ECE101 – Basic Electrical and Computer Engineering

Creating Gerber Files in EAGLE

In this post, I’ll be using the gerber viewer found here (just download the latest version of the executable), and the information here is based on our use of PCBFabExpress. For this post, I feel like the video is much clearer in explaining the CAM Processor, as the actual text becomes very wordy in trying to describe the steps you need to take to produce your gerbers.

Gerber Files – What are they?

Gerber files contain information that board houses use to control their machinery to manufacture PCBs. With so many different layout programs, gerbers act as a bridge between designer and manufacturer. The most common format in use today is RS-274-X, but you should check with the board manufacturer that you’ll be using to ensure that you use the right format in your boards.

Using the CAM Processor

To create gerbers in EAGLE open your finished board, then click File -> CAM Processor. In the CAM Processor window, you’ll need to create one section for each gerber file that needs to be created. For a two layer board with silk screen and solder mask on both sides, you’ll create seven sections. The section name and prompt have no effect on the output, so put a descriptive name in the section box. The checkboxes in Style should be correct (pos. coord, optimize, and fill pads should be checked), and both the x and y offsets should be set to zero.

The table below shows what device, file extension, and layers need to be selected for each section. To make the file name dynamic, I use the variables that you can look up in EAGLE’s help. Specifically, I use %P to get the path of the board and %N to get the name (without the extension) of the board. So, in my file section, I entered %P\Gerbers\%N.extension, where extension is the extension for the particular section. This lets me use the same processor job for any board I need gerbers for, and all I need to do is create the gerbers directory.

To create the first section, enter CMP in the section name, %P\Gerbers\%N.cmp for the file, select GERBER_RS274X as the device, and select Top, Pads, and Vias in the layer box. Click Add, and it will duplicate this section. Repeat the process until you’ve created all the sections in the table above. Once you’ve created all of the sections, click process job (make sure you’ve created the Gerbers folder in the same directory as your board file) and EAGLE will create all the gerber files you need.

Viewing the Gerbers

Once you’ve created your gerbers, you should always use a gerber viewer to ensure they were processed correctly. An error in version 5.1.0 caused some errors in this particular board that, if we hadn’t checked, would have made our boards unusable if they had been manufactured with those errors. If you’ve installed the gerber viewer I linked at the beginning of this post, open it up, click on the folder icon, navigate to your gerber files, select them all and click open. This will show you what the board house is going to see when they manufacture your PCBs. If everything looks correct, zip your files up and send them to your board house to be manufactured.

One important thing to note (and another reason to check your files) is that all text will be converted to a vector format. If your text is in any other format, it may be stretched or skewed. If you use vector based text, your text should look the same in your gerbers as it does on your board.

Now that we’ve covered the basics from start to finish, I’ll spend the next few posts going into more detail on a few things I’ve touched on in the past. As always, contact me with any questions or suggestions.