Connect with us

Problem with gerber file names

Discussion in 'Electronic Design' started by [email protected], Mar 7, 2007.

Scroll to continue with content
  1. Guest

    Hi everybody,
    I'm trying to prototyping a board with an on-
    line sevice found on the web. They ask me some gerber files that don't
    match with mine produced with OrCAD Layout.
    Notably they ask me a .GKO file - the gerber file associated with
    board outline-, but OrCAD doesn't produce any gerber file with this
    features...
    The Gerber file produced by my CAD are:
    myproj.TOP
    myproj.BOT
    myproj.SMT
    myproj.SMB
    myproj.SST
    myproj.DRD
    myproj.DTS
    myproj.GTD
    thruhole.TAP

    but none of them concerns the board outline.....
    Anybody knows how to produce this missing Gerber file?

    I have realized that the gerber extentions produced by the post-
    processor of OrCAD Layout are different from that ones produced by
    Protel and EAGLE, for istance.
    GKO is a Gerber extention used by these two CADs and I wish two know
    the corresponding extention (if exists) in OrCAD.

    Regards,
    Alex
     
  2. John  Larkin

    John Larkin Guest

    It's usually submitted as a fab drawing, not a gerber. It has the
    outline plus materials, stackup, color, and tolerance notes.

    John
     
  3. Dear friend :
    It is my fortunate writing to you . you will discover this is a wealth
    accumulation place.
    The website of our company is http://www.china-powerseller.com
    We are a big agent for Laptop
    Mobile Phone\Digital Camera\CDJ\DJM\Apple Ipod\PSP\VEDEO GAMES
    \Television\GPS\Telescope in CHINA .
    All of our commodities is the most advanced quality but lowest price.
    we also have the

    safest and most
    convenient transaction way to guarante the transaction arries on
    normally .
    looking forward to your coorporation and cause all of us both to
    profit.
    you can contact us by Email:china.seller#hotmail.com
    MSN: china.seller#hotmail.com
    best wishes!
    your sincerely

    http://www.china-powerseller.com
    MSN/Email:
     
  4. TT_Man

    TT_Man Guest

    WTF has that got to do with Gerbers? Western Union payment as well I
    presume?
     
  5. Didi

    Didi Guest

    Here is a typical text file I send out with my boards.
    Last time I had to convert my Gerbers to extended-Gerber,
    which cost me some work but OTOH elliminates a potential
    source of error (D-codes are embedded in the x-Gerber).

    Here is the file (just inserted as it is, hopefully it is
    of some use):

    -------
    25 - 59.8 mil (1.52 mm) circle,
    27 - 63 mil (1.6 mm) circle.

    Drilling tools:
    1 - 0.3 mm (about 0.2 after plating), 0.2 drilling is also OK,
    2 - 1.0 mm,
    3 - 1.0 mm,
    4 - 1.0 mm,
    5 - 1.3 mm,
    6 - 3.1 mm,
    7 - 2.0 mm.

    The board must be cut by the contour of one of the inner layers
    (e.g. layer 2, ipnl2.gbr) as if the cutting tool has zero width
    and moves through the middle of the countour line.

    The stackup is as following:
    ipnl1.gbr
    ipnl2.gbr
    ipnl3.gbr


    ipnl4.gbr
    ipnl2.gbr
    ipnl5.gbr

    Total board thikness apr. 1.5 mm or so (perhaps 1.6 is popular
    nowadays).

    The spacing between ipnl2.gbr (the GND layer) and its neighbour
    layers, both in the top and bottom 3 sets, must be something
    like 6 mil or so (so the impedance of the top and bottom
    signal layers referenced to the neighbour GND layer is about
    50 ohm). All this assumes FR4 material.

    The signal layers have been routed with 5 mil gaps and traces in mind,
    with 4 mil spaces when passing close to vias/BGA pads. The Gerber
    files have been verified to pass a 4 mil gap check.

    For any questions please contact Dimiter Popoff <>,
    or Skype didi_tgi (or call ++359/2/9923340 )
     
  6. Didi

    Didi Guest

    Oops, part of the file was lost, here I go again:

    Here is a typical text file I send out with my boards.
    Last time I had to convert my Gerbers to extended-Gerber,
    which cost me some work but OTOH elliminates a potential
    source of error (D-codes are embedded in the x-Gerber).

    Here is the file (just inserted as it is, hopefully it is
    of some use):

    -------
    File description:
    ipnl1.gbr - top signal layer (layer 1),
    ipnl2.gbr - GND plane layer, goes as layer 2 and 5,
    ipnl3.gbr - internal plane, layer 3,
    ipnl4.gbr - internal plane, layer 4,
    ipnl5.gbr - bottom signal layer (layer 6).

    NOTE: ipnl2.gbr, ipnl3.gbr and ipnl4.gbr are plotted as NEGATIVES.
    They are all copper planes except for the lines and pads plotted
    on them.

    ipnsm1.gbr - solder mask for top layer,
    ipnsm2.gbr - solder mask for bottom layer.

    D-codes:

    11 - 4.3 mil (0.11 mm) circle,
    12 - 6.3 mil (0.16 mm) circle,
    14 - 9.8 mil (0.25 mm) square,
    15 - 9.8 mil (0.25 mm) circle,
    16 - 11.8 mil (0.30 mm) square,
    19 - 17.3 mil (0.44 mm) circle,
    21 - 20.1 mil (0.51 mm) circle,
    22 - 50 mil (1.27mm) circle,
    23 - 55.1 mil (1.40 mm) circle,
    25 - 59.8 mil (1.52 mm) circle,
    27 - 63 mil (1.6 mm) circle.

    Drilling tools:
    1 - 0.3 mm (about 0.2 after plating), 0.2 drilling is also OK,
    2 - 1.0 mm,
    3 - 1.0 mm,
    4 - 1.0 mm,
    5 - 1.3 mm,
    6 - 3.1 mm,
    7 - 2.0 mm.

    The board must be cut by the contour of one of the inner layers
    (e.g. layer 2, ipnl2.gbr) as if the cutting tool has zero width
    and moves through the middle of the countour line.

    The stackup is as following:
    ipnl1.gbr
    ipnl2.gbr
    ipnl3.gbr


    ipnl4.gbr
    ipnl2.gbr
    ipnl5.gbr

    Total board thikness apr. 1.5 mm or so (perhaps 1.6 is popular
    nowadays).

    The spacing between ipnl2.gbr (the GND layer) and its neighbour
    layers, both in the top and bottom 3 sets, must be something
    like 6 mil or so (so the impedance of the top and bottom
    signal layers referenced to the neighbour GND layer is about
    50 ohm). All this assumes FR4 material.

    The signal layers have been routed with 5 mil gaps and traces in mind,
    with 4 mil spaces when passing close to vias/BGA pads. The Gerber
    files have been verified to pass a 4 mil gap check.

    For any questions please contact Dimiter Popoff <>,
    or Skype didi_tgi (or call ++359/2/9923340 )

    -----

    Dimiter

    On Mar 7, 6:53 pm, wrote:

    - Hide quoted text -
    - Show quoted text -
     
  7. Where can you get a square drill?
     
  8. Arlet

    Arlet Guest

    These do not refer to the drills. These are the "D-codes". These
    shapes are used to draw the artwork.

    See http://www.artwork.com/gerber/appl2.htm
     
  9. John B

    John B Guest

    It's been a long time since I used OrCad, but I think you'll find the
    board outline is in the '.DRD' file. You can also get it to include the
    board outline in the copper layer files ('.TOP' & '.BOT').
     
  10. In Protel, *.GKO would be the keep-out layer, which would rarely match
    the board outline.

    I put the board outline on a "mechanical" layer, then ask the Gerber
    output routine to include that layer on all copper layers. I can then
    instruct the board shop to trim the boards to the outline - seems to
    work fine for me.

    In any case, you have to tell the shop the board outline somehow -
    either by including it on the copper layer, or by providing a separate
    file.

    The readme file I send with my Gerbers looks like:

    =================================

    Job: 0983 TRIUMF Octal DAC
    PC Board P-13190 rev 0

    The following files are required for this job:
    p13190.GTL Component side copper photoplot file
    p13190.GP1 Internal Ground Plane
    p13190.GP2 Internal Power Plane
    p13190.GBL Solder side copper photoplot file
    p13190.GTO Top Component layout silkscreen
    p13190.GBO Bottom Component layout silkscreen
    p13190.GBS Bottom Solder Mask
    p13190.GTS Top Solder Mask
    p13190.TXT Drill file
    readme.txt This file


    Note: the Gerber files include embedded aperture data.

    Tool Hole Size Hole Count Plated Tool Travel
    ---------------------------------------------------------------------------
    T1 16mil (0.4064mm) 343 112.54 Inch (858.64 mm)
    T2 25mil (0.635mm) 9 36.08 Inch (916.40 mm)
    T3 35mil (0.889mm) 172 77.13 Inch (1959.06 mm)
    T4 40mil (1.016mm) 10 5.77 Inch (146.46 mm)
    T5 50mil (1.27mm) 12 16.87 Inch (428.41 mm)
    T6 55mil (1.397mm) 6 3.68 Inch (93.48 mm)
    T7 110mil (2.794mm) 10 27.68 Inch (703.05 mm)
    T8 141mil (3.5814mm) 4 11.60 Inch (294.54 mm)
    ---------------------------------------------------------------------------
    Totals 566 291.34 Inch (7400.04
    mm)


    The board is 7.20" x 11.95", +/- .010", four layer,
    ..0625" nominal thickness, FR-4 material
    1 oz or greater copper
    Standard through-hole plating, standard white tin plating on exposed
    copper.
    Standard gold plating on edge connector

    Solder mask both sides (different masks)
    Component Ident silkscreen on both sides

    Trim boards to outline on component side artwork

    --
    Peter Bennett, VE7CEI Vancouver BC, Canada
    peterbb4 (at) interchange.ubc.ca
    new newsgroup users info : http://vancouver-webpages.com/nnq
    GPS and NMEA info: http://vancouver-webpages.com/peter
    Vancouver Power Squadron: http://vancouver.powersquadron.ca
     
  11. nospam

    nospam Guest

    Bet they hate you making them strip the outline from every gerber layer
    before they plot it.

    Give them an outline on a separate layer, they will either just look at it
    or use it as a guide for creating a route.

    I always give a paper (well PDF) copy of that layer including basic
    dimensions and showing holes one of which is dimensioned so there can be no
    confusion about alignment between gerbers and drill files.
    --
     
  12. Eeyore

    Eeyore Guest

    If they can't use the files that OrCad produces do you really want to use them ?

    Doesn't bode well for their competence !

    Graham
     
  13. Brian

    Brian Guest

    Gerber isn't an intelligent format. You could put the outline on any
    layer (I have gotten in some pathetic gerber files at times). But the
    proper place for the board out line is eiter on your drill drawing or
    on a seperate mechanical layer you make. You will have to go into your
    gerber set-up and add the outline layer to your drill drawing gerber
    output if it is not already putting it their (or create a new one
    called Mechanical). I haven't used Orcad in 15 years, can't help much
    on the details of the process.

    Its probably NOT that the company can't use Orcad Gerber, its simply
    that the outline layer is not in any gerber file. How can they figure
    the outline if it is undefined in the files? Or, I could be wrong and
    they are incompetent. If you email me the gerbers (if nothing top
    secret), I would be happy to take a peek.

    Brian
     
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day

-