http://opalkelly.com/

Author Topic: Exporting working GERBER files from Eagle the easy way  (Read 3454 times)

0 Members and 1 Guest are viewing this topic.

Offline Chumanista

  • Contributor
  • Posts: 37
Exporting working GERBER files from Eagle the easy way
« on: July 26, 2016, 06:20:46 AM »
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.
 

Offline wasyoungonce

  • Regular Contributor
  • *
  • Posts: 168
  • Country: au
Re: Exporting working GERBER files from Eagle the easy way
« Reply #1 on: July 31, 2016, 11:44:14 PM »
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 thanks

Brendan
I'd forget my Head if it wasn't screwed on!
 

Offline jgarc063

  • Regular Contributor
  • *
  • Posts: 69
  • Country: us
Re: Exporting working GERBER files from Eagle the easy way
« Reply #2 on: August 02, 2016, 04:04:59 AM »
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.

Hi 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 Garcia
Cadsoft Support
 

Offline zapta

  • Super Contributor
  • ***
  • Posts: 6009
  • Country: us
Re: Exporting working GERBER files from Eagle the easy way
« Reply #3 on: August 02, 2016, 08:34:35 AM »
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
Drain the swamp.
 

Offline wasyoungonce

  • Regular Contributor
  • *
  • Posts: 168
  • Country: au
Re: Exporting working GERBER files from Eagle the easy way
« Reply #4 on: August 02, 2016, 10:41:25 AM »
Hi Jorge

yep you are correct

editing 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 thanks

Many thanks Zapta...didn't know of this and was going to Elecrow.


Brendan
I'd forget my Head if it wasn't screwed on!
 

Offline LukeW

  • Frequent Contributor
  • **
  • Posts: 567
Re: Exporting working GERBER files from Eagle the easy way
« Reply #5 on: August 03, 2016, 04:56:39 PM »
Here's the makefile that I personally like to use (well an old version of it)

https://github.com/lukeweston/eagle-makefile/blob/master/makefile

Hit 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.
 

Offline wasyoungonce

  • Regular Contributor
  • *
  • Posts: 168
  • Country: au
Re: Exporting working GERBER files from Eagle the easy way
« Reply #6 on: August 04, 2016, 11:22:33 AM »
Thanks Luke...I'll give it a go when I get home...in a day of so

I'd forget my Head if it wasn't screwed on!
 

Offline technotronix

  • Regular Contributor
  • *
  • Posts: 209
  • Country: us
    • PCB Assembly
Re: Exporting working GERBER files from Eagle the easy way
« Reply #7 on: August 06, 2016, 10:27:10 PM »
Here are a step which I use when creating gerber file from eagle.

Go or open CAM processor
open job
process the job
add file for drill holes
check out final files
 

Offline zapta

  • Super Contributor
  • ***
  • Posts: 6009
  • Country: us
Re: Exporting working GERBER files from Eagle the easy way
« Reply #8 on: August 07, 2016, 01:27:26 AM »
Here are a step which I use when creating gerber file from eagle.

Go or open CAM processor
open job
process the job
add file for drill holes
check out final files
... And then zip them. I wish eagle and the free Gerber viewing rules would work directly with zip files.
Drain the swamp.
 

Offline wasyoungonce

  • Regular Contributor
  • *
  • Posts: 168
  • Country: au
Re: Exporting working GERBER files from Eagle the easy way
« Reply #9 on: August 07, 2016, 09:52:58 AM »
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
I'd forget my Head if it wasn't screwed on!
 

Offline Josephine85

  • Contributor
  • Posts: 32
Re: Exporting working GERBER files from Eagle the easy way
« Reply #10 on: August 19, 2016, 09:40:13 PM »
Wow thanks, that´s very nice :)
 

Offline Erin.KOU

  • Contributor
  • Posts: 8
  • Country: cn
  • ALLPCB, Sales manager, [email protected]
    • ALLPCB
Re: Exporting working GERBER files from Eagle the easy way
« Reply #11 on: November 07, 2016, 12:01:53 AM »
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-X 
 2. exporting Drill files -excellon.cam
 
There 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 , .sol
 Soldermask layers - . stc, .sts
 Silkscreen layers - .plc, .pls
 Drill layers - .txt
 Outline layer - .dim
 If you want to make stencil, then also need included stencil files , that is - .crc, .crs

Hope this information can be helpful.
Free Expedite for PCB Prototype in 24-48H with min $5 ;Register to get $5 Cash Credit
FR-4 (KB-6160 Grade A)& Taiyo Ink
-site: www.allpcb.com/G4
 

Offline technotronix

  • Regular Contributor
  • *
  • Posts: 209
  • Country: us
    • PCB Assembly
Re: Exporting working GERBER files from Eagle the easy way
« Reply #12 on: December 30, 2016, 06:56:45 PM »
Thanks for sharing the video.
 

Offline richardlawson1489

  • Regular Contributor
  • *
  • Posts: 125
  • Country: us
    • PCB Assembly
Re: Exporting working GERBER files from Eagle the easy way
« Reply #13 on: February 01, 2017, 06:36:15 PM »
Will it allow me to export gerbers to a child folder?
 

Offline jgarc063

  • Regular Contributor
  • *
  • Posts: 69
  • Country: us
Re: Exporting working GERBER files from Eagle the easy way
« Reply #14 on: February 02, 2017, 04:02:35 AM »
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 Garcia
Autodesk Support
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf