No 2oz copper with JLCPCB assembly. Any alternatives? - Page 1
Forum section: electronics / general

author: superKris
author_rank: Regular Contributor
timestamp: September 29, 2020, 07:56:04 am
content: So i have been working for over a year on a project that is finally ready to be manufactured. Its a PCB with high current (40A) traces but there is also a high component count of approx 250 parts.For actual usage 1oz copper will be to thin. 2oz is just barely enough to support the 40A currents i have planned.Meanwhile, with 250 components its near impossible to assemble by hand. The hours and costs are to high, and i do not have te proper tools.And then there is costs. I build everything in easyEDA based on JLCPCB's assembled parts. Most of it is basic, and some are extended parts. A batch of 5 pcs 2oz PCB's will cost me around $ 30,- which is cheap enough for me. Assembly (through hole and some chips excuded) will cost me around $ 90,- This includes the componets and even the 1oz PCBS. Very cheap for 5pcs so this is absolutely fine with me.However, JLCPCB does not offer 2oz with assembly. I dont understand why, but they dont. I should have checked this earlier. I also send them a email just to check, but they replied its really not possible. This is a huge setback for my project.At this point i'm looking to make 5 prototypes to use myself and give to friends for testing. If the feedback will be good enough i want to maybe try to sell this product in the small community its intended for or make the full design opensource. This means i dont mind paying over 100,- but 500,- (for 5 boards) would be to much especially since this is only 1/2 of the project.Can anyone suggest a alternative manufacturing service that works in a similar way as JLCPCB does, but with the option of 2oz? This would also require a manufacturer with an (extended) list of components to choose from.

author: voltsandjolts
author_rank: Unknown
timestamp: September 29, 2020, 08:20:28 am
content: Perhaps the simplest solution is to go with JLC 1oz assembly then beef up high-current tracks with solder (leave mask off of those tracks).

author: GerardG
author_rank: Regular Contributor
timestamp: September 29, 2020, 08:38:26 am
content: Be aware when 2oz is on the edge of what you need.2oz will not be the exact thickness you will receive on a PCB.Normally the production will start with 1oz before plating. (plating 20µm according IPC)The option for adding solder to these traces is the easiest and oldest trick.

author: superKris
author_rank: Regular Contributor
timestamp: September 29, 2020, 09:22:26 am
content: Thanks you for the reply. I think there has been lots of discussion about adding solder to the tracks. If i'm not mistaking dave also did a video on this. While i'm sure it will help, i'm not so sure it will be enough to support the 40A currents i'm designing for.Here is some more info about my design and the tracks i'm talking about:https://www.eevblog.com/forum/projects/pcb-design-high-current-tracks-low-voltage-measurement-(please-review)/msg3223702/My own calculations show i need 2oz copper, but its hard to calculate with the weird shape of the tracks and all the via's. I think i will go for the 1oz option with exposed tracks if i can not find an alternative, but i would much rather pay (a lot) extra for 2oz.

author: tggzzz
author_rank: Super Contributor
timestamp: September 29, 2020, 09:34:28 am
content: Presumably there is a high current and a control section to the design.I would look at keeping the high current off the control PCB, and having control signals go offboard, possibly (but not necessarily) to a daughter PCB. There other advantages to that strategy.

author: Styno
author_rank: Regular Contributor
timestamp: September 29, 2020, 10:02:17 am
content: Why not export the design to Gerber and BOM list and use a more capable fab to manufacture your boards? In Europe; a lot of companies will happily have the board fabricated in whatever oz Cu you want (3 or 4 in your case?) and assemble them for you, though they will not be as cheap as JLC ofcourse and you will have to put much more effort in documenting your design but multiple options exist in the Netherlands alone.Aside from that, perhaps you can bend solid core wire into shape, feed it through high current via's and solder it onto the tracks?

author: Mechatrommer
author_rank: Super Contributor
timestamp: September 29, 2020, 10:27:08 am
content: Quote from: superKris on September 29, 2020, 09:22:26 am10oz will not be even enough! add thick badass wire or bar in parellel point to point... such example....if you want to get fancy, be creative...

author: superKris
author_rank: Regular Contributor
timestamp: September 29, 2020, 11:21:29 am
content: Quote from: tggzzz on September 29, 2020, 09:34:28 amThanks for your idea. This board however is mainly made for the sole purpose of replacing all wires and and loose components. Dual PCB's with a board to board connection however actually inst the worst idea. The main problem with this would be the SMD current shunts. Their output will be very low, and i want to keep the tracks to the current sense amplifiers as short as possible to prevent errors and noise. That means these IC's need to be the current PCB too including all the additional components. Its approx 10 parts per sensor, so thats still 60 SMD components that i would need to hand solder. The kinda defeats the whole purpose of a secondary PCB for power.Quote from: Styno on September 29, 2020, 10:02:17 amSure, finding a manufacturer that can do it will be very simple. Many company's here in the Netherlands that can do it, but i doubt there wil be one that can do a batch of 5 pcs under a 1000, or even a few 1000,- including components. I would really need something similair to JLCPCB especially with their big component librarySoldering wire to the trace may actually be acceptabele temporarily solution. I had not considered this yet.Quote from: Mechatrommer on September 29, 2020, 10:27:08 amWhy do you tink 10oz will not be enough? according to all my calculations 2oz will be enough. Are all calculators out there wrong?Although that copper bard is indeed badass i think this will be huge overkill for 40A. Additionally i think mechanical damage is much more likely to happen with a huge stiff copper part like this. Vibrations could tear the solder.

author: Nusa
author_rank: Super Contributor
timestamp: September 29, 2020, 11:34:40 am
content: There are all sorts of pcb busbars that could provide solutions for high-current traces. How well they might work in your case we don't have enough information to say.

author: Mechatrommer
author_rank: Super Contributor
timestamp: September 29, 2020, 12:50:07 pm
content: Quote from: superKris on September 29, 2020, 11:21:29 amwe are sorry then we cant provide you alternative... seeedstudio provides 2oz, but then you are using manufacturer's dependent tool you are stuck, we are sorry again life is hard.

author: superKris
author_rank: Regular Contributor
timestamp: September 29, 2020, 02:34:55 pm
content: Quote from: Nusa on September 29, 2020, 11:34:40 amThere is a lot of information in this post:https://www.eevblog.com/forum/projects/pcb-design-high-current-tracks-low-voltage-measurement-(please-review)/msg3223702/In my design i tried to keel the high current traces as short as possible. Basically its terminal -> 20mm trace -> double 2512 shunt - 20mm trace -> relay - > 20mm trace -> blade fuse -> 10mm trace. I have 2 of these in parallel.The traces are as wide as i could allow them to be. 10mm average on both sides of the PCB. Behind the relay the traces are even wider.This design makes busbars a little more difficult. Busbars would make more sense for a 100mm trace.Quote from: Mechatrommer on September 29, 2020, 12:50:07 pmI'm not sure what you mean with your reply. If i offended you in any way i'm sorry. I'm here to learn, and where possible help.I tried to do a lot of research concerning trace thickness and width. Here on the forums, calculation tools, and other sources. Most tell me that 2 traces of approx 10 tot 12mm wide in 2oz copper should be enough to carry 40A. In your post however you tell me that 10 oz (5 times more than calculated) is not enough. This may be true or not, but i would like to know the science behind it.I'm not familiar with seeedstudio. I will try their quotation tool tonight. It would be great if they can offer a affordable 2oz assembly!

author: Mechatrommer
author_rank: Super Contributor
timestamp: September 29, 2020, 04:03:42 pm
content: Quote from: superKris on September 29, 2020, 02:34:55 pmnot offended at all cheersi didnt look at your other thread before making the 10oz post but the most common high current pcb will use as other have said... exposed traces with no mask to put many solder, or with help with thick wires. but lets assume your 2oz design is fine (please also note the earlier poster mentioned you will not get straight 2oz), but now you come to us to ask help because your manufacturer cant provide you with design requirement, we cant, esp inexperienced me cant advice much on pcb assembly service since we think there are many parameters to make decision... part availability, price and costing shipping etc.... finding assembly service is as easy as typing it in google, but the details you will need to work and decide and contact them, given you have more time to research. but since we assumed you've researched jlcpcb, then the easiest and quickest solution we can see right now is slight editing in pcb editor to expose traces, solder later so you dont rely on that requirement, plus its cheap to ask for normal 1oz pcb, seeedstudio will charge $40+ more for 2oz spec. but then we dont know how many you are going to produce, self soldering 1000+ board can be a nightmare, we dont know if you have man power for that and how much profit can you get to repay etc etc, we advice base on small volume/hobby job.now i'm not expert in science of pcb and high current flow, what i know is we can reduce copper/conductor area and the current still flow, except hotter and higher resistance, you can continue cutting down area until it runs red glow, the current will still flow. so do you know how much temperature rise and trace resistance of your pcb during operation? putting more extra conductor area will make them comfortably cooler, and its usually dont take too much effort to add for slightly more, thats what i know. another thing is failure usually happened at bottleneck, where heat cant escape easily to surronding, maybe such as at the area where the pcb meet the pin/joint/soldering or in the connector used to connect to other devices. there are few members suggesting and shared experiences already about adding extra area and some other issues, so ymmv and good luck, cheers.ps: exposing some traces area should not hurt you can leave it as is during production, plus hasl plating can give you extra volume/area without adding a single cent. in case you figure out later you need extra area, you can easily solder on them without respinning money. without exposed traces, if heat goes beyond spec, something will be in trouble. as another way to say it... give more flexibility to your design to avoid sorry later.... there goes my long answer. ymmv and cheers.

author: Siwastaja
author_rank: Super Contributor
timestamp: September 29, 2020, 04:17:30 pm
content: JLCPCB's service is1) Brand new,2) The only of its kind.So don't get too fixated on getting exactly that kind of service.If it doesn't work for you because of any of the constraints, just suck it up and do what everybody used to do before JLCPCB, or still do because of the limitations they have. This means:1) Pay a bit more for assembly; go for cheap Chinese CMs. For example, PCBway works fine and will do 2oz for you. Assembly setup cost will be a few hundred $ though, more expensive than JLC in extremely small batches,2) If it is a one-off or mini-batch of a few PCBs, and you can't afford the cost of assembly, or the time it takes to communicate with the assembly house, just learn how to DIY it. I have made up to 700-component PCBs with tweezers and hot air gun; also miniatyre BGA image sensors, when the company I worked for faced problems with both money and (calendar) time. It's not fun, but doable.A completely different option is to be creative with increasing the current capability of traces. My favorite is exposing the tracks, adding paste mask openings, cutting some 0.1mm to 0.3mm copper sheet (easily cut with scissors) in shape, and reflowing it as a reinforcement. Can do with soldering iron, as well.

author: SilverSolder
author_rank: Super Contributor
timestamp: September 29, 2020, 04:26:07 pm
content: Can you use a 4 layer PCB, and get more space for larger traces that way? - so you could get away with 1oz

author: asmi
author_rank: Super Contributor
timestamp: September 29, 2020, 05:11:24 pm
content: Quote from: SilverSolder on September 29, 2020, 04:26:07 pmInternal layers in stackups manufactured by JLCPCB are only 17.5 um thick (0.5 Oz), so they won't have much current carrying capacity unless the board is going to be rather large. According toIPC calculator, for 17.5 um copper, 40 A current and 20° allowed temperature rise, you will need 166 mm wide traces. Compared to external 35 um (1 Oz) layer, where you need only 31 mm wide trace (it will have higher resistance and voltage drop, but since it's "outside", it can dissipate more power without heating too much.

author: SilverSolder
author_rank: Super Contributor
timestamp: September 29, 2020, 05:18:58 pm
content: Quote from: asmi on September 29, 2020, 05:11:24 pmI was thinking, move all the low current stuff inside the stack to the 0.5oz layers, leaving the 1oz layers free for large traces?

author: Alti
author_rank: Frequent Contributor
timestamp: September 29, 2020, 05:56:36 pm
content: You have a 40A relay, blade fuses and shunts there, dense stitching, with SSOP10 on top.Instead of using most of the space for copper pours, design SMD + mechanical layer on a PCB and then solder several thick jumpers on top of that, where needed. Add a new layer with jumpers. Could be soldered directly to relay/fuseholder terminals or you could put some SMD pads or THT holes for that (but that is an overkill).I do not know your expectations with regard to accuracy of current measurement, you use just raw resustors for shunts. It seems that if you substitute shunts with Cu jumpers, then the Cu jumpers can play as shunts. Alternatively, if you need 2ppm shunt, you can use isotan wire/tape (it solders quite well but not as nice as Cu).

author: mairo
author_rank: Unknown
timestamp: September 29, 2020, 10:52:35 pm
content: Quote from: superKris on September 29, 2020, 07:56:04 amI would think this is because of the oven settings - They probably reflow all boards with same thermal profile in theirs inline reflow oven, and a 2oz copper board most probably would need a tweak in the profile to achieve proper reflow with no manual reworks after that.

author: Kasper
author_rank: Frequent Contributor
timestamp: September 30, 2020, 03:29:31 am
content: Plus 1 for the seeed recommendation. I've had good results from them. They also have a big library and they have basic and advanced PCB services.

author: Siwastaja
author_rank: Super Contributor
timestamp: September 30, 2020, 08:01:54 am
content: Adding solder mask and paste mask openings (segmented! Say with a gap every 5-10mm) to the trace allows you to add solder "for free" during assembly. Remember that the solder isn't nearly as conductive as copper, but OTOH, it will be a lot thicker; say you get 100um of solder instead of 35oz of extra copper. I don't have exact numbers available but I think the result of segmented paste openings on a 1oz trace will be not quite, but fairly close to a 2oz trace.

author: superKris
author_rank: Regular Contributor
timestamp: September 30, 2020, 08:38:19 pm
content: Quote from: Mechatrommer on September 29, 2020, 04:03:42 pmThanks for the additional tips and comments. I agree with what your saying. I was just hoping there would be a similar service like JLCPCB that does check 2oz assembly, but it looks like there is nothing like this.I checked seeed, but thier online quote is 850,- instead of the 85,- at JLCPCB (1oz)Quote from: Siwastaja on September 29, 2020, 04:17:30 pmIt seems your right about JLCPSB being the only one offering this service at this price. Too badI check some other on line Chinese PCBA's but all of them charge around 400.- for assembly excluding components.For me personally doing my own SMD assembly is not a option. Its to many parts and i dont have enough experience or the right tools.I'm really loving the idea with cutting thin copper seeds and soldering them to the board. It sounds like a effective way of adding a lot of copper!Quote from: SilverSolder on September 29, 2020, 05:18:58 pmThats actually a pretty smart option i did not yet consider! I'm not sure how big the advantage would be tough. The traces could be wider, but they still have to go trough a single pin so i think there is a limit i will hit when going with a wider instead of thicker trace.Quote from: mairo on September 29, 2020, 10:52:35 pmI did not think of this. You may be right here, however i'm sure there are more people that would like cheap 2oz assembled boards. Its not like its that hard to create a new profile.

author: superKris
author_rank: Regular Contributor
timestamp: September 30, 2020, 08:45:36 pm
content: Thank you all for your kind advice.I was hoping to find something similar to JLCPCB assembly but with 2oz copper. All the services suggested here charge approx 450,- or more for assembly alone. Adding a premium price for components, PCB, and other charges, i doubt there is any other company offering the same solution below € 800,-I guess i will have to go with JLCPCB and 1oz copper. I will expose the tracks for HASL and maybe add some tin later. If the traces get to hot, i'll add copper wire or maybe thin copper sheets cut in shape. Its not ideal, but until i can do bigger batches to reduce the cost, this is the best solution i think.Again, thank you all!

author: langwadt
author_rank: Super Contributor
timestamp: September 30, 2020, 09:04:15 pm
content: Quote from: asmi on September 29, 2020, 05:11:24 pmafaik those ipc calculators are obsolete based on ancient data, especially for internal traces with planes. The dielectric has 10 times better thermal conductivity than air so an internal trace next to a plane heat-sinking

author: tszaboo
author_rank: Super Contributor
timestamp: October 01, 2020, 07:25:35 am
content: First, change to 4 layer. You have a 2 layer design, the remaining 2 extra layer can be almost 100% copper. And while asmi calculated that you would need 166mm traces on the inner layers, that is not the point. If you have 4 layers, some of the current will go on each layer, and adding extra copper cannot hurt. Also, most calculators are running with 10 or 20 Celsius temperature rise. And there is nothing preventing you having more temperature rise. A PCB doesnt magically stop working at high temperatures.Also, enlarge those tracks for the bottom layer. Use all the space. It helps spreading the heat.40A is not even that much current...

author: Mechatrommer
author_rank: Super Contributor
timestamp: October 01, 2020, 07:45:59 am
content: 4 layer is extra money..

author: tszaboo
author_rank: Super Contributor
timestamp: October 01, 2020, 07:58:00 am
content: Quote from: Mechatrommer on October 01, 2020, 07:45:59 amIt is automatic. No extra parts. And PCBs are cheap. Cheaper than a failing product or a redesign.Quickyly checking, JLCPCB charges 4 USD for 2 layer design and 7 for 4 layer at 5 pieces. That's 60 cent per PCB. Surely, you can afford it.

author: superKris
author_rank: Regular Contributor
timestamp: October 01, 2020, 10:35:45 am
content: Quote from: NANDBlog on October 01, 2020, 07:25:35 amI think you guys are right about switching to 4 layers. I'm a little inexperienced with 4 layer design, but i'm sure it wont be to difficult. I'll try to do a partial redesign.Below is a more updated screenshot of the current layout.

author: superKris
author_rank: Regular Contributor
timestamp: October 01, 2020, 05:34:36 pm
content: So i did a comparison for 2 and 4 layer including assembly and for 5 PCB's i pay €25,- extra so, that 5,- per board.I would rather not pay 5,- per PCB extra but it gives me additional copper in total thinkness and i can use wider traces on top and buttom because i have to route less on this layer. I think that is totally worth it.I just wish i had done this earlier when i was struggling to get all nets on 2 layers...

author: tszaboo
author_rank: Super Contributor
timestamp: October 01, 2020, 07:09:05 pm
content: Quote from: superKris on October 01, 2020, 05:34:36 pmSo, if you order bare PCBs, it is extra 3 USD, but if you order assembly it is extra 25? Makes sense. I really dislike these arbitrary pricing.

author: Mechatrommer
author_rank: Super Contributor
timestamp: October 01, 2020, 07:21:37 pm
content: seeedstudio will ask extra $50 or more for bare pcb 2L vs 4L 10pcs, but they let you do multiple design in a 10x10cm hobby board, unlike JLCPCB. JLCPCB will take their fun time to check meticulously your pcb, you cant have break in ground plan they will consider it different design (even if its in the same design) and quote you for many extra non-hobby $5 price. so i guess we cant predict from numbers, its a matter of principle. one's strength is the other's weakness, you have to find that out yourself.

author: asmi
author_rank: Super Contributor
timestamp: October 01, 2020, 07:35:48 pm
content: Quote from: NANDBlog on October 01, 2020, 07:09:05 pmThat makes no sense. Why would assembly cost be any different for 4 layer boards than it is for 2 layer ones?

author: asmi
author_rank: Super Contributor
timestamp: October 01, 2020, 07:42:16 pm
content: Quote from: superKris on October 01, 2020, 05:34:36 pmUse multiple layers for the same net if possible - just remember to stitch the crap out of them to provide low-impedance path for the current. And don't forget about return current too - it's not that uncommon for designers to beef up the power rail, but pretty much ignore the ground return rail.

author: tszaboo
author_rank: Super Contributor
timestamp: October 01, 2020, 07:51:39 pm
content: Quote from: asmi on October 01, 2020, 07:35:48 pm

author: Siwastaja
author_rank: Super Contributor
timestamp: October 02, 2020, 04:55:56 am
content: Quote from: superKris on September 30, 2020, 08:38:19 pmSorry I'm going on about this but I don't understand how you can do this job that way. At least I need to test things out, prototype, measure, swap parts, correct for mistakes, etc., etc., I can't just draw a finalized perfectly working design in EDA and order it. And if you can prototype and swap any part, you can definitely build a complete board as well.There's only one way to get the experience you are lacking.Tools are not expensive, either. I'm using a 3D printer heatbed for board preheat + a Chinese $30 hot air gun to do reflow. Expired credit cards to apply the paste with stencils. You need less than a square meter of table surface for your lab. Besides, you can just hand-solder with iron unless you have BGA/LGA-style packages. This is obviously for building the one or two prototypes. If you have to do a few dozen, it will start sucking life out of you, but then again, a few hundred $ of setup fee isn't that huge anymore?

author: Siwastaja
author_rank: Super Contributor
timestamp: October 02, 2020, 05:09:14 am
content: Quote from: superKris on October 01, 2020, 10:35:45 amDo note that if you already have a 2-layer design, designing in 4 layers is wayeasier. You will have two ground planes; do the routing on top/bottom like you have so far, but instead of having to think how to stitch together a good ground plane, you just leave the mid layers completely solid, and see, you get to the good, low-impedance ground plane through a simple via, anywhere, anytime! Fewer things to go wrong.Additional benefit is, these ground planes areveryclose to the top/bottom layers, say typically around 200µm (see your PCB manufacturer stackup). This means, the thermal conductivity from top/bottom to the ground plane is good simply because the FR4 prepreg inbetween is so thin. Even if the nets are different - one carrying current on top, and the ground plane directly below - the ground plane takes the heat from the top layer trace and spreads it over a larger area on the PCB. The heat is now again coupled to the other nearby top layer tracks, even when they are not electrically the same, and a larger area of the PCB works as a heatsink. This doesn't lower the power dissipation much, but allows higher dissipation given a certain maximum temperature rise.Finally, one thing worth considering, not mentioned so far, is: try miniatyrization. Can you make the PCB smaller, and thus, traces shorter? Ask yourself, why do I carry currents around this board? You have components A and B, say a connector and a MOSFET, for example, and say, 50 mm of trace between them. Can't you move A and B right next to each other?Also note, trace width calculators assume an infinite-length trace. If you have a short trace, heat is transferring from the ends as well; and, the heat is transferring to the components soldered to the trace. Say, a 20mm long, 10mm wide trace can carry much more current than a 100mm long, 10mm wide track.

author: Mechatrommer
author_rank: Super Contributor
timestamp: October 02, 2020, 06:01:35 am
content: Quote from: Siwastaja on October 02, 2020, 04:55:56 ammy thinking too... all projects that i've done so far will need corrections, the simplest is just a matter of adding few extra resistors and bypasses etc, some are simply broken/wrong design that needed major redesign. some projects i've done for years just to keep optimizing and respinning the pcb and sent to seeedstudio multiple times... thats why my primary goal from beginning is find the cheapest option for pcb production. if i understand it correctly, OP wants to produce just 5 board, if its just 5 boards i will just assembly myself... assemble 1 board first and test. if we get 5 fully populated board and we figure out it needs corrections, then its a nightmare (either paid or respin assembled pcb cost or rework needed to desolder if its decided to diy etc) but well, maybe the OP has specialty that some of us dont have, so cant argue too much..Quote from: Siwastaja on October 02, 2020, 05:09:14 amand my thinking too... i never go to 4 layer (mainly due to cost) but i can imagine we can retain existing layout of external layers and just add parallel traces on inner layer connected "via" viasbelow is example of a dev board of an opamp, we can see inner layer is nothing, just few solid power planes, we can layout traces on external layer like we do on normal 2 layers pcb, ymmv.

author: tszaboo
author_rank: Super Contributor
timestamp: October 02, 2020, 08:28:05 am
content: Quote from: Siwastaja on October 02, 2020, 04:55:56 amHmm, no thanks?I mean I work as an engineer. I order assembled boards, first prototype about 10 pieces. Some of this will be used up by testing, some of this I give to the mechanical designer, the FW writer, the sales guy. If something is not working or needs change, maybe I solder it on 1 board, to see if it is working, than I write work instructions for the other guy, to do the actual soldering. If there are a lot of changes, it goes to prototype 2. I mean, there is about 86 other things to do on a project besides putting a board together, and this is something that can be done by robots and people who are dedicated to do this.

author: superKris
author_rank: Regular Contributor
timestamp: October 02, 2020, 09:25:19 am
content: Quote from: NANDBlog on October 01, 2020, 07:09:05 pmIt includes via's, assembly, etc. Its calculated on my current version of the PCB. When i do a online quote for just the board size (120x110) and the 2 or 4 layers its 8,- vs 38,- so the difference is even bigger. Anyway, its dirt cheap as far as i care so i'm ok with the extra charge.Quote from: asmi on October 01, 2020, 07:42:16 pmDo you mean adding additional vias throughout the length of the trace? I did not do this because i think it would mainly remove copper from the layers itself. All high current parts are through hole and therefore multi layer so the connection is already there. The only exception are the SMD shunts, and as you can see in the pictures here, i added a lot of vias.All return current is off board, so no problems there.Quote from: Siwastaja on October 02, 2020, 04:55:56 amIts not my first version of this project. It is however very different form my first prototypes but i already know some things work and some have already been corrected.I dont want to do a full hand assembly because its approx 250 components and density is pretty high at some pints. Most of these parts are simple resistors and caps anyway. I see no reason to do it by hand if can be done better for just a few $. I will have to do some hand assembly though. Mainly some IC's that are not in the JLCPCB database or are to expensive. There also still is a lot of trough hole components. I do have a hot air solder station and know how to use it, but i dont have the best hand-eye coordination and steadiest hands in the world.Another reason is component price and MOQ. Especialy the basic libary of JLCPCB is very cheap and i doubt that i can get the loose components at the quantity that i require for the same money. So basically the assembly is cheaper faster, less work, and less chance for assembly errors.

author: Siwastaja
author_rank: Super Contributor
timestamp: October 02, 2020, 09:44:29 am
content: Quote from: NANDBlog on October 02, 2020, 08:28:05 amDo you read the context at all? The problem for the OP was he can't afford to pay $400 for the assembly setup. Even more expensive would be hiring another person to do the job. It's clearly not about a professional setting with a proper budget. For money-constrained operation (startup world or hobby), DIY by the designer is often the only way.

author: superKris
author_rank: Regular Contributor
timestamp: October 02, 2020, 10:24:16 am
content: Quote from: Siwastaja on October 02, 2020, 05:09:14 amThank you for all of that input. I have never done a 4 layer design before but it was simple enough so far. Yesterday i moved most most signal traces from the bottom layer to the new 2nd and 4rd layer. My reason to do this was that i wanted as much as GND on the bottom layer as possible. This layer is thicker than the middle layers and therefore more conductive. Currents through the ground layer will be low. Theoretically the max will be below 2A, and real life application will probably be below 1A for the full GND current. All the other GND will be off board. On the board its mainly the relays that need some current, and the expansion ports. A benefit of moving the bottom layer traces to the 3rd and 4th layer is that i have to do a few less layer jumps using vias.The reason i want a solid ground is that this is for a automotive application. Most of the used components are protection against aggressive surges like load dumps. TVS diodes will have to sink these current to the ground. In a worst case scenario it will be approx 10 points of 1 to 2A. Maybe i'm over engineering this...In my design i can specify a couple off different nets:- High current. I will place these on every layer as wide as i can, and keep length as short as possible.- GND. I will fill every layer to prevent as much noise as possible and keep thermal conductivity optimal.- Digital traces. I2C only. Not sure about the bandwidth, but nothing special i think. Currently running on multiple layers- Signal traces. Simple analog DC stuf not sensitive for noise. dont care about the layer.- Analog. 0-4V analog signals between current sense amplifiers and ADC's. Currently on middle layer- Sensitive analog. The shunt traces need to have as little noise/induction as possible. I need to measure in the uV range. These traces are short and currently top layer only.From your advise i take i should maybe keep the all signal traces on the top and bottom layers, and fill the 2nd and 3rd layer with GND. Do i understand this right?Is it better to jump a trace a few extra times between layers where needed, or should i use the middle layers if this means i only need to do 1 or 2 jumps?Considering the component layout; This was all done in a way to keep the high current tracks as short as possible. All the other components are put arround these and i think there is no way to improve this any further. I tried a lot of things here.

author: Siwastaja
author_rank: Super Contributor
timestamp: October 02, 2020, 10:46:09 am
content: You can route the signals on top and bottom, using the mid layers as ground planes, like I adviced, or do the opposite: use the mid layers for routing and top&bottom as ground planes like somebody else adviced. Both work; distance between mid1, mid2 is long enough so the signals don't couple too much, unless you have very high edge rates and/or very sensitive signals.Or, I often end up with this stackup that combines both ideas:Top: components and all routing that fits hereMid1: Full ground planeMid2: Routing that didn't fit TopBottom: Full ground planeIf you do this, Mid2 is shielded better than top, being between two ground planes.The reason to route in Top is because your SMD components are already there; you save space by not going through vias to another layer. But then again, if routing on Top is taking space that could otherwise be used for components, then by all means go to another layer. Tight component placement is a good driving force. (Except it does make hand assembly, test&measurement a bit more difficult, I have to admit, but I'm happy to pay that price for a tight design that doesn't require redesign to improve efficiency, EMI, or miniatyrization when you have to fit it somewhere, or add new features to it.)I prefer single-sided component load whenever possible, to save assembly cost and steps. This also leaves you the option to freely second-guess whether you want to use Mid2 or Bottom for ground plane. If I have a design which dissipates heat, I may end up bringing heat from top, through vias, to a polygon fill at the bottom, which then couples to an aluminium heatsink through a silpad. When you do this, you can't have full ground on the bottom (unless all heat-generating components have their thermal pads connected to ground, regulator ICs often are this way!), for example, FETs heatsink through drain, which would show a switching waveform.So you have many options which are all good, the key is to remember that all signals that have any significant edge rate (even I2C; definitely SPI and similar. Even a relay control signal from GPIO may have quite an edge rate, unless you series-terminate it with a resistor at the driving source) must have an uninterrupted reference plane close. So you need signal - ground pairs: Top&Mid1 and Bot&Mid2. Within the pair, you can swap which one is the reference and which one is the signal. But distance between Mid1 and Mid2 is long, they can't be a pair. Conversely, if you have crossing tracks at Top & Mid1 (or at Bot & Mid2), they are going to couple because the layers are so close to each other. Hence either needs to be a low impedance reference plane; most simply just ground, but can be a power plane bypassed to ground with capacitors peppered all over. Such power planes make sense when you have multiple chips, possibly with many Vcc pins, sharing same voltage buses.

author: superKris
author_rank: Regular Contributor
timestamp: October 02, 2020, 01:55:24 pm
content: Quote from: Siwastaja on October 02, 2020, 10:46:09 amAgain thank you for all that advice! I like the combined solution that you suggest. Right now most traces that didnt fit the top is sitting om mid1. Mid 2 is mostly ground with a few traces. Thats easy to switch around.I do have a couple running parallel above each other between top and mid 1. I'll try to prevent this. Again great advice. Thank you!

author: SilverSolder
author_rank: Super Contributor
timestamp: October 02, 2020, 08:43:56 pm
content: Where there's a will, there's a way! - Godspeed.

author: julian1
author_rank: Frequent Contributor
timestamp: October 02, 2020, 10:11:46 pm
content: QuoteFor a four-layer, with two inner grounds - do you still use (some) stitching between the inner grounds? Or just join them at the board connector for gnd? I am interested in mixed-signal designs.I was focused on having gnd and power inner layers. Then I tried routing power with signals on the outer layers, and found surprisingly that routing complexity was mostly the same. So I am thinking two inner gnds might be better.

author: IconicPCB
author_rank: Super Contributor
timestamp: October 02, 2020, 11:37:07 pm
content: Do not forego the mechanical considerations of a four layer "book layup".The weave and weft of the core materials and copper coverage of plane layers must be considered in order to ensure a flat bare board.If the finished bare board is not flat then there will be issues of pin coplanarity ( read air gap ) between solder stencil and component pins.

author: Siwastaja
author_rank: Super Contributor
timestamp: October 03, 2020, 07:16:25 am
content: Quote from: julian1 on October 02, 2020, 10:11:46 pmIf you connect the components (like the ground pins of the ICs) to the planes with a via, the return current follows this best route. With a solid plane, it doesn't need to hop through vias multiple times. Hence, unlike in two-layer design where you need to stitch the ground plane together from broken pieces, stitching the 4-layer design ground planes isn't that critical; just have the connecting vias wherever the ground currents originate. Sure, whenever you have space, feel free to add extra stitching vias.And, when you route on top/bottom layers and decide to add ground pours there (not actually necessary when you have the ground plane just below!), then you have to go through the extra task of adding vias to avoid isolated copper islands. Using top/bottom pours can be a good idea for mechanical (copper balancing preventing board warping) or thermal (copper spreads heat laterally) reasons.

author: SilverSolder
author_rank: Super Contributor
timestamp: October 03, 2020, 01:12:48 pm
content: Quote from: IconicPCB on October 02, 2020, 11:37:07 pmWhat causes that - different thermal coefficients of expansion for copper vs. fiberglass causing internal forces?

author: julian1
author_rank: Frequent Contributor
timestamp: October 03, 2020, 09:13:16 pm
content: Thanks for the good suggestions. I suspect board warping / pin coplanarityissues, can be helped/mitigated by sticking with the thicker (>=1.6mm) FR4board options.I particularly like the idea of always having a gnd plane immediately under signalsregardless if they are top or bottom layer. Having a 3rd layer power plane,so that bottom layer signals have the extra distance of an FR4 laminate, instead ofjust pre-preg to get to ground seems like an odd compromise.The whole thing with sinking extra vias to join-up isolated islands also feelslike a bad workflow.