Actions
Forum Thread Details
  • State Verified Answer
  • Replies 3 replies
  • Subscribers 178 subscribers
  • Views 1367 views
  • Users 0 members are here
Related

Drill CAM export problem

Former Member

Hi,

 

I've recently upgraded to Eagle 7.6.0 and I'm now having serious issues with exporting Drill data via the CAM processor.

The exported Excellon file does not match the .brd file at all - it's completely different.

I'm using an Eagle file that was exporting successfully in previous versions and a CAM job file that I've used for years.

This problem seems to have started with the upgrade to v7.6.0 and seems to affect all my Eagle files.

The pic below shows what I'm seeing in the Gerber Viewer. You can see the actual board in the bottom right hand corner but something has added all these extra drill files outside the board area!

Can anyone help with this?

 

image

  • 0

    On 7/25/2016 1:54 PM, Justin Owen wrote:

    Hi,

     

    I've recently upgraded to Eagle 7.6.0 and I'm now having serious issues with exporting Drill data via the CAM processor.

    The exported Excellon file does not match the .brd file at all - it's completely different.

    I'm using an Eagle file that was exporting successfully in previous versions and a CAM job file that I've used for years.

    This problem seems to have started with the upgrade to v7.6.0 and seems to affect all my Eagle files.

    The pic below shows what I'm seeing in the Gerber Viewer. You can see the actual board in the bottom right hand corner but something has added all these extra drill files outside the board area!

    Can anyone help with this?

     

     

    --

    To view any images and attachments in this post, visit:

    https://www.element14.com/community/message/202252

     

     

    Hi Justin,

     

    I hope you're doing well. They are not extra holes, they are the actual

    holes of your design. The gerber viewer incorrectly guessed the format

    of the excellon file.

     

    Newer versions of EAGLE have more precision in the CAM output by

    default. On small boards or those with few features the gerber viewers

    can sometimes guess the format incorrectly.

     

    Just specify the format of the excellon file and it will be good. Here's

    the format

     

    2.5 (1.5 is same) leading zeroes suppressed absolute inches

     

    hth,

    Jorge Garcia

     

  • 0

    I have seen this with earlier versions too. In my case it was just incorrect units and gerbv wasn't correctly detecting the unit and scaling accordingly. I think you can adjust it to tell it what the actual units are. I remember playing around this a while back and resolving the issue but I can't remember what I needed to change from/to.

     

    Best Regards,


    Rachael

  • 0

    Thanks all.

     

    Changing from EXCELLON to EXCELLON_24 seems to have solved the issue.

     

    Does seem like there is some sort of resolution/scaling difference between versions/output methods - I can see now that my original output wasn't "completely different" but just a scaled up version of the main/biggest holes on the board.

     

    Solved - thanks, much appreciated.

     

    / J