No Script, No Fear, All Opinion
RSS icon Home icon
  • EEVblog #155 – ITead Studio PCB Prototype Goof

    Posted on March 11th, 2011 EEVblog 83 comments

    Dave shares an experience with his new prototype PCB’s from ITead Studio.
    Super awesomely cheap, but beware!

    Be Sociable, Share!

    74 responses to “EEVblog #155 – ITead Studio PCB Prototype Goof” RSS icon

    • Ha! Well, you get what you pay for. Or…now you know you should design for something like 8/8′s?

      I really enjoyed this video – there’s something really fun about PBC layout. I hope you do more videos like this – this was a great real world lesson.

      Question: When you designed the board, did you know that the ground was snaking it’s way around and through the pins? Or did you just add a copper pour, and your software said “ok, that trace is done” and you went on your merry way?

      • A board like this did not let me use 8/8 rules.
        I can do my own 8/8 boards at home, 6/6 at a pro PCB house is a piece of piss.
        It wasn’t their process capability that went wrong, it was them fiddling with the gerbers when they didn’t need to.
        Yes, when routing I knew i needed that copper pour to go that way, it was the only way to route out those ground connections.

        • Why didn’t you place the via somewhere closer?
          But after all, they messed it up too :/

        • Hi

          I usually route all the connections with traces and then I might cover them up with copper pour, thisway, even if the copper pour fails I still have traces going underneath it. I think thi would help to prevent mistakes in manufacturing

      • @George Graves

        >Ha! Well, you get what you pay for.

        He paid what he was asked to pay otherwise he would not have the board in his hand.

        Do you think that he paid a few less pennies so thre removed his copper?

        Those cheapsters also messed up my board.

        I encourage to ask for refund if such things happen.

      • Good review, I changed their design rule and made it 10/10. I do not trust any board manufacturer with lower than this until proven. I have done better boards (TSSOP package with clear pins) at home using FPC board from UK.

    • Ahhh yes – I wasn’t saying it was you – it’s very clear in the video they expanded/shrunk that area.

    • Dave,

      Thanks for the video, thanks for blogging about the service. I didn’t see your note on twitter :) Even with the problems, ITead Studio looks like a very reasonable alternative to making PCBs at home.
      I have just one question: did you order the boards with e-test? If they were tested, guys ITead should eat the fu**d-up boards and send you new ones. However if they weren’t… Well…
      I think that the price even with the extra US$10 for testing is still very attractive.
      One more thing: how long did you wait for the boards?

      • Yes, 5 of the boards have two red marks on the edge which indicates testing I presume. Those boards actually measure ok, and on inspection there is the smallest slither of copper making the connection. Probably well under 1 thou.
        They stuffed up either way. My 8 though trace being expanded down to a 1 thou slither is unacceptable.

        • It looks that the 6/6 specs that they brag to seem to be fiction. I can imagine that they modified the gerbers because their process is not able to handle such clearance.
          Another option is, that it is a “subtle” suggestion to pay the extra money for the testing :)

          • Their process (or actually, their board manufacturers process) is easily able to do 6/6, as traces were 6/6 and turned out just fine. The ground plane is separate issue to that.
            Testing means very little. Some of the were tested “good”, but the traces are 1thou or less which is hardly a reliable solution.

        • Dave, I obviously agree. Either the gerbers
          should have been processed as-is without alteration
          or the order should have been paused while they
          consulted with you.

          Looks like they are still doing the clandestine
          gerber modifications as the boards I just ordered
          showed up with polygon power/ground plane breaks
          for the exact same reason. The copper-to-copper
          space used in my layout was 6-mil but this was
          modified by them to 12-15mil. My layout being quite
          tight, loss of plane polygon width to that degree
          either separates the polygon or results in a hair-line trace unacceptable for a power feed.
          The other annoying modification was the 0.3mm
          vias called out in my layout wound up being ~0.45mm
          leaving near nothing for the annular ring. 0.3mm
          vias ARE advertised as being supported. They
          also cut a few SMD pads on one edge of the board
          even though I was under the 5cmx5cm size which
          isn’t acceptable either. Finally portions of the
          silk screen component legend were relocated
          paradoxically to fall on a thru-hole where they
          wound up being clipped even though I took care to
          position the silk legend on undrilled copper such
          that it would fully render. While this doesn’t
          create a problem it is quite bizarre.

          As a comparison I have boards from another manufacturer created with the exact sane gerbers
          which were produced verbatim. At 6/6mil
          trace/space, 0.3mm finished hole, we’re not exactly
          pushing state of the art here.

          I’m don’t at all intend to dump on ITead Studio
          for this and if the reports I read are accurate,
          they are just an intermediate in the process.
          But I wish they would demand their board fab to
          cease modifying customer designs. Even if they
          respin the boards I’m looking at another 3 weeks
          to get functional boards which seriously detracts
          from the otherwise attractive price point of
          their PCB service.

          If anyone is interested I’ll provide jpegs of the
          boards to give some context.


    • Something is telling me we can expect an arduino-shield in the near future from Dave :3
      Hope that ITead Studio fix this issue, because the price is insane IMO.

    • Hmm, I was all ready to tell you that you goofed up and used one of the untested boards and that the untested board had an etching mistake (as in too much copper), because I have had that problem before.

      I’ve always done all the routing with wires and adding the fills as an extra on top of that, so my boards would work without any filling at all, so I guess that’s why I’ve never seen this problem.

      I guess the rule with ITead is to route all the signals you need explicitly and not rely on filled zones for actual connectivity.

    • Interesting video, Dave. I really like videos about “real-world” stuff, like trouble shooting.

      I guess you can send iTead this video and see what they have to say. I’d really like to know why they didn’t follow their own design rule specs.

    • Thanks for the “review” of Itead. I have been waiting to hear how your boards came out as I am considering using them myself. You have tested them at their design limits and they failed. But I don’t need 6/6 design rules so I will still give them a try.

      I remember reading this somewhere, “Just because a manufacturer can achieve a certain track/spacing, it is no reason to “push the limits” with your design.” Now where did I see it, Oh I remember, it was in PCB Design Tutorial by D. L. Jones. :) To be fair though you did say your design required 6/6 rules.

      Keep up the good work, I enjoy the blogs and Amp Hour.


      • To be fair to ITead, their actual manufacturing process did not fail, they easily met the 6/6 design rule they claimed. The problem is they modified my gerber file which is an entirely separate issue to the actual board manufacture.

        My board was originally 5/5, but I re-jigged it to meet 6/6. Yes, the board is tiny and routing space was very tight, 6/6 was a necessity.

    • It’s funny how much of a shock people get when I tell them about ITead.

      Just recently I spoke at Open Source Days in Copenhagen and I’ve had several mails from listeners who wanted to know about ITead, not the actual project I was talking about:)

    • Maybe they screwed it up for some free advertising. The price is certainly approaching the level where I’m getting interested. (= everyone and their dog)

    • How are ground pours specified in the gerber? I’m curious because I understand the gerber is just a file of shapes that make vector paths, but it seems like that wouldn’t be the ideal way to represent a ground pour.

      Further, your 6 mil trace goes through just fine at full width, so they didn’t mess with the rest of the gerber, just the ground pour.

      What are the parameters for the ground pour, and what parameter did they adjust when they created the masks?

      I’m very interested to hear what response you get from them.

      Sounds like you could fix it by hand simply by adding “real” traces between the pins to ensure ground plane continuity.

      • No idea of the exact detail of how pours are rendered in the gerber, but it’s a standard Altium Designer generated gerber file that I have never heard of anyone ever having any issue with.

        • Well you do have to watch out for altiums gerbers if you exported them on a 64bit machine. I almost sent a board in to fab that had a part of the ground plane mangled up in one corner causing some shorts, later i found out that most of the time it makes these kinds of errors until i tried doing it on a 32bit machine where it works without a hitch every time.

          Not sure if this is fixed yet cause i use the old Winter 09 version.

      • I’m not sure how they’re done in Altium, but I can say how they’re done in Eagle.

        Ground pours are specified as Width, Spacing, and Isolation. It doesn’t seem to make sense to think of a width of a ground pour (or, really any pour), however that variable sets the aperture used in the gerber. (A short aside about gerbers: they are defined using apertures and lines. To make a trace, you set the aperture then define the start and end points.) This means that the spacing defines the minimum line that can be made with the pour, and the lower bound on the smallest feature of the polygon shape.

        The spacing variable doesn’t really do much, and the isolation variable defines how much space to allow between the pour and any other copper. Even if the isolation variable is set to zero, the maximum value of the isolation of the pour and the isolation of any other object on the board is used.

        Once these parameters are set, the outline of your polygon is traced, just like any other trace, and the interior is filled by horizontal lines. These lines overlap, and you get your fill. It’s all very inefficient, really, but it works. You can see this in action sometimes if Eagle doesn’t think you’re looking.

    • Thanks for the review Dave.

      I’ve used iTead a few times (as well as their neighbors seeedstudio) and didn’t have any problems.

      Please do follow up with them and let us know what they say.

      At that price, it is cheaper to use them than to make boards at home or order a single board from batchpcb :)


    • What’s the lead time like? It says something when a service is so cheap you get excited even after hearing of issues they have.

      • It’s a 6 day turn and they seem to keep to that schedule. Shipping is the slow part…usually a week or 2 to the US but my order from early November didn’t arrive until late January because of a massive problem with China Post that affected thousands of shipments over the holidays.

    • From the information rendered on the Amp Hour radio show about ITead it sounds like they keep their proto board costs super low by just adding proto board orders to their larger panel runs. The smaller proto board designs must fit into extra spaces along the edges of other production run designs on the panels. If this is true then boards my not be so cheap in larger orders where you need 100+ in a run.

      Also if this is true then what could be happening is the small proto designs like Dave’s are added to the free space on larger orders and then maybe the panel as a whole is altered for that main production run and effecting the ground poor for the piggyback proto boards. Or maybe a scaling issue to the main production run design during the processing is causing this issue with the piggyback proto boards. Just guessing.

    • Well, most probably they scaled the drill to the next bigger one available and then had to scale the pads up because of the minimum annular ring requirements.

      But no boardhouse should do anything like this without consulting its client.

    • I have also managed to isolate grounds the same way though the circuit sort of worked by the being powered via logic gate input protection diodes.

      It might be worth using another gerber viewer like gc-prevue just to be sure that your file is OK. I don’t know enough about the volume PCB production process but I guess that it isn’t a photo resist / etching issue.

    • Hello Dave,
      what kind of unit is that “thau” you mention in the blog ? I’ve never heard about it. I”m only fammiliar with “milimeters” and “mils”.

    • This is probably a stupid question, but how can you tell from the pcb if they have messed with your Gerber or instead just left them in the etch a bit too long. It seems to me the result of a human error with the stopwatch would cause the same problem. I can imagine the underpaid employee not being alert after 21 hours at the etchbath rather than someone (presumably skilled) taking it on themselves to play with a Gerber file.

      But, hey, I don’t know anything about this stuff, so I’m just curious.

    • Awesome video! Thanks a lot! Let us know, Dave, what ITead Studio responds if they do.

    • Very interesting! Have you looked at the gerbers with a gerber viewer other than the one that comes with Altium? I’m trying to imagine what they might have changed in the gerbers to produce this result. After all, the “clearance” that got larger is not something that is IN the gerber; only the copper is in the gerber, and it is puzzling that that some copper parameter could be changed that would result in the increased spacing that we can all see.

      In EAGLE, which is all I’m really familiar with, a pour is drawn as a sort of raster using an aperture of size equal to the width of the wire used to draw the pour polygon. If Altium is similar, then the likely edit would have been to change the size of that aperture (especially if it had defaulted to less than 6 thou?) This might change whether the pour succeeds in going between pads, even if it would theoretically fit. Except I’d think that would be problematic WRT the edges, and would end up being a rather complex edit to make… (Hmm. If you have a 6thou raster going between pads that only have room for a 6thou trace, and the raster runs horizontally, then you’ll have a zero-length line segment and/or “endpoint issues” that might be a logical place for SW bugs to exist…)

      I’ve always been vaguely uncomfortable with allowing pours to make connections; I like to draw my boards so that even if the pours go away, the board would work. In a way, it’s nice to have that paranoia vindicated!

    • After hearing you talk about the service on the Amp Hour I took a look and bookmarked the service. I also use PCB Cart for production boards and have had great luck with them. I usually get 10 or so boards made to make sure the design is good, then order a full batch once I have confirmed that there is no issues. Only problem is if there is a few small changes to make they will charge you the tooling fee again which sucks.

      I am thinking I will still give this service a try for the next prototype and cross my fingers that the same issue doesn’t happen to me.

      Have you complained about the issue and heard back from them?

      • PCBCart only charge a re-tool fee if they need to touch the drill file.

        If you can make your changes entirely in copper layers, then they only charge $10 to change your design.

        This is really great and I have done this quite a few times.

    • Hmmm, MatrixDuino. Someone is cooking something. :D :D :D.

    • So Dave, official answer was:

      “this is the fault of designer, he don’t meet the minimum limitation, and we can not respond for it.”

      What you said on that?

      • So Dave, official answer was:
        “this is the fault of designer, he don’t meet the minimum limitation, and we can not respond for it.”

        They are incorrect, and I have posted my response.

    • But I saw the official respond on that post for this issue is “This design is really exceeded our level of ability, and we can not make it as original design. We should declared the minimum isolate on the product , but we didn’t. We will remake the boards with the new design which meet our producing ability.”

      Joker seemed to sow dissension

    • Itead’s response isn’t very consistent with the fact that the 6thou trace routed manually between those same connector pins worked fine…

    • This is not that bad compared to mine. I used some other China manufacturer and they modified my capacitive touch buttons into normal membrane button! From 4 mil tracks into 30 mil tracks.
      I always tried to avoid to rely too much on pour to connect the net and use tracks whenever possible. But when there’s no space for tracks, I’ll use a bunch of vias (lots of them) to connect them together. But Iteadstudio should do something about this.

    • Manufacturers will change your Gerbers. But a critical step is netlist compare. A decent CAM tool can do this easily. If the customer does not provide a netlist, one can be extracted from the original Gerbers and compared to a netlist extracted after the changes. This would have found your problem. (It would NOT find missing redundant connections however.)

    • This points out that one of the things you lose by going to a “bargain” PCB manufacturer is “dialog” about problems the manufacturer has (right or wrong) with your CAD files (gerber or otherwise.) With a more traditional PCB shop (at 5 times the price or more), Dave probably would have gotten a phone call “it looks like your board doesn’t meet our design rules; we’re going to need to change xxx”, and Dave would say “no, you’re wrong, you must be looking at the soldermask instead of the copper”, and everything would have been resolved before the boards were attempted. But at the price, you don’t get this amount of interaction.

      IIRC, Sparkfun had exactly this problem when they first started their batch PCB service; they were getting sent all sorts of boards that “needed to be discussed”, but they couldn’t afford to do so at the price they were charging.

      I’m somewhat impressed that ITead modified the design at all; usually at the bargain price, if you violate the design rules, you just end up with boards that don’t work. (of course, in this case, ITead was wrong and the board would have been better off with no modification, but I’ll bet they get plenty of boards where their intervention is in fact helpful…)

      (Interestingly, I’ve been considering using ITead as well, and this entire incident is remarkably … neutral … in affecting my decision.)

      • We still don’t know what the real reason behind the modification of the gerber or why, so unless someone else did the same design and confirmed it as a possibly a standard process by the manufacturer, then it could just be a one-off problem.
        Certainly no reason to give ITead the flick, at the price they are well worth giving a go.

    • I submitted a gerber file to ITead and they came back to me asking to recheck my gerbers because it looked like I was missing a component. Sure enough when I rechecked the gerber I had accidentally removed a component when doing some last minute tidying up. Completely my fault, but thanks to their checking I was able to put it right and send new files without having received boards that would have been useless. A big (y) to ITead.


    • That sucks. Looks like it might be easy enough to fix with a green wire or two, but I’d be curious to see how ITead resolves this, if they do anything at all. I’d love to find a good cheap and fast PCB service, but if they honk up my boards, it’s not worth it.

      One question:

      How did you “know” that it wasn’t capacitive loading on the circuit by your scope? Obviously you found the issue, but you mentioned that it wasn’t capacitive loading but only because you “knew” it.

      So… How did you know that it had to be the PCB design and not a loading issue from the scope?

      • Strictly speaking, I couldn’t know for sure at first, it could have been either in theory, but the grounding issue is a very common one, and the signal I was probing was coming from a low impedance source of a known good external circuit. So it was orders of magnitude more likely to the ground problem.
        Then a simple test to confirm the theory was to try it with only the ground clip in place, and bingo, that proved it.

    • Hi Dave,

      @4:00 you mentioned sometime a circuit works when a scope probe is attached at a point because of capacitive loading and it is a classic problem. Can you do a future blog how to fix problems like this?

      I am seeing the same phenomena in my setup where I have I2S output and measure them using Audio Precision but does not work and as soon as I put scope probe in my clock pin, circuit magically works. Obviously with capacitive loading, timing seem gets to be correctly. I suspecting long test lines. It would be nice to have a blog where a different causes of this sort of problem are given and may be possible cures are shown. This is very practical and look forward to any feedback from you.

      Love your work so far! Please keep it up.

      Audio Application Engineer

      • For starters you need to use a x10 probe which has lower capacitance than x1 probe. But they can still affect oscillators by loading them. In that case you need a special low capacitance FET probe.

    • Dave, I’m sorry for criticizing, but this is a good example of bad PCB design… :) You shouldn’t hang all supply on such small area of copper. And a few more “not ideal” things can be seen only in the still picture, without even playing the video.

      • Rubbish. It’s perfectly fine PCB design practice given the circumstances. BTW, it’s not the main power pin, and hte current is low anyway. 8 thou copper pour thickness is relatively HUGE. Plenty of margin.

    • Seems to me that Dave relied on a copper pour to join the “common” net. This would be Dave’s fault in either not going through his design properly or by not having put in a trace prior to the copper pour. Putting in all traces insures that errors like these will not happen. DRC rules can check for most design erros, although a specification in the copper pour would be needed to ensure that all “joining pours” have to meet certain requirements. This is a nice debugging and bad practices video, although the complaint part could have been dropped. Sorry Dave, from my point of view, you screwed up.

      • Rubbish. It is perfectly common practice to do this if you are professional who knows what they are doing. You should never have to put in traces under flood pours “just in case”. I knew exactly what I was doing, and fully inspected my final flooded design, nothing wrong with that.
        The trace was a whopping 8 THOU, that is massive, and gave plenty of design margin for overetching etc.
        When you get your PCB manufactured professionally, you rely on and expect your gerbers not being touched and certainly not modified as grossly as this.
        Just because having a trace under my copper pour would have saved me in this unusual case, does not mean that must be done on designs as a matter of course.
        Also, you are saying I was NOT supposed to complain about the copper pour on my gerber being modified and completely eaten away by 8 thou??
        Maybe for the price, but geeze, this is just a really bad issue for any PCB manufacturer, cheap or otherwise. Luckily ITead agree and are talking with the manufacturer to figure out what happened.

    • Dave,

      What drill size did you specify and what did they drill it at (did you specify smaller than their minimum)?

      By inspection the hole they drilled looks roughly the same size as your pads in the gerbers.

      If they rounded the drill up to the next size they might have increased the pad size to maintain the minimum annular ring. They would then have to cut back the pour to maintain the clearance which lead to the break in your GND net.



    • Looks like Itead have changed their DRC spec. Now reads “6mil, >8mil recommended”.

      Thanks Dave. This has been very informative.

    • Nice informative stuff as always!Thanks for taking time to share your great experience and knowledge through in this video posting..Great job done keep it up..

    • They provife 100% e test now you know!
      But I wonder if they compare the PCB with your original design or something else.

    9 Trackbacks / Pingbacks

    Leave a reply