Colin Karpfinger

14Jun/10Off

Ordering PCBs Designed With EAGLE

So you've figured out EAGLE's design quirks, you've routed all your airwires and you're wondering what next.  This guide will take you from a .brd file in EAGLE to a professionally made PCB.

As of now I've ordered somewhere between 15-20 boards, which seems like enough to find the common pitfalls.  I now exclusively use Advanced Circuits (http://4pcb.com)  They are quick, reliable, and relatively cheap (in that order).  This guide will only really cover their system, but the files you're creating will work to quote with most other places as well.  You are making Gerber files, which are the industry standard.

Step One - Double Check Your Work

Schematic Checks:

  • If you're using off page connectors, are they connected on both schematic sheets?
  • Are your nets in the schematic actually connected?  Sometimes when copying a part, it may appear a net is connected, but isn't.  To make sure, move each part and see if all it's connected nets move with it.  If you move an IC or other part, and the traces that are supposed to be connected don't move, they aren't connected.
  • Need a reset switch for your microcontroller?  I tend to forget these.  Sometimes they are nice to have.
  • Do you have a couple LEDs on GPIO lines for debugging?  Also handy.
  • Do you have a serial Rx/Tx swapped?
  • Explain the functionality of each block to yourself or to someone else, out loud.  This really does help.
  • Thermal/Mounting  Tabs or Pads connected as expected?  Sometimes these should go to ground, sometimes to power.  Make sure you've got it right.

Board Checks:

  • Are you using the correct footprint for your ICs?  Check their dimensions using the 'Mark' tool in eagle.
  • Can you buy your ICs in the footprint you designed?  Worth checking, this one has screwed me in the past a few times.  Make sure they're not only in stock, but that you can buy individual quantities, not just a roll of 4,000.
  • Is the footprint given in the datasheet a bottom view?  I've been nailed by this one before.  Be especially careful with modules- pinouts are often shown from the bottom view.
  • If you have a ground or power plane, turn off all layers but those, and note the path current will take.  Is the current following an unnecessary loop?  Is the return path of your digital circuit cross paths with any analog circuit blocks?  If so move things around to fix the issue.
  • Print out a 1:1 ratio copy and compare it with any parts you already have stock of.  This is a little over the top, but a nice sanity check.
  • Order your parts for the board before ordering the board, if possible.  This will tell you if anything is out of stock, or not available in the package / footprint you want.

Let's run the EAGLE DRC (Design Rule Check)  It isn't a catch all, and will sometimes have a lot of false positives, but it will save you at times.

  1. If you are going to use Advanced Circuits (4pcb.com), download my drc file: typical_4pcb.dru.  Inside EAGLE, on the left command bar, click here:
  2. Once the DRC window opens, click Load and browse to typical_4pcb.dru
  3. Click Check
  4. Go through the results.  Don't worry if there are lots of errors- sometimes the large pin count chips have silkscreen that overlaps the copper pads, and this will generate >100 errors.  You can ignore those, Advanced Circuits won't print silkscreen on copper.

Lastly, run the ratsnest command one last time.  Make sure it says 'Nothing to Do'.  If not (it might say Airwires: 2) then you have to route those signals or your board won't be complete.

Step Two - Run the CAM Processor

  1. Click the CAM processor button:
  2. File -> Open Job -> gerb274x.cam (or gerb274x-4layer.cam if you have a licensed copy of eagle and want to do 4 layer boards or put silkscreen on the top and bottom layers)
  3. Go through each tab, make sure 'Mirror' check box is NOT checked.
  4. If you have a logo on your silkscreen, make sure you have the layer selected in your Silk Screen tabs.  I typically use layer 200 for Logos on the top of the board (Silk screen CMP), and layer 201 for logos on the back of the board (Silk screen SOL).
  5. Click Process Job
  6. File -> Open Job -> Excellon.cam.  This will generate your drill data.
  7. Make sure the 'Mirror' option is NOT checked.
  8. Click Process Job
  9. All of these files will have been created wherever your .brd file is located.  Tip- if you open that folder before you run the CAM processor, they will all show up together at the end of the folder.
  10. Create a new folder and name it YourDesignName_Alpha1a.  I typically use Alpha / Beta to switch between major changes in functionality, the number (1) to switch between revisions of actual circuit boards, and the letter (a) to switch between small revisions when getting files ready for fabrication.  If you send the files in and have to change something small, re-run the cam processor and bump the name to YourDesignName_Alpha1b
     
  11. If you're doing anything fancy, like including score lines so you can snap pieces of the board off, you may want to include an assembly drawing.  This can be super simple- I just export an image from EAGLE by using File -> Export Image, and then I just add some basic info in MsPaint (say what you will, it is quick and dirty.  I can be done before photoshop even loads).  This will prevent them from putting your designs on hold in certain cases.  If you have an edge-mount connecter, they will often put it on hold if you don't specifically say you don't need gold plating.  Here are some examples:
  12. Put the files in a zip folder (including your drawing if you have one).  In windows I just right click on the folder and Send To -> Compressed Folder.
  13. You can verify your gerber files by opening them with a free Gerber viewer.  I use GerbV for this.  Functionality within a viewer is pretty limited- so try to just open the files and make sure everything looks mostly correct.  The big errors you'll catch here are missing layers, missing silkscreen, mirrored layers, and dimension errors.After opening GerbV, click the plus in the bottom right Browse to your folder, and select all the files.  You may get a few error messages, but you'll end up with something like this:

Step Three- Submit Your Files

  1. Go to http://www.freedfm.com/ Enter your email / find your zip file
  2. Click upload Zip File, and you'll get to this page:The site should recognize most of your files.  If not, see the above image for reference.  If you have internal layers for a 4 layer board, it will ask you the layer and polarity as shown above.  If you're doing a 2 layer board, ignore the files .l15 and .ly2For all the files that say 'Select One...', just select 'Drawing/Other'.
  3. Fill out the 'General Information'.  Just about everything is self explanatory. (If not, email me.)
  4. Click submit.  You'll get an email in about 5 minutes if you're lucky.  Sometimes it takes them longer.
  5. Your email will have the subject line:  Your FreeDFM.com results for your design YourDesignName
  6. Check the link in the email that says DFM Results.  With any luck, it will look like this:
    If there were any Show Stoppers, don't worry- you can typically fix them pretty quickly. Don't worry much about the automatically fixed problems- they're usually just silkscreen issues.

Step Four - Order the Copper Clad Bastards

  1. Advanced Circuits fortunately has many deals and promotions.  If your board is fairly standard- standard thickness (.062"), doesn't have super tiny traces / doesn't need to be scored / standard weight copper, then you can get a damn good deal with their 33each special.  You can get a minimum of 4 boards for $33/ea with a week turn around.  If you're a student, there is no minimum order.  Damn good deal.  If you can get a PCB for $33, there is almost no reason to etch your own.  Etch a board once for the experience, but why waste your time?
    Official 33Each specs:
    # Min qty 4
    # Lead time 5 days
    # 2-layers, FR-4, 0.062", 1 oz cu plate
    # Lead free solder finish
    # Min. 0.006" line/space
    # Min. 0.015" hole size
    # All holes plated
    # Green LPI mask
    # White legend (1 or 2 sides)
    # 1 part number per order (extra $50 charge for multiple parts or step & repeat applies)
    # Max size 60 sq. inches
    # No slots (or overlapping drill hits)
    # No internal routing (cutouts)
    # No scoring, tab rout, or drilled hole board separations.
    # Routed to overall dimensions
    If you fit the above, go to http://33each.com and resubmit your files there.If you 'are a company' (can show LLC / corp status) then you can get $250 off two separate orders for a total of $500 off.  They really do push you to show proof of LLC status.

    They have random other deals, so if you're pinching pennies, call them and just flat out ask which deal is best.  Look through the deals page first.  I do this almost every time, and sometimes they have random $100 off promotions.  I've also had them cut me non-standard deals when working on university projects.  (Shout out to my 4pcb local reps: Thanks Jackie and Heather!)

Lastly, enjoy your popcorn.  You'll see what I mean when your boards arrive.

Print This Post Print This Post
Comments (7) Trackbacks (0)
  1. Nice work, Colin!

  2. Thanks for the advice!

  3. Thanks, that was a lot of help!

  4. At last. Someone who tells you what is needed to get a working PCB manufactured.
    Thanks!

  5. Thanks! My first board is all done, but I’ve spent all day trying to figure out how to package it up to send it to none other than Advanced Circuits. Thanks for the great, straightforward info to get me over the finish line!

  6. Thanks Colin. Great tutorial.

  7. Thanks for a great run-through. I especially appreciate your lists of checks at the beginning — always important.


Trackbacks are disabled.