xtal design labs incorporated
custom embedded development

xdesignlabs

products

xMega
xTach
xLogger
xLED

projects

digital tach
palm adc

xtal's reference

avr guide
pcb tutorial
bookshelf
companies
chip review

pcb production tutorial

getting your PCB made from cadsoft eagle

introduction:

disclaimer: I am not affiliated with Advanced Circuits, ExpressPCB, Cadsoft, or any other company listed in this review. The suggestions offered are based on my personal experience. Thanks to IVAR/NA for allowing me to use their board design file in this tutorial.

For small projects, I've found it difficult to beat the simplicity of the tools offered by ExpressPCB. They've got a really great integrated PCB and schematic tool that I make use of almost daily, and I highly recommend their $51/3 miniboard service for prototyping. They've got a great tutorial and tips to get you started.

However, you can get better deals on production volumes if you produce a standard gerber file that's compatible with CAM processes at the larger boardhouses. Often, only the larger board houses offer things like UL certified processes and materials, required for products that are safety tested. For these projects, you'll have to use a standard CAD tool.

This tutorial deals with advanced circuits, but there are many other similar board houses you can choose from, convering a wide spectrum of price/quantity/time delivery options.

Some of the larger ones:

tools you'll need:

Cadsoft Eagle

Eagle has gained a wide following and tremendous suppoort from the internet community. Their package offers features on par with competitors that cost ten times as much, and they offer support for their program running on Windows, Linux, and even Mac OSX. Their support forums are great, there's a very large component library, and version available for academic use for free. We'll cover using the 'Light' version in this tutorial.

Software Companion's Gerbview

Gerbview from Software companions is a really nice tool for checking your output files prior to submitting. This can save time later if you accidentally have the top layer output as a mirror image, or with a offset. It's available in a free trial, and if you're doing any number of boards, worth the purchase price.

If you're running linux, there are a couple free gerber utilities out there. I recommend having a look at the Gerber Viewer project. It also has the capability to output your images as a PNG.

preparing your project:

We've assumed you have your project ready to go, checked, and re-checked. Did I mention you should check it again? Make sure that your traces are properly joined to pads and vias in the program, as this will cause problems with the manufacturing check later.

If you're not framiliar with Eagle, check out their great online tour.

prepare your nc drill rack:

The drill file tells the automated drilling tool what size holes and where to drill them. To prepare this file, go to the eagle command window and type 'run drillcfg'. A dialog box will pop up to select units; for North American fab houses, this will almost certainly be in inches. Eagle will then display a list of drill sizes; select OK at this step. If you're using standard options it is unlikely you will have a problem with manufacturability.

After running this command, you'll be greeted by these dialogs:

Once you select OK, you'll be presented with a dialog to save the output NC drill file, a *.drl. This information is used by the cam processor, so put it in your working directory for now. Remember to use inches for the output file.

generate cam files:

To start generating your CAM job, open up the CAM processor.

This is where most of the action takes place. You'll use the pre-existing CAM job templates in eagle to produce the manufacturing instructions for your circuit board design. There's two sets of files you need, the excellon drill files, and the commonly known gerber 274x format files. These are accessed by opening up the job file from within the CAM procesor.

The first step is to generate the excellon drill files. Select "open job", and load the "excellon.cam" file. You'll see the below dialog open up:

Confirm that the options match up with the dialog. Then, select the "process job" button. This will take the drill information you created in the previous step and generate the cam information to properly drill your PCB.

Next, generate the gerber 274x files. As before, open the "gerb274x.cam" file. You'll be presented with a multi-part dialog with tabs along the top. Each tab corresponds to various copper and silkscreen layers in the PCB. For a PCB with more than two layers, you'll have more dialogs to work through. The dialogs for all layers in the example should appear as below:

Once you're happy with the dialog options, select "process job" as before. Eagle will then generate a gerber file representing your circuit board. You only need to click process job on one of the dialogs and the gerber set is generated.

If all went well, you now have a set of manufacturable PCB cam files!

review output files:

Once you've generated all the files using the CAM tool, it's important to make sure that the output files make sense. Gerbview is a good tool for doing a sanity check;

Loading gerbview, we can add in the files from Eagle one by one. Your drill files should line up with the copper layers (pads) on the top and bottom. You can see how your silkscreen will look, too. Consult the table below to see what each of the layers is. A common problem is that one of the layers might appear to be flipped, or presented as it's mirror image. If that's the case, go back to Eagle and make sure that the CAM job is set up correctly. Run the job again and load the file to confirm.

Once you're happy the board file looks more or less the same as it did in eagle, you can be confident it will look correct when presented to the manufacturing design tools.

packaging up files:

The next step is to make a text file up, called README.TXT that contains the filenames of the above files and a description of what they are. This helps the folks behind the scenes put a sanity check on your file before it goes to production.

Sample README.TXT:

test100.brd : eagle project file test100.drd : excellon drill description test100.dri : excellon drill tool description test100.drl : drill rack data test100.gpi : gerber photoplotter information data test100.plc : component side silk screen data test100.sol : solder side data test100.stc : component side solder stop mask data test100.sts : solder side solder stop mask data e-mail : xtal@xdesignlabs.com

You'll need to package up all those files above, including the text file, and make a zip file archive to upload to their servers. Winzip is the easiest way to do this. I'll usually put the eagle board and schematic files inside as well; this steps makes for a good time to milestone your project and burn it to a CD for backup.

submitting your order:

You'll need to register with Advanced Circuits and create a user name. Once this is done, you're able to log into their upload utility and send your file that you've prepared in zip format. Select the "FreeDFM" link and you'll be greeted by a dialog propmting you to select where the file is located.

Before you submit your order, make sure to use their online viewing functionality to confirm what you have sent looks correct after it's been interpreted by their system.

Once you've sent the file, you'll need to explain what the files are and what parameters you want for your board, for example, the dimension of the board in inches, the number of layers on the board, the color of solder mask or silkscreen (if any), etc. You can see an example of these below.

online DFM checking:

Great! Now, the software will come back and email you the results of their online DFM check. This is an automated proceedure to check for common problems that would prevent them from making your circuit board properly.

There are two sets of problems; ones that get flagged as potential show stoppers, or issues that would prevent them from accepting your order as it stands now. The other type is a more minor problem that can be automatically fixed in the software; this is most common with silkscreened fonts having regions that are too thin. They will be automatically repaired.

Show-stoppers should be addressed in the tool. The most common problem is having traces that don't connect properly with their pads, resulting in odd clearance problems. These may or may not affect the final manufacturability of the design. It's good practice to make sure these are lined up correctly.

If you've corrected problems, or the DFM tool has automatically fixed it, now would be a good time to use the on-line "view" tool to look at how their software interpreted or repaired your board. A common problem will be the silkscreen fonts are no longer in the location you think that they should be and is a good idea to watch for.

getting your quote:

Once your order has been placed, you'll have the option to look at a table of manufacturing prices that will look something like the image below. Select the price / order service you like best, and follow though with your order.

final product:

A few days later, you'll recieve your PCB:

that's it!

Wasn't so bad, now, was it? With all the competition for your board turn dollars, there are some really good deals out there. It's questionable if it's worth it to go mucking about with buckets of etchant and resist paper unless you absolutely need a sub 24h turn around on boards.