element14 Community
element14 Community
    Register Log In
  • Site
  • Search
  • Log In Register
  • Members
    Members
    • Achievement Levels
    • Benefits of Membership
    • Feedback and Support
    • Members Area
    • Personal Blogs
    • What's New on element14
  • Learn
    Learn
    • eBooks
    • Learning Center
    • Learning Groups
    • STEM Academy
    • Webinars, Training and Events
  • Technologies
    Technologies
    • 3D Printing
    • Experts & Guidance
    • FPGA
    • Industrial Automation
    • Internet of Things
    • Power & Energy
    • Sensors
    • Technology Groups
  • Challenges & Projects
    Challenges & Projects
    • Arduino Projects
    • Design Challenges
    • element14 presents
    • Project14
    • Project Groups
    • Raspberry Pi Projects
  • Products
    Products
    • Arduino
    • Avnet Boards Community
    • Dev Tools
    • Manufacturers
    • Product Groups
    • Raspberry Pi
    • RoadTests & Reviews
  • Store
    Store
    • Visit Your Store
    • Or choose another store...
      • Europe
      •  Austria (German)
      •  Belgium (Dutch, French)
      •  Bulgaria (Bulgarian)
      •  Czech Republic (Czech)
      •  Denmark (Danish)
      •  Estonia (Estonian)
      •  Finland (Finnish)
      •  France (French)
      •  Germany (German)
      •  Hungary (Hungarian)
      •  Ireland
      •  Israel
      •  Italy (Italian)
      •  Latvia (Latvian)
      •  
      •  Lithuania (Lithuanian)
      •  Netherlands (Dutch)
      •  Norway (Norwegian)
      •  Poland (Polish)
      •  Portugal (Portuguese)
      •  Romania (Romanian)
      •  Russia (Russian)
      •  Slovakia (Slovak)
      •  Slovenia (Slovenian)
      •  Spain (Spanish)
      •  Sweden (Swedish)
      •  Switzerland(German, French)
      •  Turkey (Turkish)
      •  United Kingdom
      • Asia Pacific
      •  Australia
      •  China
      •  Hong Kong
      •  India
      •  Korea (Korean)
      •  Malaysia
      •  New Zealand
      •  Philippines
      •  Singapore
      •  Taiwan
      •  Thailand (Thai)
      • Americas
      •  Brazil (Portuguese)
      •  Canada
      •  Mexico (Spanish)
      •  United States
      Can't find the country/region you're looking for? Visit our export site or find a local distributor.
  • Translate
  • Profile
Autodesk EAGLE
  • Products
  • More
Autodesk EAGLE
EAGLE User Chat (English) pcb, gerber&drill files problem
  • Blog
  • Forum
  • Documents
  • Events
  • Polls
  • Files
  • Members
  • Mentions
  • Sub-Groups
  • Tags
  • More
  • Cancel
  • New
Autodesk EAGLE requires membership for participation - click to join
Actions
  • Share
  • More
  • Cancel
Forum Thread Details
  • State Suggested Answer
  • Replies 8 replies
  • Answers 1 answer
  • Subscribers 147 subscribers
  • Views 590 views
  • Users 0 members are here
Related

pcb, gerber&drill files problem

Former Member
Former Member over 10 years ago

Hi there,

 

I'm ready to send my first board to a pcb manufacturer. I've generated the GBL,GTL,GBS,GTS,GBO,GTO and the drill TXT file using the manufacturer's cam.

Now the problem is that when I open those files with two separate gerber viewers (GERBV 2.6 and Viewplot) I get the same result.. the holes are where they're supposed to, but everything else is placed +0.409 mm from the origin, on both axes.

It took me a while to understand what's wrong, and after that I placed everything in Eagle's Board Editor 0.409 mm right from and 0.409 mm above the origin. After that I generated a new set of gerber/drill files and the problem seemed to be solved. I mean I get the same exact (positive) results in two different gerber viewers.

 

My questions is why is that happening, if it's normal (like an alignment of the board from 0.409,0.409 and not from 0,0) and if should send it like that.

Can I trust these software viewer that the board would look exactly like that when finished ?

 

what's bother me the most is that in the second scenario the holes are still at the same coordinates and only the other layers were repositioned (although I selected and moved everything in eagle).

 

thanks in advance

  • Sign in to reply
  • Cancel
  • Former Member
    0 Former Member over 10 years ago

    I just made some progress !?

     

    In the manufacturer's CAM everything but the drill file has "Pos. Coord." and "Optimize" checked.

    I've enabled these two options for the drill file, repositioned the board at 0,0 (lower left corner) and remade the gerber+drill files.

    Now everything looks in place, but I still wonder why.

     

    Should I send the files like this and why were those options unmarked ?

     

    *sigh...

     

    oh boy.. long night ahead

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • dukepro
    0 dukepro over 10 years ago in reply to Former Member

    On 05/03/2013 08:03 PM, Jim Raynor wrote:

    I just made some progress !?

     

    In the manufacturer's CAM everything but the drill file has "Pos.

    Coord." and "Optimize" checked.

    I've enabled these two options for the drill file, repositioned the

    board at 0,0 (lower left corner) and remade the gerber+drill files.

    Now everything looks in place, but I still wonder why.

     

    To fix this, your best bet is to leave the "Pos. Coord." option OFF

    (unchecked) on all sections of your CAM job.  Everything will line up

    properly.

     

    This has come up several times in the past.  See my post in

    eagle.support.eng dated 26-Mar-2013.  Search for "Gerber files and Pick

    and place file"

     

    The "Pos. Coord." options causes Eagle to move the entire layer such

    that no part of any object is in any quadrant other than the first.

    That is, everything has positive coordinates.  For example, if your

    board has the bottom and left edges along the X and Y axes, and you run

    a 10-mil wire around the board, then half of this line is below the X

    axis, and to the left of the Y axis.  Eagle will shift the layer 5 mils

    right and 5 mils up so that the entire wire is X>=0 and Y>= 0.

     

    Eagle does this on a layer-by-layer basis, so different layers may get

    shifted different distances.  Your drill file already had everything in

    Quadrant 1, thus no shift occurred.  In the past, I have had the copper

    layers shifted one distance, and the tNames shifted a different

    distance, and the bNames shifted yet another distance.

     

    If your board house can't handle negative coordinates, they will shift

    the entire design (not just one layer at a time) as they see fit.

    Besides, they will generally add your design to a much larger panel (48"

    x 48" comes to mind) consisting of multiple designs from different

    customers.  They process the entire panel and cut it up after the entire

    panel is fabricated.  Many times, they will place multiple copies of

    your design on a single panel to more efficiently utilize the panel.

    Larger designs are placed first, and smaller designs fill in the edges.

     

    To find out what's causing the shift you observed, turn on all layers

    with the "display all;" command.  You'll probably see something you

    don't care about (like component values) hanging to the left of the

    Y-axis, or below the X-axis.

     

    HTH,

        - Chuck

     

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Reject Answer
    • Cancel
  • autodeskguest
    0 autodeskguest over 10 years ago in reply to dukepro

    On 05/04/2013 10:39 AM, Chuck Huber wrote:

    On 05/03/2013 08:03 PM, Jim Raynor wrote:

    I just made some progress !?

     

    In the manufacturer's CAM everything but the drill file has "Pos.

    Coord." and "Optimize" checked.

    I've enabled these two options for the drill file, repositioned the

    board at 0,0 (lower left corner) and remade the gerber+drill files.

    Now everything looks in place, but I still wonder why.

    To fix this, your best bet is to leave the "Pos. Coord." option OFF

    (unchecked) on all sections of your CAM job.  Everything will line up

    properly.

     

    This has come up several times in the past.  See my post in

    eagle.support.eng dated 26-Mar-2013.  Search for "Gerber files and Pick

    and place file"

     

    This is especially important if you have the "Standard" or "Light"

    versions and are trying to cram lots of parts in the license-defined

    (160x100mm or 100x80mm) component placement area. The license permits

    you to make the board itself larger than the component placement area,

    and you can route traces through the larger area, but this results in

    negative coordinates. Because of the license limitations you can't shift

    the components to prevent this. Checking the "Pos. Coord." will cause

    the Gerber layers to shift out of alignment unless you place some sort

    of mark on every layer at a common Quadrant III point, an error-prone

    requirement.

     

    Unless your board house just can't deal with negative coordinates, let

    them deal with it.

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • autodeskguest
    0 autodeskguest over 10 years ago in reply to dukepro

    Am 04.05.2013 16:39, schrieb Chuck Huber:

    Eagle does this on a layer-by-layer basis, so different layers may get

    shifted different distances.

     

    Does EAGLE REALLY do this (I NEVER use the CAM processor, so I just

    don't know)? If yes, this seems a very bad thing to me, which should

    DEFINITELY be considered an error and be fixed.

     

    If "Positive coordinates" is active, THE WHOLE BOARD should be shifted

    by the minimum amount necessary to make ALL coordinates positive,

    INDEPENDENT of the current output layers. Only this way the same Gerber

    coordinates mean the same positions.

     

    Andreas Weidner

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • autodeskguest
    0 autodeskguest over 10 years ago

    On 5/3/2013 7:44 PM, Jim Raynor wrote:

    Hi there,

     

    I'm ready to send my first board to a pcb manufacturer. I've generated

    the GBL,GTL,GBS,GTS,GBO,GTO and the drill TXT file using the

    manufacturer's cam.

    Now the problem is that when I open those files with two separate gerber

    viewers (GERBV 2.6 and Viewplot) I get the same result.. the holes are

    where they're supposed to, but everything else is placed +0.409 mm from

    the origin, on both axes.

    It took me a while to understand what's wrong, and after that I placed

    everything in Eagle's Board Editor 0.409 mm right from and 0.409 mm

    above the origin. After that I generated a new set of gerber/drill files

    and the problem seemed to be solved. I mean I get the same exact

    (positive) results in two different gerber viewers.

     

    My questions is why is that happening, if it's normal (like an alignment

    of the board from 0.409,0.409 and not from 0,0) and if should send it

    like that.

    Can I trust these software viewer that the board would look exactly like

    that when finished ?

     

    what's bother me the most is that in the second scenario the holes are

    still at the same coordinates and only the other layers were

    repositioned (although I selected and moved everything in eagle).

     

    thanks in advance

     

    --

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

    http://www.element14.com/community/message/75600#75600

     

     

    Hi Jim,

     

    The key here is the pos. coords option needs to be set the same across

    all of the gerber tabs and drill job. Either have them all set or have

    them unset but you can't have a mix. You don't have to make any changes

    to the board design for this to work.

     

    If pos. coords is checked across all of the tabs then all of the design

    files will have the same offset added to them so everything will line up

    nicely.

     

    hth,

    Jorge Garcia

    Cadsoft Support

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • autodeskguest
    0 autodeskguest over 10 years ago in reply to autodeskguest

    Am 07.05.2013 21:14, schrieb Jorge Garcia:

    The key here is the pos. coords option needs to be set the same across

    all of the gerber tabs and drill job. Either have them all set or have

    them unset but you can't have a mix.

     

    Fine to see that there is a possibility to make this work properly in EAGLE.

     

    BUT since this is not obvious, why leave the user in the dark about it?

    If "pos. coords" should be either on or off in ALL the CAM tabs, why not

      1. either make this option GLOBAL for the whole job (so as not to give

         the user the chance to screw things up),

      2. or leave it as it is, but, in case the user checked the option in

         SOME tabs, but not in others, display a warning that this MIGHT

         cause problems with the Gerber output?

    If a software gives the user vital information on how NOT to do things,

    or prevents him from doing these wrong things, that's MUCH better than

    letting him run against the wall...

     

    Andreas Weidner

     

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • dukepro
    0 dukepro over 10 years ago in reply to autodeskguest

    On 05/08/2013 04:31 AM, Andreas Weidner wrote:

    Am 07.05.2013 21:14, schrieb Jorge Garcia:

    The key here is the pos. coords option needs to be set the same across

    all of the gerber tabs and drill job. Either have them all set or have

    them unset but you can't have a mix.

     

    Good morning, Jorge,

     

    Thanks for this bit of information.  I knew everything lined up with

    pos. coords turned off.  I don't believe I've ever tried it with all of

    them on.

     

    I never use this anyway, and in the default (empty) CAM job they're on.

    I have yet to run across a board fab house that can't handle negative

    coordinates.  However, I can see where it'd be handy to have if you're

    cutting your own boards.

     

     

    Fine to see that there is a possibility to make this work properly in

    EAGLE.

     

    BUT since this is not obvious, why leave the user in the dark about

    it? If "pos. coords" should be either on or off in ALL the CAM tabs,

    why not

    1. either make this option GLOBAL for the whole job (so as not to give

        the user the chance to screw things up),

     

    Andreas makes a good point here.  Perhaps Pos Coord should be associated

    with the job, and not each section.  The X and Y offset would also be

    good candidates for the same treatment.

     

    Enjoy,

        - Chuck

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
  • autodeskguest
    0 autodeskguest over 10 years ago in reply to autodeskguest

    On 5/8/2013 4:31 AM, Andreas Weidner wrote:

    Am 07.05.2013 21:14, schrieb Jorge Garcia:

    The key here is the pos. coords option needs to be set the same across

    all of the gerber tabs and drill job. Either have them all set or have

    them unset but you can't have a mix.

     

    Fine to see that there is a possibility to make this work properly in

    EAGLE.

     

    BUT since this is not obvious, why leave the user in the dark about it?

    If "pos. coords" should be either on or off in ALL the CAM tabs, why not

      1. either make this option GLOBAL for the whole job (so as not to give

         the user the chance to screw things up),

      2. or leave it as it is, but, in case the user checked the option in

         SOME tabs, but not in others, display a warning that this MIGHT

         cause problems with the Gerber output?

    Hi Andreas,

     

    I like number 2, I'll file an enhancement report on this. I don't think

    it would be difficult to implement so thanks for the idea.

     

    Best Regards,

    Jorge Garcia

    If a software gives the user vital information on how NOT to do things,

    or prevents him from doing these wrong things, that's MUCH better than

    letting him run against the wall...

     

    Andreas Weidner

     

     

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Verify Answer
    • Cancel
element14 Community

element14 is the first online community specifically for engineers. Connect with your peers and get expert answers to your questions.

  • Members
  • Learn
  • Technologies
  • Challenges & Projects
  • Products
  • Store
  • About Us
  • Feedback & Support
  • FAQs
  • Terms of Use
  • Privacy Policy
  • Legal and Copyright Notices
  • Sitemap
  • Cookies

An Avnet Company © 2023 Premier Farnell Limited. All Rights Reserved.

Premier Farnell Ltd, registered in England and Wales (no 00876412), registered office: Farnell House, Forge Lane, Leeds LS12 2NE.

ICP 备案号 10220084.

Follow element14

  • X
  • Facebook
  • linkedin
  • YouTube