Eagle drillfile/gerber creation - diyAudio
Go Back   Home > Forums > Design & Build > Parts

Parts Where to get, and how to make the best bits. PCB's, caps, transformers, etc.

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 26th November 2008, 11:27 AM   #1
diyAudio Member
 
Join Date: Sep 2008
Default Eagle drillfile/gerber creation

Hi, I hope somebody will help me out here.

When creating drillfile and gerbers from Eagle, which (if any) gerbers should be mirrored/rotated?

I read in another post in this forum "Beware of CAM mirroring" but without any further explanation. A few days of searching the Internet has not revealed how to do this. The Eagle documentation just says run gerb274x.cam, and nothing more.

If I use gerb274x.cam in Eagle, the solder side gerbers are mirrored by default, causing complete misalignment when viewed in gerbv.

Gerbv won't display .drd-files correctly, so I have no idea if it should be mirrored or not.

I messed around with these settings until they aligned correctly in gerbv, and sent them off for production. The copper was the wrong way (what should be inwards to the board was outwards), and my silkscreen ended up on the copper side. Understandably I don't like this to happen again, so I'm hoping you will are kind enough to help me get it right.

Thank you very much.

-skrodahl
  Reply With Quote
Old 26th November 2008, 04:23 PM   #2
BWRX is offline BWRX  United States
diyAudio Moderator Emeritus
 
Join Date: Jan 2005
Location: Pennsylvania
Even if the layers are mirrored any reasonably competent board house will see that and can mirror them using whatever software they use to view the gerber files. Even so, I'll post more on how to do it correctly when I get home from work.
__________________
Brian
  Reply With Quote
Old 26th November 2008, 10:32 PM   #3
BWRX is offline BWRX  United States
diyAudio Moderator Emeritus
 
Join Date: Jan 2005
Location: Pennsylvania
After opening the gerb274x.cam file, click the in the CAM processor window click the solder side tab and just uncheck the box next to mirror. Do the same for the solder stop mask tab. Process the job and then view the results in your gerber file viewer. The layers should line up that way. They were the last time I did that and checked them in gerbtool (part of the orcad toolsuite).
__________________
Brian
  Reply With Quote
Old 27th November 2008, 01:08 PM   #4
diyAudio Member
 
Join Date: Sep 2008
Quote:
Originally posted by BWRX
After opening the gerb274x.cam file, click the in the CAM processor window click the solder side tab and just uncheck the box next to mirror. Do the same for the solder stop mask tab. Process the job and then view the results in your gerber file viewer. The layers should line up that way. They were the last time I did that and checked them in gerbtool (part of the orcad toolsuite).
Thanks for the replies I've gotten so far.

Just to make sure I'm reading this reply correctly:
Are you saying that none of the gerbers should be mirrored?

-skrodahl
  Reply With Quote
Old 2nd December 2008, 08:20 PM   #5
marce is offline marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
Hi Skrodahl,
None of the gerbers should be mirrored.
Generaly the standard convention for providing gerbers is:-
Viewed from the top layer, usualy as they are designed on the ECAD system.
Preferably alligned, if not some reference points on each layer to allow easy allignment by the fabricator.
Instructions , minimum indicating the stack up, ie which gerber layer is the top, which is the bottom layer (for multilayer the inner layers stack up info). Required copper weight. Surface finish etc. The more info you supply the less guess work involved when the gerbers are put through the front end system.
RS-274X for gerbers and Excellon II for drill data. (Excellon II is the drilling equivilent of RS-274x, it has an emebdded drill table at the begining of the file, cuts out translating drill table errors.)

One of the reasons for not mirroring is that when the actual photo tools are created from the gerbers, they are created so that the emulsion layer (the actual image) is always face down to the copper, this avoids the image expanding as it passes through the film. Not so critical with wider tracks and gaps but every little helps. And most fabrication houses will be geared up to process data this way so it makes thier job easier and helps reduce errors.
Hope this helps.
Marc
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
Eagle: Mirror bottom layer for Gerber files? orthoefer Everything Else 4 17th August 2006 01:38 AM
Question about Eagle and Gerber-files... CJ900RR Everything Else 2 9th August 2006 01:08 AM
Eagle & Gerber metal Parts 11 15th November 2005 11:09 AM
My first creation Simpleton Tubes / Valves 15 3rd September 2005 03:24 AM


New To Site? Need Help?

All times are GMT. The time now is 09:47 AM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2