HOW-TO: Get your PCBs manufactured

in tutorials by DP | 21 comments

The latest version of this tutorial is available on the documentation wiki.

In the last few years many inexpensive PCB services have popped up. It used to be that buying PCBs in hobby quantities was expensive and filled with gotchas.

Now, places like Seeed Studio can send your PCBs to the inexpensive prototyping factory in Shenzhen China, and ship them anywhere in the world at great prices. You get two-sided PCBs, with the works, starting at $1 per 5x5cm PCB. Turnaround is a few days, worldwide shipping starts at $3. It’s a happy day for electronics hobbyists.

Other services like DorkBotPDX and BatchPCB pool multiple orders so the group benefits from bulk pricing. Enough people are using these services that turnaround is quite fast. DorkBotPDX offers signature purple PCBs that have become quite popular.

Our goal is to help you get your Eagle PCB designs manufactured. We show our ‘pre-flight’ checks to help spot problems before ordering boards. Learn what defects to spot, like under etching, over etching, and misaligned vias. How-to continues below the fold.


Check for air wires

It’s easy to miss a small break in a trace, and Eagle doesn’t provide any flashing warning signs. The zoom-unrouted ULP script will zoom in on any broken traces and save you headaches later.

  1. Download zoom-unrouted.ulp
  2. Run it: File > Run… > zoom-unrouted.ulp
  3. Eagle will zoom in on any air wires
  4. Add the missing traces if any are found
  5. Run it again until no new air wires are found

Polygon fill isolation

A common error is when the ground fill or ground plane is connected to a trace. This is a symptom of under-etching at the PCB factory, and it can be minimized by using a reasonable isolation distance.

If you use a ground plane or other filled polygons on your board, be sure to increase the isolation to at-least 12mils (16mils+ recommended, depending on manufacturer).

  1. Right click on a polygon’s edge
  2. Go to: Properties > Isolate
  3. Set the value

Picture by Sebastian CC-BY-SA.

Design rule check

Make sure your design is within the specifications of the PCB service you use. Most hobbyist-friendly PCB services provide an Eagle design rule check file that can highlight anything that can’t be reliably produced.

These services all provide a DRC file that works in Eagle:

Eagle processes the DRC file and evaluates the board automatically. To run a design rule check:

  1. Open your PCB layout in Eagle
  2. Go to Tools > DRC…
  3. A DRC window will open. Load the manufacturer’s DRC file.
  4. Click ok to start the check

From the DRC window you can adjustment the various design specifications like minimum trace width, clearance, etc. If a board doesn’t need the smallest stuff the factory can make, we increase these settings a few mils as a safety margin.

The DRC will scan your board and log all the areas that go outside the manufacturer’s limits. Click on various log entries to highlight each problem on the PCB.

After fixing the errors, run the DRC again to see if everything passes. Rinse and repeat until the board passes the DRC.

Generate gerbers

Once your board is electrically sound, it’s time to generate files that the manufacturer can use in production. Gerber formatted files, usually just called gerbers, are files any respectable PCB house can use to make boards.

We’ll generate them using a CAM file provided by the fab:

Follow these steps to generate gerber files:

  1. Open our PCB files in Eagle
  2. Start the CAM processor: File > CAM Processor
  3. A CAM Processor window will pop up
  4. Go to: File > Open > Job… and select the CAM file
  5. Click on the process job button

The gerber files will be saved in the same directory your Eagle source files

Each gerber file represents a layer of the PCB. They’re like a PDF for circuit boards, any manufacturer should be able to open the files and make the board if it is within their ability.

  • GTO Top Silkscreen (text)
  • GTS Top Soldermask (the ‘green’ stuff)
  • GTL Top Copper (conducting layer)
  • GBL Bottom Copper
  • GBS Bottom Soldermask
  • GBO Bottom Silkscreen
  • TXT Routing and Drill (the holes and slots)

These are the seven layers/files typically required to manufacturer PCBs.

Preview gerbers

Before you send the gerbers to the board house, preview the files and make sure they look reasonable. You’ll need a Gerber viewer, here are some free ones:

We use ViewPlot. To view your files:

  1. Start ViewPlot
  2. Go to File > Load Files
  3. Select the 7 gerber files (GTO, GTS, GTL, GBL, GBS, GBO, TXT) and click “Open”
  4. A window with a list of the files will pop-up, click “OK”
  5. On the next screen (shown above) select the “Leading zero suppression” radio button, then select “2 4″. Click OK

You should see a version of your PCB with each layer displayed as a different color. Scroll through the layers using the lower left corner drop down menu.

Look for any errors that might have happened before or after generating the gerbers. More common ones are:

  • Problems with the footprint, the solder pad is sometimes buried by mask.
  • Drills outside board or flipped.
  • CAM didn’t export expected silkscreen layers.
  • Evaluating not only whether a silkscreen is present, but if it’s legible (size, location, etc).
  • Quickly seeing whether all of the vias on a board are tented or not.
  • One last check to make sure soldermask is on the correct side for the correct component (PCB’s that have components on both sides).

Zip up the files and submit them

Now the gerbers are ready to go to the board house. Each service has different requirements, but most involve zipping the files and emailing them to someone. Submit by email to Seeed Studio, Itead, and DorkBotPDX. Upload via web page at BatchPCB.

Get your boards

In our experience, you can expect to wait about this long from order to your hands:

  • Seeed Studio, from 2 to 4 weeks
  • ITead Studio, from 2 to 4 weeks
  • DorkBotPDX, around 2 weeks
  • BatchPCB, from 2 to 4 weeks

Seeed and ITead offer cheaper boards if you only test 50% of them. The tested boards will be wrapped in masking tape and/or marked on the side with a marker.

Inspection

Before you build the first PCB, spend five minutes looking it over. E-tested PCBs will nearly always be good. If a PCB is untested then you absolutely must inspect the board, or risk a broken or shorted trace under a chip that you’ll never be able to find.

Here are three common problems. Eliminate these and save hours and days of debugging headaches.

Shorts

Under etching leaves extra copper that connects traces together. Avoid this by:

  • Use larger traces and increase the distance between them
  • Check your board house production limits, avoid working with the smallest traces and spacing

Broken traces

Over etching removes too much copper and breaks traces. Avoid this by:

  • Use larger traces
  • Check your board house production limits, avoid working with the smallest traces

Image source: Greeeg CC BY-SA

Misaligned vias

The hole that connects two layers is drilled outside the via. This might break the connection between layers, or connect a trace to another nearby trace.

Avoid this by:

  • Using larger vias and larger annular rings (the copper pad around the via hole)
  • Check your board house production limits, avoid working at the smallest sizes
  • Increase any ground plane isolation so slightly miss-drilled holes don’t short the trace to ground

We need a picture of this, can you help?

Conclusion

Good luck with your PCBs. Don’t forget to share your latest creations in the project log forum and through the contact form.

This entry was posted in tutorials and tagged , , , .

Comments

  1. As of a couple of months ago, iteadstudio now does 100% etesting of PCBs.

    • arhi says:

      Davies, I got some 100% e-tested boards from ITEAD, there were no marks on the pads from sharp end of the probes so it’s really hard to truly believe they actually tested them… Second problem is – bunch of vias were not even drilled trough, and bunch of other errors on those “100% e-tested” so I have troubles trusting this 100% e-test ITEAD is selling :(

      • arhi:
        1) Do you have photos?
        2) Did you send them to itead to give them the opportunity to correct it?
        3) Did you actually test the board yourself? (Remember, the board may still electrically function and pass an etest with these flaws if there are multiple vias in your net.

      • arhi says:

        Davies,

        - no pictures, this “failure pictures” thread was not up then and I don’t feel any joy in taking pictures of that type of failures (ones that you can’t learn from)
        - no, sent nothing to ITead, I tried communicating with them few times and it was extremely hard to understand them, and the forum they have is hard to track as it is full of spam (looks like they don’t clean it, and as they don’t have any protection)
        - of course I did. Not all boards were broken, 6 boards had a missing via’s, only 3 boards were actually failed (as other 3 boards had only ground via’s missed but ground was attached trough some other path). I noticed missing via’s immediately but boards worked fine, then I stumbled on the 3 non-working boards where some required via’s were missing :(

        What is weird is that previous boards I was getting from ITEAD always had half of them marked and those half had small dots in the pads from e-testing. This batch had no marks on pads on any of the boards so mine conclusion is that they have their own testing machine and that they are doing testing while factory is not testing anything any more, but that their own testing is not e-test but a visual inspection gear. I had some experience with visual inspection gear and they find all over/under etching problems but they don’t find missing and poorly plated holes, and they don’t leave the “dots” on the pads… anyhow, might be just a glitch, won’t prevent me from ordering pcb’s from ITEAD in future :D, it will just prevent me in “trusting the 100% e-test”, I just have to inspect every board myself before using it.

        Did I mentioned that I found tip of the drill bit in one of the pcb’s? It’s obvious that drill failed there (tip of the bit is stuck in pcb) and then missed to drill holes further down the process.. I think I have that board somewhere, I’ll try to find it to take a picture of it

  2. Arup says:

    So long I was waiting for this comprehensive guide. Thanks @Ian and crew.
    BTW, when we’ll see the PCB mailing video?

  3. Frank says:

    I’m sure a lot of people does this, print out a 1:1 scale copy of the layers on paper to verify sizes of footprints and silkscreen text and stuff

  4. Hey dangerousprototypes,

    I’ve been reading you guys for what feels like forever and I just wanted to say Thank You. I don’t think I’ve ever read any of your articles and not appreciated them.

    So, again – thank you.

    Y’all awesome.

  5. Carl says:

    Hey,

    Just sent another simple board to ITead. Sent out a couple before their break, got them there 2 days before the cut-off they had published, and they still didn’t process them pre-break.

    The one set I was really eager for (they went to different addresses), so UPS was paid for to get it here quicker. They screwed up the address, shipping, etc so it showed up over a week after the air mail package.

    Boards looked good, some off-center drill in via, but not much else to complain about (thus the second chance).

    Built 10 boards up, 10 worked as expected (5 each of 2 designs). I will let you know how this next order goes, it is a simple board for a dual stir plate for home brew using the lm317 and national’s reference design, so only a handful of parts.

    –Carl

  6. Alan Rosenthal says:

    Electrical testing – is it worth it? I would love to know if its worth the hassle (time is worth more than money) or it’s just an added fee that people get just to be sure.

    What does 100% electrical testing get me that 50% doesn’t?

    How often are there errors in fab?

    How do they actually test it?

    Has anyone experienced a bad board even though they get the testing?

    • Ian says:

      Hi Alan,

      We only build on tested boards, it’s not worth the hassle of building up a potentially busted PCB.

      50% vs 100% etest means that half or all of the PCBs are electrically tested.

      Errors vary with the tightness of tolerances on your PCB. They certainly do occur.

      They test with pins that know what parts of the board should be connected based on the gerbers. Any breaks or shorts are detected.

      Arhi had tested boards that were bad, but they had no indications that they were tested or passed (a marker on the side usually).

    • rsdio says:

      I don’t have much data to go on, but I recently ordered 60 boards and got the RoHS report which included some numbers. They manufactured 72 boards to meet my order of 60. 5 boards failed electrical testing. That’s about 7%. Parts for each board are $32.21, and assembly is $11.25, meaning I would have lost over $200 without the e-testing if I had stuffed them only to find out that some were bad.

    • Laen says:

      E-testing is just one of several checks a fab can do, and the closer you are to your fab’s capabilities, the more important e-testing becomes.

      My fab relies primarily on automated optical inspection. Each board is scanned in at several steps of the process, and compared with the gerbers. They go down to 3 mil traces and clearances, so the 6 mil clearances we throw at them are downright spacious.

      In practice, this combination has worked pretty well. My reported failure rate due to fab errors is about 1 in 15,000 boards.

      That being said, if I were making a product for sale or putting $200 in parts on a board, I would want them electrically tested. It doesn’t add much to the cost if you’re ordering from a fab directly.

      • rsdio says:

        Seems like it might be best to know your fab and ask them what they recommend. If they’re happy with optical instead of electrical testing, then that should be good enough. I’ve just had a hard time with some fab houses when asking them for suggestions. Other fab houses just include e-test in their quotes, so they obviously recommend it.

        Of course, I’m talking about full-price PCB making, not the ganged stuff from smaller shops. I think the same questions are valid, but the pricing can be vastly different once you get to a shop that is including e-test in their price quotes.

  7. kuhltwo says:

    Great article. Finally something this “old schooler” can follow. I am from the tyme when everything was done by hand.

  8. Hi Guys! I just want to give some props to Seeed Studio for making my PCB’s. I got them in about 3 weeks, had them 100% tested, and they were visually and technically beautiful. I made my first kit to sell (RGBW LED Controller) and it was also my first project in Eagle. I must of gone over the boards 12 times, but it really paid off, no problems at all with any of them. I had ordered 50, and they sent me 52. :)

  9. Sleepwalker says:

    Perhaps Ian is best qualified to answer this – How good is the quality with Seeed? I’m assuming it’s pretty good being that Ian uses them all the time? Laen’s quality is great and I’m really happy with the service, but the purple boards just don’t suit our needs and I haven’t been able to convince him to offer other colours like Green, etc., so looking to give Seeed a go. A friend who runs a small business is in the same boat, he likes Laen’s quality, but wants red, so Seeed might be the go.

    • Ian says:

      Protoboards from Seeed are sent to a local proto factory in Shenzhen. It’s the same factory used by Itead, and probably several smaller eBay PCB outfits. I have never had a problem with the boards, but they are intended for prototyping only. If you order 100 boards, for example, they go to a different factory (is my understanding), and are production quality. The difference is like a quick inkjet or laser printout compared to proper offset printing. Both are readable, but inkjet and laser is a fast, cheap process for 1-offs that doesn’t produce the quality of an offset printer making 1000s of pages for a book.

      In practice, I have noticed this to mean:
      Proto boards tend to have silk screen issues. Smears, unreadable parts, poor “dot matrix” appearance of text. This happens on maybe 1 board on every few batches of PCBs (1 out of 30-40 PCBs). Production boards have perfect “beautiful” silkscreens.

      Proto boards are a slightly different color. Production boards look more like powder coated metal finishes. I don’t think this effects quality…

      Proto boards have somewhat uneven tinning. Pads will have slightly varying amounts of tin spread unevenly, while production boards are perfect.

      Untested protoboards are liable to have shorts, breaks, or drill problems. This depends on how bad you torture the board house with tight designs. This is no longer an issue for us, all our boards from Seeed seem to be 100% tested (included in the default price) now.

      None of these things effect the usability of the (tested) PCBs. Overall I give the protoboards a HUGE thumbs up for making PCBs more available than ever. It sure beats slaving over a hot acid bath and printing my own negatives. The production boards made in larger batches are as good or better than anything else I have seen, but maybe you’ve seen some super quality boards :)

      • Sleepwalker says:

        Thanks for the detailed info Ian. Interesting that it’s the same proto fab as Itead, as I’ve seen a fair few complaints about Itead’s boards, but not Seeed. Will probably try it and see, at the prices they charge I guess you can’t go too far wrong.

Leave a Comment

Your email address will not be published. Required fields are marked *

You may use these HTML tags and attributes: <a href="" title=""> <abbr title=""> <acronym title=""> <b> <blockquote cite=""> <cite> <code> <del datetime=""> <em> <i> <q cite=""> <strike> <strong>

Notify me of followup comments via e-mail. You can also subscribe without commenting.