[dsavitsk]

I am trying to go from Eagle files to boards, which of course involves gerber files. I have followed the directions at http://www.interq.or.jp/japan/se-inoue/e_eagle44.htm as well as those in the eagle tutorial, but I am not sure what to do with all of the files.

I have tried to look at the gerbers in a viewer (both gc-preview as well as Viewmate) but I get tons of errors from both and different layers don't seem to line up. The hope is to panelize several boards (using GerbMerge http://claymore.engineer.gvsu.edu/%7...rge/index.html) so getting a good look at the gerbers sems important.

Can anyone give some tips about how to view gerbers from eagle successfully, or any thing else I should know? Basically, I am stuck and need a push in the right direction.

-d

 

[tangent]

Quote:

Originally Posted by dsavitsk I am not sure what to do with all of the files.

Generally, you zip them up along with a readme file and send that package off to your board house. The readme file tells the technicians at the board house what each file contains: there are no standards for the file name extensions, so you have to tell them that, for example, *.plc is the top-level silkscreen layer. The readme may also have other information, like manufacturing requirements, but the exact contents depend on the board house's needs.

Quote:

I get tons of errors from both and different layers don't seem to line up.

There are several different EAGLE CAM processors, each of which produces somewhat different Gerber files. Are you sure you're using the right one? Check the manual -- there were changes to this as recently as v4.1.

The most common reason for layers not lining up is due to mirror image problems. You can correct this sort of thing in the CAM processor.

 

[dsavitsk]

Quote:

Originally Posted by tangent The readme may also have other information, like manufacturing requirements, but the exact contents depend on the board house's needs.

I imagine I am not the first to find this process a little odd.

Quote:

Originally Posted by tangent There are several different EAGLE CAM processors, each of which produces somewhat different Gerber files. Are you sure you're using the right one?

I used gerb274x.cam

Quote:

Originally Posted by tangent The most common reason for layers not lining up is due to mirror image problems. You can correct this sort of thing in the CAM processor.

There are two layers that are mirrored. If I un-mirror them in the CAM processor then gc-preview seems to get things right. Is there a reason for the mirrored nature? Is it a mistake, or do some board houses want data this way? Is it okay to un-mirror them?

Also, gc-preview throws errors on the dri and gpi files, and does not know what to do with the drl file. Or, at least, I don't know how to get it to use these files. Are some of them safely left out? That is, of the files I have produced (drl, drd, dri, cmp, plc, sol, stc, gpi, sts) which will I generally need to send to off, at least in people's experience?

-d

 

[tangent]

Quote:

Originally Posted by dsavitsk I imagine I am not the first to find this process a little odd.

Look at it this way: it's your second chance to make sure the manufacturing technician gets your order right. Aside from rarities like ExpressPCB, this process isn't 100% automated. There's room for human error, so the more times you tell them exactly what you want, the more likely you'll get what you want.

Quote:

If I un-mirror them in the CAM processor then gc-preview seems to get things right. Is there a reason for the mirrored nature? Is it a mistake, or do some board houses want data this way? Is it okay to un-mirror them?

In my experience, if GC Prevue shows the right data, it gets manufactured correctly.

Quote:

Also, gc-preview throws errors on the dri and gpi files, and does not know what to do with the drl file.

The .dpi and .gpi files are neither Gerber nor Excellon format -- they're just text files, for the layout engineer's benefit. (That's you.) You don't feed these to GC Prevue, and you don't send them to the board house.

The .drd file is Excellon CAM data, which the board house needs. As of EAGLE 4.1, GC Prevue should cope with it correctly. (EAGLE 4.0 used a nonstandard Excellon format.)

You shouldn't have .drl files as of EAGLE 4.1. This is part of the nonstandard Excellon issue. As I recall, it's created by drillcfg.ulp, which was needed in 4.0. If there is no .drl file, the Excellon CAM processor writes out standard Excellon data, but if it is there, it goes back to the old behavior. You should remove this file and stop using drillcfg.ulp. See the EAGLE 4.1 release notes for more about this; it's been many months since I last had to look at this, so I may be getting some of this wrong.

 

[Pars]

Don't mean to threadcrap, but Tangent, do you have a recommended Gerber viewer for Mac OS-X?

Thanks for the good info so far... generating Gerber files is not intuitive at all.

 

[tangent]

Quote:

Originally Posted by Pars do you have a recommended Gerber viewer for Mac OS-X?

Being an old Linux hand, I still use gerbv, part of the gEDA suite. Unfortunately, the easiest way to get this working on OS X is to use these Fink packages. (Ideally, there should be someone offering binary packages, or gEDA should build out of the box, but alas...)

Bonus once you get gerbv working: now you have gschem, too, the best free tool for creating beautiful human-readable schematics.