EEVblog Electronics Community Forum
Electronics => PCB/EDA/CAD => Eagle => Topic started by: Chumanista on July 25, 2016, 08:20:46 pm
-
Hello!
I made a video on how to export GERBERs from Eagle and it takes (with checking them) less than 2 minutes:
https://www.youtube.com/watch?v=oXWwHbusicM (https://www.youtube.com/watch?v=oXWwHbusicM)
I created it because I couldn't find anything useful online, hope it helps somebody.
-
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
-
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
-
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 (http://www.elecrow.com/wiki/index.php?title=How_to_export_gerber_files_from_eagle_file)
-
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
-
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.
-
Thanks Luke...I'll give it a go when I get home...in a day of so
-
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
-
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.
-
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
-
Wow thanks, that´s very nice :)
-
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/ (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.
-
Thanks for sharing the video.
-
Will it allow me to export gerbers to a child folder?
-
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