# Can you load Gerber files back into a PCB layout designer such as Eagle?

There's a PCB I may need to change a solder pad, but the schematic and layout are gone and were not added to source control. Is it possible to load the Gerber files back into a designer to change the pads so that I don't have to try to draw out the entire schematic and layout again?

• Were the Gerbers originally created from an Eagle design? – DerStrom8 May 12 '16 at 17:15
• I'm told that is correct. But I'm also told that with enough hesitation that I couldn't say that with certainty. Does that matter, though? I thought Gerbers were Gerbers were Gerbers. – D4ILYD0SE May 12 '16 at 17:18
• Some Gerber viewers support editing. Risky business though, IMO. – Matt Young May 12 '16 at 17:27
• @JeffHawkins no other distributor offers smaller order quantities ? – efox29 May 12 '16 at 19:50
• You can do this in KiCad. It's definitely not optimal. – pipe May 12 '16 at 21:43

As of Eagle 7.5, this is indeed possible. It's a simple case of File->Import->Gerber from the layout editor. There is a video demo on YouTube.

As others have mentioned, there is no real DRC checking possible of the imported file as the Gerbers contain no information on nets and connectivity. Eagle simply imports all of the various shapes and lines onto the copper layer.

It does however allow you to make modifications manually (with great care) and then re-export as a Gerber again once you are done.

No. A standard Gerber format file contains only primitive shapes and positions. It contains no concept of WHAT any of the shapes represent, or even that it is an electronic printed-circuit board.

However, the Gerber format is a quite simple and strightforward text file. It can be edited in any low-level text editor. So, if it is worth the time and effort, you COULD "tweak" the contents of the Gerber files to make a change as simple as modifying a pad.

• I did not know this. But that would seem a little tricky. Is it just kind of like an XML format sort of thing where it says "Filled at (x,y) coordinate at length width (i,j)? I guess I could go look at it right now. – D4ILYD0SE May 12 '16 at 20:31
• @JeffHawkins Even lower level than that, actually. Gerber files are essentially a list of instructions to be executed by a plotter. – duskwuff -inactive- May 12 '16 at 20:41

Essentially, the Gerbers are vector drawings (that PCB fab equipment understands). In a Gerber, you can have a rectangle, but the Gerber doesn't "know" that this rectangle is actually a pad, and it's a part of footprint that has other pads. Gerbers don't carry the schematic information: all traces are just lines (or polylines) for x1,y1 to x2,y2.

Afaik, Gerbers can't be loaded back into Eagle PCB layout designer. When Gerbers are generated from an Eagle layout (from the BRD file), a lot of information is left out from the Gerbers.

There are Gerber Viewer and Gerber Editor programs, which allow to edit Gerber files. They work independent of the software from which a Gerber was generated. They provide a lot less DRC (if any), because a Gerber Editor doesn't "know" the schematic. (@Matt had already mentioned that manual editing of Gerbers is risky.) You would have to compensate for this lack of DRC with additional human diligence.

• I concur. What many softwares do allow however (unsure about Eagle) is importing graphics as silk. If you can separate the gerber into layers, save each as an image, import them as silkscreens, then you can re-do each trace overtop the silkscreens for a "guide." In KiCAD it may be possible to then back-annotate PCB to a schematic, but it will not be easy and as Nick states, DRC will be a pain. -1 to whomever lost the source control! – rdtsc May 12 '16 at 17:55
• In Eagle V7.5 and newer, Gerbers can be imported to the layout editor as objects on the copper layer. There is no schematic recreated, but it is possible to then edit the copper layout and then re-export. – Tom Carpenter May 12 '16 at 21:22

Eagle paints many of the gerber features with a raster of 0.3mm lines, making it difficult to seamlessly identify features such as pads or tracks, versus polygonal pours, ground planes and so forth.

If your version of Eagle supports import, you are mostly done and dusted. If not, other options would include converting to another file format which you may be able to import into eagle, i.e. the following utility can create a gEDA PCB compatible footprint with a gerber file, but has to make guesses about which polygons are pads versus ground pours, and like any gerber->layout conversion tool, will not be 100% reliable in reproducing all of the features.

https://github.com/erichVK5/translate2geda

(disclaimer: my WIP conversion tool)