blue leds, were rad for a while because you couldn't do them before so it screamed modern. The novelty wears off.

author: DerekG
author_rank: Frequent Contributor
timestamp: February 05, 2016, 12:02:15 pm
content: Quote from: free_electron on March 02, 2013, 09:25:24 pmHaving being involved in many designs that have been mass produced in overall runs of several hundred thousand, I agree with free_electron.When a track break is located, it is normally found at a right angle (simple right angle or T junction).Quote from: BravoV on March 05, 2013, 09:15:20 amWith finer pitch & thinner tracks now possible due to improved manufacturing materials & techniques, I suspect that Lee Ritchey would amend his older views if he himself had been involved in the mass manufacture of modern boards.

author: MT
author_rank: Super Contributor
timestamp: February 07, 2016, 12:37:23 am
content: Any experienced power RF engineer would ask for your CV if served a 90 degree trace intended to carry power RF signal!

author: LukeW
author_rank: Frequent Contributor
timestamp: February 16, 2016, 06:13:54 pm
content: Just in terms of PCB fabrication, ignoring issues like transmission line design and impedance control, just find a fab that agrees that they can manufacture to whatever design rules you want.If they specify 4/4, then do your layout to 4/4 rules. If they specify 4/4 and no right angles, then follow that.Personally, I have never ever seen the so-called "acid trap" breaks happen, either in a professional fab or in a competently performed kitchen etch, working to realistic design rule limits that you can expect from kitchen photolithography (let's say about 8/8 or 10/10).If you and the fab are both working to the same mutual understanding of what the acceptable design rules are, and they can't successfully fab as specified without breaks or shorts in the finished copper, then don't take your business there again.

author: metacollin
author_rank: Contributor
timestamp: March 22, 2016, 10:38:34 am
content: The simple truth is that it doesn't matter. At all. It never did. Why isn't anyone asking where 45 degree traces came from in the first place? If you look at circuit boards stretching back in time, most had completely freeform traces that were hand-taped out with rubylith, and often you'd see right angles as well, and there was clearly no effort being spent by anyone on making the traces have or not have right angles, or anything else. They just wanted to get the shit done. There was no solder mask on the early boards, the etching process was the same photosensitization process used at home for years by hobbyists.It never mattered and it still doesn't.I'll ask the question that everyone should have been asking (and everyone has yet to ask): Why did 45 degree angled traces become the norm?They never became the norm per se. No one was trying to use 45 degree angles (and no one was trying not to - because it didn't and still doesn't matter). The only significance behind 45 degree angles was, and always has been, little more than a sign of how it was designed. A board designed using computer aided design software would have nothing but straight lines, going in one of 8 directions. 45 degree angles often, but not always present given those constraints. A board that wasn't designed with a computer would be all curves, like you see topological autorouters create now. You'd also see sharp corners at any angle, it was really whatever was most easily cut out with rubylith. Very early boards did seem to make an effort to minimize very sharp edges, but entirely at the masking level, rounded right angles were routed all the time. Or worse, 120 degree angles or sharper.Exhibit A, a board which was from an old HP Frequency Synthesizer. It was fully enclosed and shielded extensively, it is an output filter with a bazillion stages. Made in the early 70s:It was much easer and less computationally intensive to only have to deal with 8 possible directions. Originally, 45 degree angles was a sheer compromise that was necessary when CAD layout tools were in their infancy. Just like how raster graphics were pixelated, so too were vector graphics simplified and lacked curves. Any board around this time will not only lack any of the curvy stylings of hand-taped designs, butfeatured 45 degree and 90 degree trace angles without any preference because they had 8 directions to choose from and they used them. No one cared about right angles or 45 degree angles.. In fact, looking at any layout, its obvious that the only thing that dictated when right angles or 45 degree angles were used or not was trace density. You can maintain a constant width of a group of parallel traces using 45 degree angles, while using right angles will require square-root of 2 more width when corning a group of traces. So, basically, designers used trace angles in the way that made sense.Exhibit B: A board when CAD boards were more or less the norm, but being used by people who still remembered a time when there were no software aids - 1983. This is a disk controller board from Western Digital, ©1983. A good year - engineers used reason, rather than the mix of that with superstition and tradition that seems to have taken ahold of many engineers today.Also, here is an oscilloscope. Hand taped. Lots of curves but also sharp T junctions and hard corners to be found all over. It's almost as if the designer didn't give a shit about the angles of his traces (hint: he didn't).A few other points:1.Every via IS A RIGHT ANGLE.Where is your diagonal god now?2. Every through hole lead meets at aRIGHT ANGLE.3. Every layer of every SMD chip capacitor is connected at, you guessed it, aRIGHT ANGLEto its end terminations.4. If you're using FR4, then angles don't matter. If you're using FR4, it means whatever you're doing is slow or short enough to tolerate the dielectric loss, which means it will tolerate right angles. Yes, it can matter for somethings, but it doesn't matter for you. (If you're using FR4 I mean.) And you'll be dealing with things like the parasitics created by the gap between two pads, the height of ceramic capacitors (1206s? YUCK, 1.2nH from the termination height alone! No good! 0805? 800pH! Terrible! If you've never thought these things, then I promise you that you don't need to think about the angle of your traces. And you probably don't even if you have thought about capacitor termination inductance.)5. This is the single biggest point:When angles actually do matter,45 degree angles AND 90 degree angles are totally incorrect!!Youneveruse them, and they are equivalent in terribleness. High speed signals don't care about corners, they care about discontinuities in impedance. Sharp impedance changes and sharp corners have little to do with each other. Besides both using the same adjective. A right angle bend introduces a sudden decrease in impedance due to the width of the micro strip suddenly widening to ?2 times the width, due to the corner. Two 45 degree angles change the width by...if my geometry serves me.... (ugh we need LaTex on these forums) square root of (4- square root of 2), or about 1.08. Twice. While the magnitude of the discontinuities is smaller than a right angle corner, the right angle corner introduces one discontinuity, and one source of reflection and what have you. The 45 degree angle has lowered the magnitude but now you have two reflections instead of one. Personally, I would not favor either outcome over the other. Do I want to die by bear or by tiger? *shrug* Either way, I'm still getting eaten alive and pooped out some animals butt.You have to use smooth curves with a radius of at least 3 times the width of the trace, or when you can't, you calculate the optimal amount of mitering you need to do to preserve the impedance. What you wind up with, and this is hilariously ironic, is a corner that is simultaneouslya right angle and 45 degree angle.That's right, even in the very specific cases where it does matter, the correct way is the perfect juxtaposition of the very thing being argued over.Personally, I value my time enough that I don't spend it worrying about things that don't actually matter, and completely ignore any thoughts about traces being this angle or that. At least, when I have that luxury. When it does matter...well, it doesn't, 90 degree angles are fine as long as they are mitered correctly, otherwise a 3w curve. I use whatever cornering works best in a given layout, and that's all the thought that needs to be put into it. There are more important things to think about. Hell, gossip about the Kardashians is slightly more important than worrying about the angle your traces are cornering at. Some arbitrary software decision decades ago has bizarrely turned into tradition for some. Yes - tradition exists even in engineering. And that is ultimately all there is to 45 degree angles. Tradition. Use what you prefer.

author: Warhawk
author_rank: Frequent Contributor
timestamp: March 22, 2016, 12:37:34 pm
content: Amen

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 23, 2016, 12:26:31 pm
content: Quote from: metacollin on March 22, 2016, 10:38:34 amYou circled the wrong things...Those are all very near 90 degrees.Check the mounting holes along the left side...QuoteYup, those are good examples. There's one more style you missed:Japanese boards, which I assume are designed for minimal copper waste? Most any stereo/TV/monitor/VCR/DVD/etc. has such an example. This is the kind of thing:http://4.bp.blogspot.com/_SPwX1vYEKqg/TVLLhwmwGvI/AAAAAAAAFoY/HrZVukSDr_Y/s1600/IMG_3711.jpgIt's not obviously made from polygons and traces, much more freeform, but definitely CAD in origin. Seems to emphasize negative space.QuoteUh... so? Those are all sealed, as-manufactured corners. The only concern anyone's ever had, at any time in history, is etching and acid trapping. None of those solid inside forms are made by subtractive process.That said, theystill are concerns, but not because we cando anythingabout them. We're stuck with it. It's up to the PCB manufacturer to get it right.Problems include surface and inner layer copper tear-out during drilling, incomplete plating (particularly to inner layers, and inside the barrel of high-aspect holes), and cracking/peeling during handling, soldering, storage (moisture, thermal stress), etc.Also, soldered inside corners aren't sharp, they are fillets. Check with a pocket loupe or microscope!QuoteWell no, I know of many people who do picosecond* pulse circuits on FR4. The edge is a little sloppy due to loss and dispersion, but the Q factor is low (it's just a transmission line, not a resonator) and as long as the edge still reaches your receiver intact (e.g. ECL or LVDS), jitter stays good.*Meaning it's a whole number of picoseconds for the edge, i.e. 1-999. Usually these sorts of things bottom out in the 20-100ps range. Edges of that speed are capable of resolving bend and via mismatch.RF boards need low-loss materials because they depend on the board for reactive power. Matching networks are built into the board, so a real fraction of signal power is handled by the board materials; actually, not even a fraction, but a multiple, because resonant power (VARs) goes up with Q, which is usually >1 for such things.QuoteHaven't been watching? \$ We \,\, have \,\, \mathrm{ \LaTeX } \$ .QuoteYou overestimate the importance -- there is no unique structure, and this one is only known because it is relatively easy to study. Simple geometry and all that.Likely, it is one of those cases where the bandwidth is extended a modest amount, but not the optimal amount. I would imagine softening the corners, and perhaps removing notches or bites from suitable locations, would get closer to ideal.The problem has three aspects:1. Current prefers to flow along the inside edge, so the rest of the corner looks like a capacitive flag tacked on: a reduced impedance. This implies taking a circular bite from the inside corner would have a similar effect as chamfering the outside corner, but would lead to more even current density.2. The inside edge has a shorter path length. Normally this doesn't matter, but "bandwidth" of a trace is determined by the point where higher order (waveguide) modes join in: frequencies where the trace width itself becomes significant. This implies that the geometry of the edges quickly becomes significant, and a profile shaped to focus reflections (like a reflecting prism, but in 2D) would be necessary. (Of course, a prism is quite large relative to the wavelengths it handles. Such a structure might not end up any better than a "gradual curve" method.)3. The traces are closer together along the inside corner. That is, the distance between traces, along a diagonal, is less than the propagation distance along the electrical trace. No it won't be much, along most of the trace -- but also apparent is that this will be significant right at the inside corner.Differing propagation modes is already a problem for microstrip: a fraction of the energy propagates in air at the speed of light, while most propagates in the PCB at a lower velocity. (This leads to more dispersion than dielectric loss causes, which is why it isn't much of a problem to use FR4 over RF types. A higher quality dielectric doesn't solve this problem. Buried stripline is required. But multilayer construction is even more expensive to fabricate in those materials, so it's even more of a burden for little advantage.)Of course, coplanar waveguide with ground, or stripline with via walls, does a good job of shielding those diagonal paths, but it takes more space too.Or, as most engineers do, you can simply ignore the problem altogether. Use thinner laminates and narrower traces, pushing the waveguide modes to ever-higher frequencies where you don't have to worry about them. A radio at 20GHz might be reasonable on a precision PCB, but doing one at 40 or 80GHz requires laser-etched hybrids, or monolithic ICs at still higher frequencies. Back in the 70s, a GHz sampling oscilloscope was reasonable on PCB; 10s of GHz models are built on hybrids, and 100s of GHz models are monolithic (using such esoterica as nonlinear schottky transmission shock lines to generate <20ps sampling pulses).Tim