Exporting working GERBER files from Eagle the easy way - Page 1
Forum section: electronics / general

author: Chumanista
author_rank: Contributor
timestamp: July 25, 2016, 08:20:46 pm
content: Hello!I made a video on how to export GERBERs from Eagle and it takes (with checking them) less than 2 minutes:I created it because I couldn't find anything useful online, hope it helps somebody.

author: wasyoungonce
author_rank: Frequent Contributor
timestamp: July 31, 2016, 01:44:14 pm
content: Many thanks...tried your cam generator...works a treat but had errors "could not read" the plotter Gerber "gpi" and drill station gerber "dri" with Gerbv. Not really an issue, no one uses plotter anymore or drill station.I also had errors with drill file "txt" using Excillion output. In fact the drill file was corrupt..no drills at all! I needed to change this to Excellion24 to get a valid "txt" drill file. Worked ok with this. I think its an Eagle issue!Many thanksBrendan

author: jgarc063
author_rank: Regular Contributor
timestamp: August 01, 2016, 06:04:59 pm
content: Quote from: wasyoungonce on July 31, 2016, 01:44:14 pmHi Brendan,That sound like the problem right there, EAGLE doesn't have Excillion output.All joking aside, the default EXCELLON cam job uses 2.5 precision as the default. All gerber viewers take a guess at the format of an excellon file when they receive it. Sometimes they guess wrong(this is especially true if the board is small). By switching to excellon24 you used a lower precision which apparently gerbv was able to guess correctly.In the future, you can use the default excellon cam job driver. If you don't get the result you expect then you can tell gerbv the format of the excellon file explicitly. Here's the format we use.5 place after the decimal(might be listed as 1.5 or 2.5) leading zeroes suppressed absolute inches.So as you can see, it's not an EAGLE issue just a limitation of the guessing algortihm in gerber viewers.hth,Jorge GarciaCadsoft Support

author: zapta
author_rank: Super Contributor
timestamp: August 01, 2016, 10:34:35 pm
content: Good to see Cadsoft support here. ;-)As for cam files, some PCB vendors provide files that match their processes. For example, I am using this for elecrow orders:http://www.elecrow.com/wiki/index.php?title=How_to_export_gerber_files_from_eagle_file

author: wasyoungonce
author_rank: Frequent Contributor
timestamp: August 02, 2016, 12:41:25 am
content: Hi Jorgeyep you are correctediting the drill file format in Gerbv to 5 decimal ...fixed the issue. I saw that the drills were ~10x larger than the board...now they are where they should be. many thanksMany thanks Zapta...didn't know of this and was going to Elecrow.Brendan

author: LukeW
author_rank: Frequent Contributor
timestamp: August 03, 2016, 06:56:39 am
content: Here's the makefile that I personally like to use (well an old version of it)https://github.com/lukeweston/eagle-makefile/blob/master/makefileHit make, and you get the Gerber zip file, fab-ready in an instant.You can invoke gerbv to make a preview picture if you like.Sometimes it needs to be edited slightly from one job to the next (because e.g. sometimes I like tValues included on the silkscreen and sometimes not) but that's pretty fast.Rip out all the gerbv stuff, and the gitHub stuff, to your taste if you don't like it.

author: wasyoungonce
author_rank: Frequent Contributor
timestamp: August 04, 2016, 01:22:33 am
content: Thanks Luke...I'll give it a go when I get home...in a day of so

author: technotronix
author_rank: Regular Contributor
timestamp: August 06, 2016, 12:27:10 pm
content: Here are a step which I use when creating gerber file from eagle.Go or open CAM processoropen jobprocess the jobadd file for drill holescheck out final files

author: zapta
author_rank: Super Contributor
timestamp: August 06, 2016, 03:27:26 pm
content: Quote from: technotronix on August 06, 2016, 12:27:10 pm... And then zip them. I wish eagle and the free Gerber viewing rules would work directly with zip files.

author: wasyoungonce
author_rank: Frequent Contributor
timestamp: August 06, 2016, 11:52:58 pm
content: Thanks Gents. I'm trying all methods....it was just the drill file. The holes coordinates were 10 times bigger than the other gerber coordinates, this is a common issue...according to Mr Google. Its to do with the Gerber viewer (Gerbv) coordinate accuracy and the accuracy of the generated drill file. This is sorted now but I am exploring all other ways of generating Gerbers. I also noted the drill file does not include the "Milling layer". Which incidently was fine.Many thanks

author: Josephine85
author_rank: Contributor
timestamp: August 19, 2016, 11:40:13 am
content: Wow thanks, that´s very nice

author: Erin.KOU
author_rank: Newbie
timestamp: November 06, 2016, 01:01:53 pm
content: Most PCB fabs require to send the Gerber files.When exporting Gerber files, it is really quite easy.Also I share a way to exporting the Gerber files from Eagle.It should including 2 steps -1. exporting Gerber files - choose RS274-X2. exporting Drill files -excellon.camThere is a share in - it shows the steps to genrate Gerber files from Eagle with PICs. which may be easier to understanding.Refer link:http://www.instructables.com/id/Generate-Gerber-Files-From-EAGLE-File/And also it is important to generate the full complete Gerber files.that should include:Copper layers - .cmp , .solSoldermask layers - . stc, .stsSilkscreen layers - .plc, .plsDrill layers - .txtOutline layer - .dimIf you want to make stencil, then also need included stencil files , that is - .crc, .crsHope this information can be helpful.

author: technotronix
author_rank: Regular Contributor
timestamp: December 30, 2016, 07:56:45 am
content: Thanks for sharing the video.

author: richardlawson1489
author_rank: Regular Contributor
timestamp: February 01, 2017, 07:36:15 am
content: Will it allow me to export gerbers to a child folder?

author: jgarc063
author_rank: Regular Contributor
timestamp: February 01, 2017, 05:02:35 pm
content: Hi richardlawson1489,Yes it will. You just have to use the appropriate variables. See Chp 9 of the EAGLE manual to see the different file variables available. Keep in mind that whatever folder you want the gerbers to go to has to exist BEFORE you run the CAM job. EAGLE won't create the folder if it doesn't exist.Best Regards,Jorge GarciaAutodesk Support