Summary： In this post we will see how to generate the necessary files to have our prototypes manufactured with a professional finish, usually printed circuit manufacturers require the GERBER file generated in RS274X format, for each layer that makes up our design.
Note: For eagle the latest version 9.6.2, please click How to Generate Gerber and Drill Files From Eagle 9.6.2
In this post we will see how to generate the necessary files to have our prototypes manufactured with a professional finish, usually printed circuit manufacturers require the GERBER file generated in RS274X format, for each layer that makes up our design. It is important to mention that to carry out these steps the design must have been previously verified.
These are the files PCB Way needs:
Now we will detail each of the previous files to know which layers we should activate, so we will start by configuring the CAM Processor, as follows.
Select the CAM Processor icon or File >> CAM Processor menu.
In Device we must select GERBER_RS274X.
In File we select the place where we want to save the files, I regularly create a folder called GERBER within my project folder. We put the name and extension of the layer that we want to create. To place the same file name we put the following (selected path)% N. (Layer extension).
Well the result should be the following:
It is important to say that we will do this process for all the desired faces, the only thing that will change will be the file extension, I must also say that this post is designed in a two-sided design, it goes without saying that if your design does not use all of them, you must omit the files not needed.
TOP Copper layer(.cmp). We must activate in Layer: Top, Pads, Vias and Dimension.
To add the next layer, we just have to click Add.
BOTTOM copper layer(.sol). We must activate in Layer: Bottom, Pads, Vias and Dimension.
Silk screen layer of TOP components(.plc). We must activate in Layer: tPlace, tName and Dimension.
Silk screen layer of BOTTOM components(.pls). We must activate in Layer: bPlace, bName, and Dimension.
Solder mask layer of TOP components(.stc). We must activate in Layer: tStop.
Solder mask layer of BOTTOM components(.sts). We must activate in Layer: bStop.
Layer of internal cuts, milled(.gko). We must activate in Layer: Milling and Dimension.
Perforation layer(.ncd). We must activate in Layer: Drills and Holes. Here it must be changed in Device GERBER_RS274x by EXCELLON
When you have all the layers (of course those that do not apply in your design, they must be omitted), to start the process we must click on Process Job.
After this, it will begin to run layer by layer until it is finished, when it finishes we simply close the window, if it asks you if you want to save it you can do it in the same folder of the project. In the end depending on the layers used we will have something more or less like this:
Drilling configuration file(.drl). To do this we execute the ULP: drillcfg.ulp, whether we use the ULP icon or in the File >> Run ULP, after selecting it we simply open.
Then we select "inch" and we give OK.
A list of the sizes that we have in our design will appear, we simply click OK.
Finally we select the path where we want to save it, it is important that it be saved together with the other files created.
Well now we have all the files ready, the next thing is to add the GERBERs in a .ZIP or .RAR file to load them in PCB Way. Here is a screenshot of what my project folder looks like:
In yellow the .RAR file, in blue the folder where all the GERBERs are saved, in orange the CAM file that we generated in the previous steps, this file can be used for other projects as a master file and only add or delete layers that are not used. To use it, just open the CAM Processor then in File >> Open >> Job ... and look for the path where we have saved the file.
To visualize and corroborate that everything coming out with the GERBERs you can use viewMate or Gerbv, well I hope that these steps have been ulutrative so that you can generate your GERBERs without problems.
