Updates at the end of the topic: 1.Latest suggestion from Seppo Vesterinen for exporting gerber files with silk screen file on both side of PCB These days, our team is preparing the PCB service for customer. As we all know, there are many PCB layout softwares, such as Altium Designer, OrCAD, KiCad, PowerPCB etc. CadSoft EAGLE PCB design software is one of the best PCB design software available for designing printed circuit board. Also in the Arduino community , there’re lots of open source designs based on Eagle software.Unfortunately, our manufactory can’t support the Eagle design files directly. In this tutorial I will introduce the way to export the Gerber files from your eagle design step by step, helping you to manufacture your design or the open source design from the others you interested in.
DRC usually makes sure that your board doesn’t exceed the manufacturer’s production abilities. So we supply a DRU file for you to run the DRC. Based on the checking result you can modify your design a little bit to avoid some common problems. Of course, if you have a special requirement of your design, you can also ignore some errors from the report.
Start eagle PCB software, load your brd file, then select Tools -> DRC…
Then press load to open the DRU file from DFRobot. Press check to get the report of errors.
Export Gerber files
Gerber files are typically produced by PCB designers using general PCB software. These files are sent to PCB fabricators like us where they are loaded into a CAM system by using CAM350 to prepare data for each step of the PCB production process. In this workflow they transfer the layer information from .PCB/.brd files to CAM. 1. First of all, in the Eagle Board window, select File->CAM Processor. 2. Click File -> Open -> Job...: 3. Select Gerb274x.cam, and click open: 4.Now it's the important, make sure "Mirror" is unchecked on all tabs, then click "Process Job...”. 5. It may take a couple seconds to generate all files, once it is done, close the dialog. Note: The job (gerb274x) of processor will just export Dimension,tPlace and tNames layer in your design. And it also won't export the bottom layer silk screen also. So you need to print the tValues layer and the bottom layer silk screen, you could modify a little bit based on the gerb274x job and save a custom job!
Generate Excellon drill files
The Excellon format is used to exchange drill and rout data between CAD/CAM systems as well as to drive CNC machines. 1.Open the CAM Processor again and Click File -> Open -> Job 2.Select excellon.cam, and click open: 3.Click process Job. Then it will output the drill files instantly. Clicking the 'x' icon on the right corner to close the window.
After all the steps above, the files for product are ready. Just send it to the factory. These are the files:
drd Excellon drill description
dri Excellon drill tool description
cmp Component side data
sol Solder side data
plc Component side silk screen data
stc Component side solder stop mask data
sts Solder side solder stop mask data
gpi Gerber photoplotter information data
Check the Gerber files
If you’d like to check your Gerber files generated, you can use the CAM350 which is used by the factory to review your design again. It’s very simple. 1.Open CAM350, then Click File -> Import -> AutoImport... 2. Open your design files folder and click the Next>> to read the gerber files: 3. Click finished, then it’ll take a short time to auto import files. 4. Now you can check all the layers supplied to the factory for your design .
A easy way to generate the manufacturing files with soldering side silk screen as follows:
1) Run gerb274x.cam and excellon.cam jobs in EAGLE CAM processor according to the instructions by DFRobot 2) Open the CAM processor with gerb274x-4layer.cam and run just the "Process Section" for the Soldering Side Slik Screen layer to generate the missing *.pls file 3) Put all the generated manufacturing files into a zip-file