Routing Questions - I thought I knew - Page 1
Forum section: electronics / projects

author: envisionelec
author_rank: Frequent Contributor
timestamp: August 09, 2018, 01:51:01 pm
content: I started working for a fairly large international company (you would recognize their products) and had a design review recently where I was called out for routing a trace under an 0805 pull-up resistor (circuit voltage 3.3V). Two engineers called it out and one said it was obviously bad design practice. I was pretty shocked considering it didn't violate DRC. They also complained that there were "acute angles" that cause acid traps. Now, I had heard of this one, but thought it was a non-issue these days. It's pretty hard to route a tight layout without incurring an acute angle, but I typically put in teardrops to eliminate this issue.Some of the arguments included tin whiskers, dendrite growth and just looking bad. Now, correct me if I'm wrong, but wouldn't fine pitch devices also have these problems if those things were true?Is this really a concern? How can I go about convincing them it isn't a problem?

author: Zucca
author_rank: Unknown
timestamp: August 09, 2018, 05:32:19 pm
content: It all depends, what are the EMI/working frequency, thermal situation of that board? Project specifications? Pictures?There are no general rules to be applied with closed eyes and turned off brain IMO.There is the good and holy theory which has to be implemented in every single situation/board.The more you know, the more experience you had/have, the more you will be create good/design board.PS: Never lose, either teach/win or learn

author: tomato
author_rank: Regular Contributor
timestamp: August 09, 2018, 06:00:17 pm
content: Quote from: envisionelec on August 09, 2018, 01:51:01 pmYou just started working for a large, well-established company and you want to tell them they are doing things wrong? Good luck with that.

author: DaJMasta
author_rank: Super Contributor
timestamp: August 09, 2018, 08:12:37 pm
content: I'd assume that their engineers know the manufacturing process they've used before and should be deferred to, I'd also assume they're being especially scrutinous of your work because you're new. Tin whiskers are more metallurgy territory, but they could be basically advising best-practice to minimize inevitable failures in production due to changes that can't be made (like getting different lead pitch on certain parts), again they've probably seen issues in products before and want to be careful to not have to spend the big bucks on recalls and replacements.So some of it is probably being careful to minimize risk of problems at stages they're hard to correct at, some of it is based on past experience with the process and designs, and some of it is being cautious of the new guy's work.

author: james_s
author_rank: Super Contributor
timestamp: August 10, 2018, 01:12:32 am
content: My advice would be put your pride aside and try to incorporate any suggestions they have, regardless of what you think of them. Go ahead and offer your opinion but don't keep pushing if they push back, and be open to ideas from the more established engineers. Eventually after you've been there a while you'll earn respect and have more leeway to do things your way.

author: rx8pilot
author_rank: Super Contributor
timestamp: August 10, 2018, 01:32:03 am
content: This is why I won't work for a large company.Many engineers MUST be right all the time - including the ones that are your boss.Many engineers worry about non-existent problems because they don't truly understand the manufacturing process or how things have changed since 1985Many engineers actually do know about finicky details that have burned them in the past and do not want to repeat it.Nearly zero engineers are willing to get a lesson from a new PCB designer - they are responsible for the sign off in the end.After some period of success and doing it their way - you can judge who is willing to have a conversation and who is not.

author: JS
author_rank: Frequent Contributor
timestamp: August 10, 2018, 01:34:25 am
content: 0805 is a pretty small package to put a trace between pads, you can fit it within standard DRCs but depends on the 0805 footprint as well, then consider the solder mask retraction, and you are not with a lot of space for insulation, you apply solder to it, there's no space underneath, little insulation, you might see a problem or two while producing hundred of thousands of those and it can be avoided reasonable easily unless you are in a single sided PCB and you shouldn't be using jumpers, so I see no problem with that restriction.Acute angles have always been called problems, many reasons why, for HF are really a problem, for LF the problem could be in the process, not so much for the signal, DIY, hobbyists, self etchers learn all this stuff in the hard way early on, when you start with manufactured PCBs you don't realize how or why the process constrains are there. Even if the process for self etch and big manufactures is quite different it shares many of the constrains in different scales. At home 8 mil rules are the limit, when I started I wouldn't be confortable under 16 or 20 mils your manufacturer might be 4 mils, but the process is pretty much the same, some resist material and etching, they have better tooling than I do.JS

author: james_s
author_rank: Super Contributor
timestamp: August 10, 2018, 01:49:53 am
content: Quote from: rx8pilot on August 10, 2018, 01:32:03 amThere are a lot of large companies out there and not all of them are like that. If one is new there though it's not unreasonable to have to gradually earn the respect of more experienced people. It's not all that unusual for some new guy to march in and think they know everything.

author: KL27x
author_rank: Super Contributor
timestamp: August 10, 2018, 02:26:37 am
content: QuoteI don't see why that applies specifically to a trace that runs between the pads. If you run the trace between 2 separate 0805's in such a way the spacing is the same, you could claim all the same issues, right? And you would change your DRC settings?I suppose flux residue stuck under the resistor or heat/thermal issue from the resistor can open up other cans of worms?

author: RoGeorge
author_rank: Super Contributor
timestamp: August 10, 2018, 03:13:17 am
content: Quote from: envisionelec on August 09, 2018, 01:51:01 pmThat is absolutely what you shouldnotdo. The reviewers are not attacking you, they are just guiding your work.Since there were 2 persons, and they also explained the concerns (whiskers and acid traps), you need to correct the design, and also keep in mind these best practices for the next PCBs.

author: ludzinc
author_rank: Unknown
timestamp: August 10, 2018, 03:14:01 am
content: Quote from: rx8pilot on August 10, 2018, 01:32:03 amMany engineers have lost $10,000's that they were responsible for and have learnt that lesson all too well.As me about an un-tented via underneath a transistor that saw me replace over 200 units in the field.....

author: Mr. Scram
author_rank: Super Contributor
timestamp: August 10, 2018, 03:21:31 am
content: You don't stand to gain anything from fighting this battle. If you get it your way you only risk being held responsible for any issues down the line that may or may not be caused by your design choices. Just accept this is their version of doing it right and do it how they want it. The only exception would be something where there's actually an issue with how they do it.Pick your battles.

author: krish2487
author_rank: Frequent Contributor
timestamp: August 10, 2018, 09:10:26 am
content: Disregarding almost everything what the existing engineers said about acid traps and EMI and anything else.Is it really so hard to redo the board just to avoid conflicts and make your life easier??You said it yourself, it should not be a problem. If you can make them happy, you are making your life easier.Just my 2 cents..

author: max_torque
author_rank: Super Contributor
timestamp: August 10, 2018, 02:41:20 pm
content: If there is no (zero cost) way of avoiding the track going under the component, then you need to assess the relative risk that this track creates.If you can simply move the track out from under the resistor (by using another layer, or re-routing the track, or moving the component) then that's what i would do.There's no point adding risk for little gain imo, even if that risk is low in absolute!

author: exmadscientist
author_rank: Frequent Contributor
timestamp: August 10, 2018, 04:37:43 pm
content: For what it's worth: my assessment of whether these practices are OK would depend mostly on the intended application, summarized in the IPC Performance Class. For Class 2 stuff (standard reliability), I don't see anything wrong with routing traces under components. I'd even consider vias under components to be fine in Class 2; things like putting vias under caps to create low ESL connections can be very useful. But if this is a Class 3 (high reliability) design, or higher, then the negatives outweigh the positives. The requirements for Class 3 are a lot more strict, and the process much more expensive, because the end application justifies it.And for Class 1 (low cost), it's fine if it waits until after it leaves the factory before catching on fireAcute angle routing traces, on the other hand, are not something I like to see ever. While modern processes have improved to the point where acid traps and tin whiskers are rarely problems now, acute angles are usually just a sign of routing sloppiness and can be trivially fixed. Usually when I find one, I don't worry so much about the angle itself as how much attention the rest of the nearby routing got... and I usually find something else I don't like nearby.

author: james_s
author_rank: Super Contributor
timestamp: August 10, 2018, 04:51:36 pm
content: I try to only use 45 degree bends whenever possible, weird angles just looks sloppy and whenever I see a board router that way I immediately think it was done by an amateur. It's the same feeling as looking in an electrical box and seeing that the outer sheath has not been stripped off the NM cable all the way back to near where it enters the box, it still works but it just says sloppy and inattention to details.

author: aandrew
author_rank: Frequent Contributor
timestamp: August 10, 2018, 05:27:56 pm
content: Quote from: ludzinc on August 10, 2018, 03:14:01 amOk, I'll ask. What's the story of the untented via under a transistor that saw you replace over 200 units in the field?

author: KL27x
author_rank: Super Contributor
timestamp: August 11, 2018, 02:23:41 am
content: ^Bridges? I'm curious, too.I have done this on accident on a production board, but I noticed it, immediately. I spent several miserable hours with kapton tape and an exacto knife.QuoteI am curious if the minimum DRC rules change enough to make this (trace under a resistor) impossible, or is it specifically prohibited in Class 3. And what is the failure mode? Also, is it equally prohibited to run a trace under an IC? Where's the cutoff? Surely it is ok under a DIP? An SOIC? A narrow SSOP? SOT-23?Obviously OP should say "thank you" to his senior for correcting his mistake. But I don't expect he will ever get a rationale explanation. Just the same smart-sounding non-answers that people post here.I checked a production board I have, and maybe I made my own footprint/library part. I can't remember. But there's soldermask between the pads. Maybe it's not supposed to be there?I've never needed to do this on a production board but I have several working boards I use daily for nearly a decade with traces between 0805 sized resistor pads... and no soldermask. The actual component on there is in some cases smaller, even, than 0805; though in this case it is hand soldered with a deliberate air gap.I was also under the impression that one of the reasons 0R resistors exist is to jump traces.

author: exmadscientist
author_rank: Frequent Contributor
timestamp: August 11, 2018, 04:48:00 am
content: Quote from: KL27x on August 11, 2018, 02:23:41 amIPC standards (which define the Performance Classes) don't cover DRC or fab rules; those things are agreed on between designer and fabricator. The standards are more interested in things like defining defects and allowable defect densities, so saying "Class 3" in this context is more shorthand than anything else. Usually Class 3 acceptance rules are specified when a failure would put someone's life at risk (e.g., automotive, aerospace, defense, medical life support, etc) or when truly giant piles of money are involved (e.g., space). Quite obviously that kind of work demands a higher level of performance, hence the very strict acceptance criteria for this class.As you point out, for normal use there's no reason not to run traces under components. (Though I personally don't do it without solder mask.) My guess is that the failure modes are along the lines of debris getting trapped at the edges of components combining with solder mask degradation to provide a potential shorting path. Solder mask is vulnerable to abrasion, so it's not hard to imagine chip components or low-clearance parts causing mask damage given some thermal cycling. But don't take my word for it, I don't think I've ever done a class 3 design!

author: KL27x
author_rank: Super Contributor
timestamp: August 11, 2018, 07:12:39 am
content: ^Well, if you have never done a class 3 board, and class 3 has nothing to do with DRC or fab rules, I'm curious why you suggest running a trace between 0805 pads is not kosher in a class 3 pcb? Is this a rule of some sort? If it is just your opinion, I wonder why you stated it so strongly, as if you agree with the OP's senior colleague. Telling someone this is "obviously bad engineering practice" is so devoid of useful information, it's mindboggling. At least you included some interesting/useful information, albeit, it appears to me to be completely tangential to the original point, lol.BTW, the OP stated the resistor is a pullup resistor to 3.3V. For say 10K pullup, that is 1.1mW. If anything, the presence of the resistor will protect the soldermask from damage.I can imagine OP running a trace under an SO-4 IC in the future. Is he going to get beat with a stick for not having learnt what is "obviously bad engineering practice?" What about a 2412 resistor? Does it matter if it were a size D tantalum cap? I mean, it's pretty much open to interpretation what the heck that means. A quick "why" would clarify a lot. Maybe an anecdote of that personal disaster of 1984...

author: Rerouter
author_rank: Super Contributor
timestamp: August 11, 2018, 08:47:57 am
content: I went digging without much success, as high reliability layout is something I try and keep up with.As Class 3 is "If Things fail, people can die" level of requirements, I take it as removing every possible risk,So my take would me the additional height of the solder mask over the copper trace would cause a bending force in the SMD component, which especially for ceramic capacitors can reduce reliability, by reducing the flex margin (how much the board can flex before cracks form)In the same case, it can reduce the margin of your paste re flow, if 1 pad melted first, the part would be see-saw'd away from the other pad, so if you had an untented via that sucked up most of the solder on that pad, it could leave it very marginal.I have to constantly keep it in mind for QFN packages, if you run traces under one, its better to fill Idle space with a supply rail pour so with solder mask the entire underside area is the same height than to have just the few squiggles causing pivot points. And ironically that solder mask thickness rise of the board can increase reliability as thicker solder fillets can better handle flexing.Acid Traps are something I rarely worry about these days, less that its still a problem, more so that rounded-rectangle pads, teardrops on Via's and trace neck down removes all but the weirdest issues. and unless your layout package allows spline like traces, 45 degree traces is a good compromise to give you more space efficiency than 90 degrees when you go High density.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 11, 2018, 06:41:59 pm
content: Funny, I've inherited a design from a Large Company You'd Recognize, and it's full of odd design decisions and ugly routing. (It's from a much smaller department, however, which is probably part of the reason why we've been called in to help.)FWIW, I avoid acute angles where possible, not because of acid traps but just because it looks ugly. Take pride in your work, create a masterpiece. Don't settle for "found art".Tim

author: Mr. Scram
author_rank: Super Contributor
timestamp: August 11, 2018, 09:49:27 pm
content: Quote from: T3sl4co1l on August 11, 2018, 06:41:59 pmIf it saves space functional "ugly" angles take preference over pretty but more space consuming angles. Take pride in coming up with the best solution within your constraints. If it doesn't make a functional difference then sure, go wild and shine things up.

author: james_s
author_rank: Super Contributor
timestamp: August 11, 2018, 10:11:51 pm
content: There are certainly exceptions, but in many cases the same rule of thumb that applies to airplanes tends to work pretty well with PCB layouts. If it looks beautiful, it will often work well.

author: KL27x
author_rank: Super Contributor
timestamp: August 11, 2018, 11:28:32 pm
content: The other thing with inheriting a design is maybe it wasnt finished? Altium is super snazzy and easy to reroute like an afterthought. In Eagle you are wasting your time about "pretty" until you are sure the components are in the most efficient positioning and exact locations, and the thing works.... and once it works, there is a saying. If it ain't broke...I appreciate esthetics in the housing and ergos of the device and the proper functioning and responsiveness of firmware. I don't too much care what the pcb looks like under a microscope. The engineer in me might think I could have done it smaller/cheaper or more reliable (on a level more significant than tin whiskers). Never did care too much about pretty, unless the ugliness increases the cost/area. And sometimes there's extra area on a board due to odd shape or housing requirements, anyway, where you could tighten up some things and reduce some area but it wouldn't decrease the cost... so go crazy in there. I don't care. I guess Sometimes I mix 45 degree angles and curves on the same board. I often operate on super fine snap-to just by eye, rather than grid. It's not until the very end I would even care if everything is perfectly evenly spaced or symmetrical... and I get to that point sometimes never, before new board revision requiring major changes.QuoteHaving etched a lot of my own boards, I have a pretty good idea of where acute angles are problematic. And it's pretty much nil on larger pitch boards 7+ mil. That said, if I see some ugly amateur routing, it might pique my interest. I see the other side of the coin. Examing the board, I might find some unique design decisions and maybe some easily identifiable components rather than inhouse numbers. And seeing how bad something looks and still works you learn more than seeing things made pretty for (possibly) no reason. And you can instantly have some idea of what the trace isn't for. If you find something you don't like, and the board works, anyways, maybe you will learn something.I do take pride in my work, but for me it comes down to primarily cost and reliability. I don't understand what end user/consumer cares about what the board looks like, and why should you? They care that the thing works. The contractor cares that he makes a profit, which includes ease of assembly, QA/testing, reliability, and cost. The cost to reproduce the board, not just your bill for making it pretty.I did a collaboration, once, per desire of my contractor. I did the firmware and worked with another hardware designer. Dude was mad skilled in Altium in making pretty traces like lightning. rRight before you eyes, he would paint a picasso of routing. Problem was he didn't bother getting the important bits right. Location of critical things like mounting holes and finger contacts. This company made insanely stupid mistakes, creating new prettier revision 3 times, WITHOUT BEING ASKED, every time making the board look cooler, more complex tab routing for no reason, cool graphic silkscreen, but improving NOTHING. At least once they made the fit to the housing WORSE where a press fit contact was, resulting in 90% fail rate. All the while, they refused to implement some changes I insisted would fix the biggest issues with the PCB; they had more experience and did it their way, which is great but it didn't work. Contractor thankfully didn't quite go bankrupt, and is now using my hardware. It costs less to produce and it brought the rail rate from double digits down to maybe 1%.

author: exmadscientist
author_rank: Frequent Contributor
timestamp: August 12, 2018, 07:55:28 am
content: Quote from: KL27x on August 11, 2018, 07:12:39 amSorry, I could have been more clear: I was trying to give examples of how odd restrictions (like no traces between chip passive pads, which I agreeisan odd restriction) can derive from unusual environments (high reliability being one example that came to mind).I fully agree with you that OP's colleagues should have explained thewhybehind the criticisms, and that for routine work they sound unreasonable. But without more detail about the design and environment, it's impossible to know what "unreasonable" really looks like.

author: Siwastaja
author_rank: Super Contributor
timestamp: August 12, 2018, 12:19:58 pm
content: Quote from: JS on August 10, 2018, 01:34:25 amBullshit.Maybe in 1985.Or maybe in a super-extra-low-cost made-in-batch-of-10000000-on-single-sided-pertinax-clad with 10/10 mil rules territory, but for anything else, putting one single trace between 0805 is normal everyday practice. It leaves massive margin for soldermask registration error before the track is exposed. Even without reliable soldermask, there is still massive margin for paste / placement error before there is a risk for a solder bridge.The same is true for 0603 as well! And yes - even for low cost production.There may be reasons not to do it, but these would be fairly specific.Tin whiskers are dealt with pad-to-pad DRC rule. Tin whiskers are totally irrelevant to this question.DRCs existexactlyfor this reason.I totally hate incompetent design engineers who cannot support their statements with technical arguments and resort to "it looks bad" things. Does it? I don't know, I think an optimally designed and functional PCB looks beautiful, and avoiding a few vias, possibly a break on a reference plane and a couple of extra stiching vias, would make this optimization look beautiful.This being said, putting traces between the pads of 0805 is 100% totally everyday and normal industry practice, and the arguments you get makes it sound like these engineers are not very experienced.There are reasons why I choose to work as a technology chief in a small startup, even though it's more uncertain and stressful at times.

author: Siwastaja
author_rank: Super Contributor
timestamp: August 12, 2018, 12:26:02 pm
content: Quote from: RoGeorge on August 10, 2018, 03:13:17 amSo, 2-1 voting wins, facts being totally irrelevant to the matter?You know, "whiskers" is not related to the actual thingat all- they just picked a random cool tech word they have heard.So, does "correcting the design" mean:1) make the design electrically correct, i.e., so that it works reliably, and can be manufactured easily, with good margin for error, or2) make the design suit randomly voted opinions which have no relation to any fact,if 2, what to do when the next day these random "rules" have arbitrarily changed?I fully agree you sometimes just need to do wrong things because you are told to, and get paid for it. This might be such a case. Do it as long as it's morally OK for you, as it is in this case.But don't lie to yourself about it. Keep questioning and learning while playing the "company game".

author: KL27x
author_rank: Super Contributor
timestamp: August 12, 2018, 01:06:15 pm
content: Maybe we're all looking at it the wrong way.If these are the only criticisms of OP's PCB, perhaps it was really a compliment.

author: RoGeorge
author_rank: Super Contributor
timestamp: August 12, 2018, 01:35:38 pm
content: Quote from: Siwastaja on August 12, 2018, 12:26:02 pmYou got it all wrong:- it is not about voting: One reviewer might mistake or might be too pedantic, two reviewers making the same observations most probably means the design has issues.- correcting the design means to edit the PCB in order to include the reviewers' change requests.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 12, 2018, 01:50:01 pm
content: Quote from: Mr. Scram on August 11, 2018, 09:49:27 pmI don't know of anywhere I've had to sacrifice space for gloss, but yes, that is part of the "where possible".Which, I suppose, might be a hint that, if you think it's too hard, it's not, just keep shoving and swapping things around until you find more space for placement and routing. Beyond the most trivial layouts, there is essentially no chance of findingtheoptimal layout -- there's always more space to save, just a matter of finding it. (Most cases, you don't have that time, so the project settles for "good enough".)Tim

author: RoGeorge
author_rank: Super Contributor
timestamp: August 12, 2018, 02:04:51 pm
content: Another reason for sharp corners to be considered "ugly" is because the electric field is way larger on the tip of a spike than on the rest of the conductor. This can created EMI problems.

author: NorthGuy
author_rank: Super Contributor
timestamp: August 12, 2018, 03:13:17 pm
content: Strange they use 0805 for new designs. May be they have special considerations for these boards. What do we know?Anyway, the problem is not technical. The problem is that you work for the company, you don't run things around there. It's up to you how to deal with that. Possibilities are endless.

author: Mr. Scram
author_rank: Super Contributor
timestamp: August 12, 2018, 04:47:20 pm
content: Quote from: KL27x on August 12, 2018, 01:06:15 pmYou're touching upon another phenomena; when experts are asked to check or review something, they often seem to feel they have to come up with something. You see this with auditing, design reviews or committees quite a lot. They don't find anything that's really a problem but still have to justify their role, so they'll come up with some small nitpick items. Generally this is a sign you did your job.I don't think people are consciously out to fabricate issues, but I do think there's a lot of different psychological phenomena in play that these people aren't quite aware of themselves.

author: Mr. Scram
author_rank: Super Contributor
timestamp: August 12, 2018, 04:49:33 pm
content: Quote from: NorthGuy on August 12, 2018, 03:13:17 pmMaybe the power requirements are such that smaller parts aren't quite suitable. Maybe they're taking the current component shortages into consideration. Maybe it's an inventory thing. Maybe it's just what they're used to.There's plenty of reasons not to go for the thing that would be the obvious choice.

author: rx8pilot
author_rank: Super Contributor
timestamp: August 12, 2018, 05:10:12 pm
content: Quote from: Mr. Scram on August 12, 2018, 04:49:33 pmI have a new design that has 0805 for all of those reasons..... power requirements, they are already loaded in the pick-and-place machine, I have a lot of them, and I am copy-pasting from previous designs/pcb layouts. I am slowly upgrading my P&P feeders and collecting more inventory 0402 parts to make the transition to smaller parts but it will take some time. Since I do a lot of power electronics - I have to use a lot of 0805/1206/1220 caps because of voltage/capacitance needs are not available in smaller packages.In the end - I have 0805 in new designs because it is known art and fast.

author: nctnico
author_rank: Super Contributor
timestamp: August 12, 2018, 05:58:41 pm
content: Quote from: Mr. Scram on August 12, 2018, 04:49:33 pmI agree. 0805 is also easy to inspect visually and rework manually. If board space isn't a problem then there is no need to switch to anything smaller.Regarding the OP's situation: I've been in similar situations at both ends. What is important is to try and understand the reasoning why someone thinks a design is not optimal. Any engineer should be susceptible to good arguments.

author: ludzinc
author_rank: Unknown
timestamp: August 12, 2018, 10:35:29 pm
content: Quote from: aandrew on August 10, 2018, 05:27:56 pmLong story short - the via connected to Vcc and the transistor it was under drove a buzzer.Leakage? Flux residue? No idea of the exact mechanisim but after a while the buzzers would turn on weakly and intermittent and drive the operator nuts.Fix? Remove SMD transistor and dead bug a through hole part in place. Ever since this, *any* via under any part I get tented.Been told many times it’s not needed. Best excuse not tondonit is that tenting can trap acid and the via can fail. It’s at that point you play the “if if fails, I wear the blame, do as you are told” Card.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 13, 2018, 03:35:43 am
content: Fabs prefer fully tented vias, or fully open vias. One-side tented, traps crud that outgasses and is impossible to wash.In your case: who knows? Corrosion from deposits? Nasty environment?Tenting does help with corrosion resistance. And if the post-assembly washing was bad, soaking that in conformal coating probably wouldn't help much.I prefer the best of both worlds: fully tented where possible, 'cheat' tenting when needing to be open. By "cheat", I mean soldermask 3 mils from the hole. It's not tented (mask in hole), but it's not useful as a pad (the annular ring is mostly covered). Most often, the need is testpointing, for which the bottom pad is open the usual amount, while the top is still 'cheated' in this way. This prevents the via from wicking solder if it's near a pad on the top side.Tim

author: envisionelec
author_rank: Frequent Contributor
timestamp: August 27, 2018, 04:57:24 pm
content: This generated a lot more discussion than I expected!The background is this project was an adapter board to be used in-house. Five parts; not high speed and not critical. I was trying to keep it cheap by going single sided so I routed a pull-up trace under a resistor.I am the senior PCB engineer with over 20 years experience - this isn't my first "major corporation" gig. I was just surprised that these guys were stuck in the 1980s. They are pretty "mom and pop" as far as PCB design goes. They certainly have a lot of experience, but without data to back up their findings. Just mostly a lot of "well, it worked after we did this so that's how we want it." And I'm totally fine with that, so long as I've got their desires on paper - not just through tribal knowledge.I conceded their points and had already made the changes to their desires by the time I posted here. I didn't fight it but I did ask about it - which is how I learned about their last PCB guy who was pretty awful and had pissed a lot of people off. So I get that - and I'm totally on board with doing it their way, but only as long as it doesn't cause manufacturing issues.Thanks for everyone's input!

author: free_electron
author_rank: Super Contributor
timestamp: August 27, 2018, 07:21:11 pm
content: Dendrite growth could be the issue.What cleanliness spec are you designing to ? Automotive ? Avionics ? Space ?Will they use soldermask ?Depending on where this board may land and how it will be fabricated it could be prohibited to route under 0805 parts.