Seeedstudio 4-layer PCB quality
Note: this blog post is aimed at PCB designers, it may contain some jargon and references that you wouldn't get if you don't at least occarionally design circuit boards.
The democratization of PCB prototypingFirst off, a little bit of PCB design history for the people that are relatively new to the scene. In the olden days, PCB design was a cost and labor intensive process. There were very few properly free design tools around, and believe it or not, until the early 2000s there was a lot of custom and proprietary file formats for PCB designs. Also, you as a PCB designer had to account for all kinds of things that were really none of your business - you had to make sure copper density was fairly equal over the area of your board, you had to specifically draw panels, routing or v-grooves according to the manufacturers specifications (even if they purported to be compatible with Euro card standards or other standard registrations) and you usually had to pay a pretty penny extra for nonstandard solder mask colors, double sided silkscreen, having SMT pads, number of vias, etc. And maybe the most important difference with now: it was hella expensive to get anything made. You could not prototype under a couple hundred dollars - setup fees were astronomical.
This is very different nowadays. The Gerber RS-274X file format has been standardized and is actually also interpreted equally between manufacturers, design rules have tightened up considerably (everybody supports 6/6mil design rules, SMT, high density vias, various pcb thicknesses, etc.). You don't need any human interaction and your board just gets made exactly the way you want it. And you can get all of this for $10 per 10 boards, a dollar per board!
Old tech is still aroundWell, you can get all this goodness at places like Iteadstudio, Seeedstudio, Elecrow and TinySine. Most other manufacturers that offer some kind of prototyping service have some catching up to do. I live in the Netherlands, and around here there are a couple of big name PCB manufacturers: Cyner, Ramaer, Vermeulen printservice, van Zon and Eurocircuits. Most of these are really traditional PCB manufacturers and don't offer any kind of prototyping - apart from for instance a sponsorship deal that Cyner had with a student project I participated in. Two exceptions to this rule - Vermeulen and Eurocircuits - do offer prototyping and... still have ancient design rules and methods.
For instance, Eurocircuits charges extra for SMT, double sided silkscreen and has comparatively poor design rules for their prototyping services. Also, they manage to have equal or sometimes even longer shipping times than PCBs I order from China, partly because their QA and finishing services are not in the same place as the PCB manufacturing plant. Like many more old-fashioned companies they also have the dreaded proprietary panelization/registration formats (called eC-registration in their lingo) which attempt to lock you in to one manufacturer for batch work. Lastly, they are still one of those manufacturers that have a ton of bugs importing Gerber files. All this for significantly higher prices than Chinese manufacturers.
Of course, until recently this was kind of a moot point because these more traditional fabs had two big advantages: the ability to make PCBs using the most advanced technology, and the integration of tools to help medium to large companies let their employees directly order PCBs on company budget, and under direct (digital) supervision of their bosses. This was a big time and money saver as you did not need to route this kind of stuff through a purchasing department.
Times are changing, though. Whereas the 'cheap Chinese' manufacturing used to just have 1.6mm green, small PCB facilities, they quickly grew to now encompass basically all technologies you frequently need. 4-layer, all colors, all PCB thicknesses (down to 0.2mm, up to 3.2mm), even flexible and RF substrates. And it seems like 6-layer PCBs are just around the corner, making it possible to do extremely dense BGA breakouts. And the quality has since far outgrown hobby levels. 6/6mil is now standard, going down to 2/2mil design rules with laser cut vias (!!) on flex PCB. There is very little reason anymore not to order from China, so: everybody does. They even offer fairly competent PCB assembly and small to medium run PCB fabbing services - with lightning quick turnaround (15 days + shipping).
And account control as well as budget control is also improving by leaps and bounds. The Chinese services still require pre-payment, but other than that the ordering process is completely automated and supervisable. Contrary to my experiences with European services, I have never needed to fix any mistake that was not mine or a crappy gerber importer error. In general, I have saved tremendous amounts of time talking on the phone or e-mailing back and forth with PCB fabs because the Chinese manufacturers offer such a good hands-off experience. Of course, this would be a horrible thing if they would often make mistakes, but they don't. They just make everything the way I designed it.
Seeedstudio 4-layer qualitySo let's go to the actual topic at hand, let's look at some PCBs. The internet is full of 2-layer PCB examples from Iteadstudio and Seeedstudio and apart from coarse silk screen it is usually pretty decent if you respect their 6/6 mil rules. However, I recently had the need to route PCI-X and PCI express riser boards for my work and those are a total pain, if possible at all, to do on 2 layers. So for the first time in 2 years I started a 4-layer design and ordered it at Seeedstudio. Here's the result:
So a full run-down of the specifics:
|Board material||FR-4 1.55mm|
35µm outer layer copper thickness
18µm inner layer copper thickness
|Surface finish||ENIG (Electroless Nickel Immersion Gold) ~2µm|
|Solder mask color||Red|
|Amount ordered/received in good order||5/5|
|Price||$105.90 + $29.24 shipping (DHL)|
|Total time||11 days|
That may seem like a steep price, but if I were to order the same board with a longer (!) lead time from Eurocircuits, it would cost me €1064, or about $1450 - mainly because I was ordering over the end-year holidays.
Alright, first off there seems to be some confusion on the site over the copper thickness and I highly suspect this just to be some kind of translation error. They say that the inner copper is 18µm and outer is 35µm thickness, but the design rules are the inverse of what you'd expect: 8/8 mil for inner layers, 6/6 for outer. Thicker copper usually means looser design rules. Also, it's very unusual to have the thick copper on the outside, as the inner copper layers are meant for ground and power plane routing as well as heatsinking, favouring thicker copper. Also, the 4-layer process is being done on a card edge compatible process (see later why I think this is the case), which always has 18µm outer layers to accomodate easy insertion into card edge connectors. But enough talk about crazy Chinese people jumbling their specifications, let's look at the actual PCB. First off: did they get the build-up right?
Yep, spot-on. As is usual with multilayer boards, I dedicated a small area on an unused side of the board to numbers placed on consecutive copper layers with the solder mask removed. The reason you can see the '1' and '2' so clearly, but not the '3' and '4' (squint a little and they should be apparent) is that the first two layers are only separated by a very thin sheet of prepreg material, but layers 2 and 3 are separated by the bulk of the FR-4 material. FR-4 has glass fiber reinforcement in it, and that stuff disperses the light all over the place, making it hard to look through. If you intend on making a multilayer board, especially more than 4 layers: always put these marks on the edge of the board. As you can see here, I'm actually lighting this slightly from the side, because you can't see anything but the '1' and '2' if you illuminate the numbers from behind.
Alright, next up: layer alignment.
Let me first point out the little breakout tab that hasn't been properly finished on this board. It sticks out only about 0.2mm, so it's alright and this was the worst board (other boards also had a little bit of breakout tab left, but even less than this). Anyway, as far as the photographic layers (copper, solder mask, plating and drilling): they are absolutely perfect. Those traces you can see are 6 mil, so the misalignment between solder mask and copper is definitely less than 2 mil. Other boards were just as good, with the worst-case misalignment still not visible to the naked eye.
Silkscreen, unfortunately, is lacking even on this premium service. I know from past experience that you really have to specify 0.15mm minimum silkscreen line width to get readable text on the 2-layer designs. However, I would have hoped for better quality silkscreen on their 4-layer service. It is also, especially considering this process has significantly better quality than the 2-layer stuff, quite far out of alignment, up to about what seems like 12 or 15 mil. The misalignment is only in one direction. However, they still printed the little lines (more like dots now) between the pads for those 0402 resistors, which is alright. Because I've specified via tenting in my gerbers they also printed silkscreen on top of tented vias, which is a first for me. Other services usually cut out vias from being silkscreen-printable. Speaking of via tenting...
As an aside, look at that great routing alignment on the left of the leftmost finger pad. They definitely routed these boards in-panel and not separately. Very happy about this, because PCI and PCI express need a decent slot/outline alignment to the fingers.
Anyway, they have also done an excellent job tenting these 12 mil via holes. Not a single one has collapsed on the entire board, counting more than 200 vias. And yes, they also do via in pad very well. Very impressed. Because these are the absolute smallest holes they will do, and they are already a bit dimpled, I do not expect them to be able to tent larger (20+ mil) via holes. I know from the 2-layer board service that such large holes will not properly get tented, so if you want to have tented vias (e.g. for heatsinking a big QFN): use the smallest supported hole size. Talking about holes (I am great at segoues):
Those are some very sexy holes. Also note the little oopsie on the silkscreen on that middle hole: it almost seems like they first did the silkscreen, and did plating afterwards. Anyway, the plating is very good, the hole finish is alright (a bit of drilling and layer connection roughness is visible, but nothing too bad). The plating really juts out on these holes, it seems like they did properly thick plating and not that sub-micron stuff on very cheap Chinese electronics. This photograph is also a nice example of the excellent solder mask and hole alignment.
But when I got these boards back I noticed a very pleasant surprise. Look at this:
That is a board edge chamfer on the fingers. Okay, you say, what's so special about this? Well, I didn't tell them to do this. I assumed that their manufacturing plant would be a bit too bare-bones to do chamfering. But they recognized this as a card edge connector (probably because I plastered 'PCI-X' all over it) and did the chamfer for me. Very nice, and thoroughly appreciated.
So, the boards are perfect and I am totally happy? No, there is one little niggle with these services that I have tried to resolve with this batch of boards and failed. These board fabs tend to put all kinds of manufacturing codes on the board, usually in places where you don't want it. It mostly doesn't matter, but I intend to order things like front panel PCBs and other boards with aesthetic purposes in the future and I really don't want them to ruin it with their scribblings. So I put this on the board and specifically instructed them to put any markings in that area:
As you can see from the emptiness of this box, they didn't put it here. Instead, they put it all the way on the edge on the other side of the PCB:
Apparently, I could have known this. On the forums people say that seeedstudio always puts these codes on the rear side (bottom copper) layer, and iteadstudio puts them on the top layer. I and *many* people with me would very much like the option to say where they should put it! This is one of those instances where it would have been nice to be able to call someone at the manufacturing plant.
ConclusionSeeedstudio.com has fared very well today, delivering excellent quality at not the lowest of prices, but still a very acceptable price (and certainly much less than it would cost locally). The ordering process and delivery are so good that I didn't even mention them, that's how good they are. The PCB itself was pretty much perfect except for them messing up the manufacturing code, a little bit of breakout tab not being finished properly and not-great silkscreen quality.
Something I have been using a lot and found very useful is this little renaming script. If you want to order from seeedstudio.com and are using FreePCB or another EDA program with compatible gerber file names, you can use this DOS batch script to rename and zip (using 7-zip) your files in accordance with their Fusion PCB service:
1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28
::-----CODE----- ::Eradicate rogue temporary files if exist filelist.txt del filelist.txt -y if exist seeed del seeed /q dir /b >>filelist.txt ::Make target folder and get project name if not exist seeed md seeed for %%* in (..) do set pname=%%~n* @echo %pname% ::rename all the files copy board_outline.grb seeed\%pname%.GML copy bottom_copper.grb seeed\%pname%.GBL copy bottom_silk.grb seeed\%pname%.GBO copy bottom_solder_mask.grb seeed\%pname%.GBS copy drill_file.drl seeed\%pname%.TXT copy top_copper.grb seeed\%pname%.GTL copy top_silk.grb seeed\%pname%.GTO copy top_solder_mask.grb seeed\%pname%.GTS if exist inner_copper_1.grb copy inner_copper_1.grb seeed\%pname%.GL2 if exist inner_copper_2.grb copy inner_copper_2.grb seeed\%pname%.GL3 :: zip it "%ProgramFiles%\7-zip\7z.exe" a -tzip seeed\%pname%.zip .\seeed\* :: remove temporary file del filelist.txt ::------CODE------
I hope this will help some people speed up their workflow and avoid filename and extension mistakes that happen so easily when manually copying and renaming files.
This has been part one of this small series. Next time we will be looking at Iteadstudio.com's flex PCB quality and smtstencil.co.uk's paste stencil service.
Onderdelen erop solderen en gebruiken voor het doel waarvoor je hem ontworpen hebtXessive schreef op vrijdag 03 januari 2014 @ 21:23:
maaruh... wat doe je er precies mee dan..??
In dit geval is het een riserbord met meetweerstanden, zodat ik het verbruik van PCI(-X)-insteekkaarten kan meten.
I have used their service at work, also using the service of them generating gerber files from Eagle files. After this experience I will never do that again.
After they sent a design review PDF document, I noticed some oddities on the silkscreen. I asked if it still on time to be corrected (with renewed design files). It was not possible. Already started production, goodbye. They recommended I should start swish ('grasduinen') through the Eagle manual. In other words, screw you.
You pay ~270 euros for 4x half-eurocard 4-layer PCB's, and they are finished after 3 workdays instead of 5 workdays. Are they sending it early? No way! 3 day service is a premium service and costs extra, screw you. You have to wait another 2 workdays.
My experience with Itead and Seeed is they turn boards around in 3 days, and send orders if everything is in stock. With DHL & Itead I experienced; ordered on Monday, done on Thursday, sent on Friday, order was on Monday.
What Eurocircuits does have in favor over China, atleast the "mainstream" sites like Itead etc., is they have more options. However they charge a ton of money for that, so in the end you avoid it at (all) cost. China produces normal 2 or 4 layer PCB's very cheaply, making them really attractive.
About your other comments:
Final copper thickness can be defined as thickness of copper film + plating thickness. If the copper is 18um and 18um plating, results in ~35um copper thickness. This plating is done for via's etc. ofcourse.
Inner layers don't get plating over the copper foil, so they usually start with 18 of 35um and dont grow.
I also experienced silkscreen offsets on Itead & Seeed, worst at the bottom.
I've done via tenting before on Itead&Seeed, and works beautifully. They also didn't complain about 1000 holes on a 10x10cm board, via's through pads, via's close together (the holes basically touching) by accident, etc.
Watch out via in pads though: during reflow soldering it could happen the via sucks in solder, which means there may be not sufficient solder to complete the connection (especially if you via spam cooling pads or stitch planes together).
In my experience the production codes were either put on the back and once conveniently under a DC power barrel jack connector. So if populated you wouldn't see it !
I can life with all those 'minor' things. The only thing that did annoy me was, on that design 1000 holes on a 10x10cm board, I think they ran out of reserves for my design (I also pushed their design rules a bit with like 2 QFP chips of 144 * 48 pins, 0402's, and generally quite high density routed for 2 layers), so 1 board had a "manual fix" on it. They cute a piece of the board between a 0402 passive where the clearance between both pads was a bit tighter (a thick trace ran through one side of the pad), so they obviosuly had a short on the last board.
For me that means 1 board less, unless I really have to use it..
[Reactie gewijzigd op vrijdag 3 januari 2014 23:22]
Ik dacht dat dat best wel obsolete was tegenwoordig (sorry )
Het is voor een serverbord, waar nog een 3.3V PCI-X slot in zit. Waarschijnlijk zullen er alleen 32-bit PCI kaarten in gestoken worden (if anything), maar voor het geval dat heb ik alle 64 bitjes doorverbonden. Kostte toch niks meer - zowel in design time als printplaatkosten.timberleek schreef op vrijdag 03 januari 2014 @ 22:16:
Wordt er nog zoveel met pci-x gedaan dan?
Ik dacht dat dat best wel obsolete was tegenwoordig (sorry )
Aha, volledig out-of-my-league.. da's aan mij niet besteed zo iets. Heb 2 elektrotechnisch ingenieurs in de familie en daar ben ik er dus geen van hahaha. Als jij het maar snapt maar dat komt wel goed heb ik afgelopen jaar/jaren al wel gelezen hier!mux schreef op vrijdag 03 januari 2014 @ 21:27:
Onderdelen erop solderen en gebruiken voor het doel waarvoor je hem ontworpen hebt
In dit geval is het een riserbord met meetweerstanden, zodat ik het verbruik van PCI(-X)-insteekkaarten kan meten.
This was written a few years ago, have you encountered any improvements ordering prototype PCBs online?
Looks like Macrofab is trying to get into this space but I ended up talking to engineers at the end of the day. Not too automated...
PCB:NG (http://pcb.ng) looks interesting. They were on AmpHour a few months ago http://www.theamphour.com...athan-hirschman-of-pcbng/. Pure software solution and I didn't have to speak to anybody