Iteadstudio's flex PCB quality

Door mux op vrijdag 17 januari 2014 21:43 - Reacties (6)
Categorie: -, Views: 58.149

This is part two of a - probably - longer running series on PCB quality in the 'hobby' space. I say hobby space mainly because of prices, not necessarily quality. If you haven't done so already, I highly recommend reading my previous blog post about seeedstudio's 4 layer PCB quality for some background on the subject.

Overview of the PCB

For my work work I needed a flexible PCB that could fit inside more or less arbitrary electronics to function as a sensor. I didn't have any control over its position or shape, so the PCB had to be as flexible as possible to accomodate any usage scenario. Flexible PCBs (also called Flat Flex PCBs) of course immediately sprang to mind, but until very recently this technology was incredibly expensive - last time I ordered one from Cyner the invoice was well above 2000 euros for a small prototype. For some time however, offered an up to 100x100mm flexible PCB manufacturing. That's past tense, because it seems right now that I'm writing this blog, they are discontinuing the service. However, after informing about this service, I heard from the PCB service behind Itead studio that they will be re-launching the product after the spring festival. The service is back, you can find it here. Prices are pretty great; $65 for 5x5cm up to $80 for 10x10cm.

Anyway, here's a rundown of my board

Board materialMylar 0.15mm
18µm copper thickness
Surface finishENIG (Electroless Nickel Immersion Gold) ~2µm
Board size34x50mm
Solder mask colorYellow
Amount ordered/received in good order10/10
Price$75 + $33 shipping (DHL)
Total time20 days

I have to say - this is an absolutely stunning PCB technology. The boards are incredibly thin. The substrate is actually a bit thinner than 150µm and very transparent. But not just the looks are good, the design rules are incredible. With 2/2 mil copper width/spacing (yes, you read that right) and lasercut vias, you can use this technology not just for flexible stuff, but also to break out extremely dense BGA packages for just $6.50 per PCB. And because almost everything in the process is lasercut, alignment and tolerances are absolutely stellar. Have a look at this:

This is almost a microscopic view of the PCB, looking at an 1812 Kelvin sense resistor footprint with a via to the other side. That has to be the roundest via you have ever seen. It's not a large via by any stretch of the imagination: it has a 10 mil hole, but the very thin plating and lack of fill makes it seem very wide. Anyway, also visible on the photo is the exceptional solder mask and especially board outline alignment. That there is copper within 5 mils (0.127mm) of the board edge. Nobody on conventional 0.6mm+ thickness FR-4 will allow this because of machining tolerances, but here you can.

Anyway, it's not all glorious. This is great technology to be able to use at a low price, but for FPC quality, it is not quite the best. The gold plating is even thinner than on their 2/4-layer service, and the plating is incomplete with rough edges at places where copper dives underneath the solder mask. Another small heckle I have is the horrendous silk screen:

That is some crusty silk screen, and this is especially bad on a flexible PCB. On one side lines are missing or very thin, on the other the lines are too thick and there are some extra blobs (e.g. the blob on the side of the '0' in 'rev0'). Alignment is not very good - look at how far that silkscreen has shifted inside the SOT-23 footprint. Also, the resolution is pitiful.

It seems to me that they use the same screen printer here as they do for other technologies, but the problem with that is: on flex PCBs, you want to use smaller components. Whereas 0402 is the smallest you can do with 6/6 design rules on their standard process, on here you would definitely want to go 0201 or 01005 with 0.4mm pitch QFNs and BGAs, and it is absolutely impossible to make part outlines on the silkscreen with this coarse of a screen printer. And another important problem with the silkscreen is its sheer thickness: it seems to be almost thicker than the copper and soldermask! I hope this service will switch to either a much finer mesh screen printer or even better photographic silkscreening in the future, which yields results like this (from Eurocircuits):

Isn't that much better? Even though it's slightly overfilled, those (equally thick) lines have much better definition than Iteadstudio's service. By the way, that 1.6mm PCB now looks enormous, doesn't it?

However, even though it should have been obvious already, the most important feature of flexible PCBs is their... well, flexibility. I was worried they would mess this up or refuse to produce my design, but they did it and it worked briliantly. I am of course referring to the strip of very thin board in between the business end of my board and the connector side. Here is the board with components installed, and the bendy bit functional:

Those are actually 2 mil wide traces, 6 in total (3 on top, 3 on the bottom), on a strip of mylar base material that is just 1.5mm wide. And they produced it without a problem! Unfortunately I could not get a lens close enough to the traces to show you how extremely clean the edges of those traces were, but I am actually confident that I could draw 1 mil traces and they would be able to produce it. Marvellous.

Oh, and also...

They put the code in the little box I made for the code! They listened to me! Iteadstudio, just for this you can expect a lot more orders from me in the near future. And Seeedstudio, shame! Itead can do it, why don't you!


This has been part two of this series that shows the quality of cheap chinese PCB services, and I have to say I have been looking forward to this. Five years ago I was etching my own PCBs with toner transfer and horrible methods like that, and now for less than the cost of one hour's pay I can order 2/2 mil flex PCBs from China.

The quality is great for the price, but if anything I'd like the plating quality to be a bit better, the silkscreen definitely needs some more work and ideally - but this is honestly just a consequence of being pampered with other services - I'd like the turnaround to be a bit quicker. We've had 1-week turnaround for everything from 0.6 to 3.2mm PCBs for a couple years now with DHL shipping, so I'd like for FPCs to eventually get there too.

I hope this blog will help my fellow electronic design engineers and for now, happy designing!

Seeedstudio 4-layer PCB quality

Door mux op vrijdag 3 januari 2014 20:11 - Reacties (9)
Categorie: -, Views: 62.372

Today I'd like to delve a bit into PCB quality, features, delivery and pricing of the most well-known PCB prototyping services around today. I have been using quite a large selection of PCB manufacturers for over 100 PCB designs (and revisions) since 2007. However, this was mostly 2-layer design - to keep costs down. Recently I have been tasked with the design of quite a few unusual designs on 4-layer and flexible PCBs, so this seemed like a good time to evaluate PCB and stencil quality from the arguably best value sources on the internet. This is part one, where I go a bit into the history of PCB fabs and show you how well faired with my 4-layer order.

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 prototyping

First 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 around
Well, 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 quality

So 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 materialFR-4 1.55mm
35µm outer layer copper thickness
18µm inner layer copper thickness
Surface finishENIG (Electroless Nickel Immersion Gold) ~2µm
Board size150x25.4mm
Solder mask colorRed
Amount ordered/received in good order5/5
Price$105.90 + $29.24 shipping (DHL)
Total time11 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.

Conclusion 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 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:

::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\ .\seeed\*

:: remove temporary file
del filelist.txt

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's flex PCB quality and's paste stencil service.