Unwritten list of DFM "don't" and "do" - Page 1
Forum section: electronics / general

author: nuclearcat
author_rank: Unknown
timestamp: June 30, 2020, 03:29:30 am
content: I noticed that many PCB manufacturers are talking about DFM, and many things are not obvious and wont be checked by DRC.Like this list (taken fromhttps://www.autodesk.com/products/eagle/blog/top-10-manufacturing-mistakes/), some questions i will comment here.#1 – Not Leaving Enough Edge Clearance(Probably good idea)#2 – Making Acid TrapsMany are leaving question, is they are still a thing or depend on manufacturing process? Like this acid trap.#3 – Placing Vias in PadsI think i saw such thing recently, someone complained in twitter about JLC, while he placed vias in pads.#7 – Using Multiple Tool SizesIs it still a thing? Sure it is bad idea to use many Via sizes, but way it is done in Kicad, it is already hard to define many sizesI saw also somewhere recommendations how to attach traces to pads, especially if many traces are connected to it:Not sure if it matters for reflow PCBA.Maybe worth to try to make a more complete list of such "design" recommendations?PCB manufacturers suggestions are welcome, as it will reduce their pain with losses on failed, poorly designed boards.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 30, 2020, 05:07:31 am
content: 1. Altium at least supports rules for edge clearance, and most other mechanical features, or electrical features on the same layer.2. Acute angle is also on there. AFAIK, acid trapping isn't a problem these days; personally, I just avoid it because it's ugly. Smooth your routes, it's called artwork for a reason?3. Assembly issue. Can be accommodated, or mitigated; generally not recommended. Fab alternative: filled and capped vias ($$).7. I like to keep the number of drill items short. Given the tolerance (or house tolerance if you don't specify!!), they'll just bin everything into the nearest sizes they have; it's your problem whether that still fits or not. Best practice, specify tolerance and check it against the real components. Follow proper mechanical drafting practice!??. Thermal relief is not one that Altium for instance has, and even some enterprise DFM tools (e.g. Valor) don't always get right. Best to keep a watch for this while you're working -- repour polygons from time to time and check if they're drawing more spokes to some pads than there are traces on the other pads.Only affects chips (R, C, etc.), particularly small ones (0603-). Larger ones tend not to tombstone, and more pads, tend not to twist or tombstone. Tombstone, head-on-pillow and such failures are the main issue, a production yield problem.Don't go nuts with thermal relief. You don't need teeny spokes on every damn pad. Conversely, don't go nuts against it. You don't need solid pours all around the pad, basically anywhere. Go ahead, calculate the thermal resistance of average sized spokes, I'll wait! -- We should be so fortunate, to work in a field where so much (in principle,everything) can be calculated directly, or at least modeled! -- you'll find that the effect on thermal resistance isn't too much, a few °C here or there, while the improvement in soldering is substantial (both reflow and hand soldering). Basically, soldering delivers much higher heat flux, and takes a smaller temp drop (most of the board is already near soldering temp, in reflow), than is the case for heat dissipated by passive convection.I normally scale spokes, so that the clearance (pad to pour) is whatever, 10 mils say, and the spokes are 4 x 10 mil width. Thinner for small SMT pads (under say 20 mil width), wider for larger pads (say 20 for >70 mil pads, 30 for >150, etc.). This keeps everything from 0402 chips to D2PAK thermal pads readily solderable.And you can always double down, in those few cases where you need more.Example: a D2PAK can dissipate almost 10W on a conventional 4 layer board, maybe even 2 layer (2oz copper). To pull it off, you need solid pours -- no spokes -- on both sides, and lots of vias to bring the heat between them.Moreover, the vias can be filled with solder, reducing their Rth almost in half. (Yes, solder is a poor enough conductor that a via fully loaded with the stuff, barely performs better than the hole lined with just a thin foil of copper! BTW, lead-free is better in this respect; in general, alloys conduct worse than their constituents, and SAC305 has much less alloying than Sn60.) Bonus points for via-in-pad, but only if the assembly is reasonable -- for example, maybe you can't ensure adequate reflow of a D2PAK with tons of via-in-pad on its tab, but maybe they get filled on a subsequent wave soldering step. (Or if you're doing it by hand, just flood the bastard, eh?)Finally, now that you've got the heat spread out on both sides of the board, clamp it between two heat sinks, with thermal pads. Thermal pads aren't great either (typically 1 W/(m.K); though 3, 6, even 10 and higher are available these days!), but you're using a wide area of them so it works out.FR-4 itself is mediocre on conductivity, in-plane, and downright dismal thru-plane. The lateral thermal conductivity is about, what was it, doubled or so? by pouring copper on the outside, and obviously, that much more still with inner layers. Thru conductivity is dominated by vias; the only case where FR-4 is acceptable is when it's already very thin, like traces and pads to inner planes. (Indeed, this is enough conductivity that trace ampacity is increased markedly -- double or so -- when routed over inner planes!)Tim

author: phil from seattle
author_rank: Super Contributor
timestamp: June 30, 2020, 05:34:31 pm
content: Most of the items on the eagle list are reasonable. Good for beginners to hear though most of us who have been designing PCBs for a while know them. The last couple are kind of in the category of "check your work, dummy". Maybe they ran out of specific stuff to make 10 items.The "fat trace to a pad" thing seems wrong to me. That basically becomes a fuse. I size my traces to carry the expected current. Why would I shrink it down in one spot? if 10 mil is good enough, I'd run the entire trace that width. I've never seen that on any PCB, by the way, and I look at a lot of them. Thermal relief makes sense for pads connected to planes but that still needs to have enough width for a given copper thickness to carry the expected current. Maybe that is from the days when 10 mil traces was pushing the envelope.

author: asmi
author_rank: Super Contributor
timestamp: June 30, 2020, 05:51:55 pm
content: The top item on my personal DFM list is - don't ignore thermal aspects of your design! I've seen way too many boards (and sadly some of those were designed by me) that like to cook themselves over time if left unchecked. Solving thermal issues is much easier during design and layout, than inventing all kinds of band-aids once the board is already assembled, not to mention that end result will not look like hedgehog if designed properly from the ground up.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 30, 2020, 06:10:41 pm
content: Quote from: phil from seattle on June 30, 2020, 05:34:31 pmIt's an old style thing, I think. You wouldn't see it on consumer stuff at the time, since that was largely wave soldered, and single sided at that. You see it on some military gear, and I think Tektronix did that in the 80s. Like my TDS460, it's laid out weird, most components have short thin connecting traces and vias immediately taking the connections down to planes or inner routing. Very little is routed on surface layers. Almost no silkscreen, either (partially a consequence of non-serviceable boards).As for necks -- see above, we should be so lucky that we can calculate these things! Namely, when it comes to ampacity, there's two things: heat generation, and heat dissipation. Necks don't matter much because, while they do dissipate more power, they are heavily heatsunk by everything around. Ampacity is only important over longer lengths. And also like I mentioned, inner planes can more or less double the ampacity, thanks to the higher heat dissipation.Tim

author: HHaase
author_rank: Regular Contributor
timestamp: July 01, 2020, 03:24:13 pm
content: For mixed technology boards, watch your clearances around thru-hole components. It drives me absolutely bonkers at times trying to create nozzle paths for my select solder machines. Some assemblies I see have 0201 passives just packed right up to the thru-hole connectors, maybe only 1-2 mm clearance or so. Heck, I've even seen SMT parts placed BETWEEN pins on a thru-hole connector. Give yourself room to work!Multi-sided assemblies are pretty common, and really not a problem per-se, but does drive up process costs if you have two sided SMT placements and things of that nature. If it's possible to put all your parts on one side of the PCB, it dramatically simplifies the overall process, and can be a huge cost reduction.Do an actual paper print of your board design too, and make sure you can read all your silkscreens. You'd be surprised how often component designators and polarity markings are unclear.

author: E-Design
author_rank: Regular Contributor
timestamp: July 01, 2020, 04:12:37 pm
content: Ditto all the above comments..Additionally, dont forget that when you decide which PCB vendor you are going to use.. go get their design rules.You will find constraints like minimum holes size and the usual clearance stuff. Sometimes you may find one or 2 things that are a unique constraint to them or a preference. If you make their life easy, they will go easier on your wallet.Plus, its an eye opening experience to play around with quoting the board different ways (if you have the time to do so) - you will learn where the price sensitivities are (like making too small of holes or too small spacing etc). Those kinds of things usually indicate they have yield problems due to pushing limits of their process/machines. So there is standard DFM and then sometimes it can become more specific to the vendor. You should be motivated to find out.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 01, 2020, 04:31:46 pm
content: Quote from: HHaase on July 01, 2020, 03:24:13 pmA good rule of thumb is 150 mils (4mm) away from THT pads; this gives ample room for solder shield or selective solder. Well, or maybe more for SS alone, I don't know, depends on the nozzle I suppose.More specifically, last enterprise-grade DFM I used, this was tuned to a clearance cone around the pad -- thus, 0402s can be closer than 0805s, etc. (This would not be the case for a selective solder nozzle alone!) It's my understanding, they can make do with even tighter, but at some point, it goes from a cheap (composite based?) shield, to something insane like titanium jig plate.Tim

author: phil from seattle
author_rank: Super Contributor
timestamp: July 01, 2020, 04:41:33 pm
content: Quote from: HHaase on July 01, 2020, 03:24:13 pmThis! I will even go so far as to do a mockup - print it 1:1, glue it to a piece of Styrofoam and insert the TH components looking for physical interference and legibility of the SS plus an eye to possible rework issues. When working with CAD, I find it sometimes hard to get a sense of the actual assembly process so that helps too.

author: asmi
author_rank: Super Contributor
timestamp: July 01, 2020, 05:23:13 pm
content: Quote from: phil from seattle on July 01, 2020, 04:41:33 pmAlso when you do so connect all cables and other external stuff that is supposed to be connected, as some (most?) cable's side connectors are larger than corresponding board-side connectors. I've designed a board in the past which can not have 2 HDMI ports connected at the same time because there is not enough space for cable connectors.

author: phil from seattle
author_rank: Super Contributor
timestamp: July 01, 2020, 09:44:46 pm
content: Quote from: asmi on July 01, 2020, 05:23:13 pmYup. or at least size the connectors. But when it comes to cables, leave extra room for the connectors because some of them are amazingly fat.

author: Siwastaja
author_rank: Super Contributor
timestamp: July 02, 2020, 08:37:28 pm
content: Quote from: asmi on July 01, 2020, 05:23:13 pmFor this reason, when I'm creating 3D models of the PCB connectors, I simply draw the mating connector and even a bit of the wire exiting the connector, into said model itself (see attachment for the idea; in this case the color coding of wires also double-checks the pinout). Now the resulting 3D isn't strictly what you get out of PCB assembly shop, but actually more; it models how it looks like after plugging it in, which is what matters! Great for the mechanical designer to put into their CAD and verify.Speaking of which, creating the 3D models, do that yourself. Downloading from the internetz results in fancier-looking models because someone had a lot of spare time to make them neat, but they are often dimensionally wrong (because people focus on appearance over function). Your own models can be very simplified, as long as the simplification consist of "bounding boxes" that cover all the complex shapes.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 03, 2020, 01:33:48 am
content: Also dimensions can be wrong because they were drawn to MMC. Which can in turn be laughably wrong from the manufacturer, when they forget to put any tolerance at all on the drawing...3D models should be average dimension, for the most part, but it does depend a bit on what you're using them for (appearance vs. mechanical constraints).Tim

author: phil from seattle
author_rank: Super Contributor
timestamp: July 03, 2020, 02:00:42 am
content: Another unwritten rule - never trust any else's footprint, even if it came with the design tools. Always verify against the datasheet. I had a footprint that I had used numerous times for hand assembled boards. When I did a production run with reflow, I discovered that it was slightly crooked. Not enough to prevent solder surface tension from making it work correctly but having a bunch of ICs on your board that are slightly crooked is pretty embarassing.

author: nuclearcat
author_rank: Unknown
timestamp: July 03, 2020, 08:35:09 am
content: Quote from: phil from seattle on July 03, 2020, 02:00:42 amI had worse , relay footprint on 3rd party website was mirrored. It was hard to spot until moment i tried to solder it

author: langwadt
author_rank: Super Contributor
timestamp: July 03, 2020, 09:13:22 am
content: Quote from: phil from seattle on June 30, 2020, 05:34:31 pmI'd guess it is to make it more symmetrical so that the part doesn't pull or tombstone

author: SMTech
author_rank: Frequent Contributor
timestamp: July 03, 2020, 10:44:22 am
content: Quote from: langwadt on July 03, 2020, 09:13:22 amThat's exactly what its about it needs to balance both sides, of course it still needs to be rated to carry the current it needs to, sometimes I see boards where one end of the part is whacked straight on a plane of copper and the other side has a tiny trace, asking for trouble. It will be worse for DIYers with toaster ovens.