Gerbers to Footprint!

Foreword

This post is excellent for those who are looking to extract reference designs (in Gerber files) from silicon manufacturers. In this example, I am trying to save myself from having to draw a PCB trace antenna from scratch! We will copy the reference antenna design from Dialog Semiconductors for its DA14580 BLE chips and use that as a footprint for my PCB.

Let me show you how to extract a component footprint from the Gerber files,

Tools

Gerber Files

In this example, I downloaded the reference PCB trace antenna design from Dialog and extracted the Gerber files which were in ART format. These are the “blueprints”, if you will, to a PCB manufacturer in terms of how each layer of the PCB is supposed to look.

PCB Design Software

We will be using Altium Designer 13.1 PCB Design software for this tutorial.

Reverse Engineering the Gerber Files

Import Gerber and Drill Files

First, we have to import the Gerber files into Altium Designer. Create a new CAMtastic document by clicking File>New>CAM Document. Next, initiate the import process by clicking File>Import>Gerber.

Select the desired Gerber files (i.e. layers of interest) into the CAMtastic document.

TIP: Click on “Settings…”.

TIP: Follow the above settings.

It is important that you follow the recommended settings during the import. This will guarantee that the dimensions are correct (in my first few attempts, they were several times larger). Now click “OK” to execute the import.

The imported Gerber files. Highlighted here is just the Top layer which I am interested in.

The import process is not complete yet without the Drill file(s). Initiate it by clicking File>Import>Drill. Follow the same import settings as with the Gerber files. TIP: If we don’t import the Drill files, we won’t be able to extract the netlist(s) later on to export to PCB.

Select the Drill file(s) to load into the CAMtastic document.

TIP: Select the appropriate import settings.

Providing Information about the Layers

To extract the netlists, we need to first associate and establish the layer sets (for eg. the drill layer and top and bottom layers). Click on Tables>Layers Sets. You need at least ONE layers set to move on. You should also set the Layers Order by clicking Tables>Layers Order, otherwise, you will encounter an error when trying to export to PCB.

Insert a layer set by associating the drill layer(s) with the signal/plane layer(s).

Extract the Netlists

We need to now extract the net(s) by clicking on Tools>Netlist>Extract. Now, the traces are identified with a net as they were during the PCB design process.

TIP: Ensure the netlist(s) are extracted from the Gerber files. You can export it to a PCB document.

Export to PCB Document

To generate the PCB document, click on File>Export>Export to PCB (previously grayed out if the preceding steps are not performed). You will now see all the Gerber files being converted into the PCB document.

TIP: Select the desired trace(s) that you want to copy as a footprint.

Copy as Footprint

After you have selected the trace(s) that you wish to copy, paste them in the Footprint PCB Library and create a new component for it.

Now you’re ready to rock and roll with your new footprint reference design!

Summary

We have gone through a step-by-step analysis on how to import the reference design in Gerber files, extract the necessary layer and netlist information, convert them into the PCB document and thereafter be able to reuse it as a component footprint! Perhaps, if you had tried to draw this from scratch, you would have taken a full day to do just that.

I hope that you found my example useful and hope it will come in handy for any advanced users out there. Thanks for reading!

References

1. https://techdocs.altium.com/display/ADOH/CAM+Editor+Reverse+Engineering+PCBs
2. https://techdocs.altium.com/display/ADOH/CAM+Editor+Panels+for+Fabrication+and+Assembly
3. http://techdocs.altium.com/display/ADOH/CAM+Editor+Data+Verification