Connect with us

EasyPC Gerber "Dimensions" File Problem

Discussion in 'CAD' started by [email protected], Mar 15, 2007.

Scroll to continue with content
  1. Guest

    I sent a set of Gerber files from EasyPC v8.0.8 to Advanced Circuits
    ( ), and was told that the "dimensions" file
    contained improper information ("only two small dashes"). This
    resulted in my pcb design being put on "CAM Hold", which delayed its

    I ended up having to create a PDF for them, with a drawing showing a
    marked reference point and the dimensions to each side of the PCB
    outline from the reference point, so they could make a Gerber
    dimensions/outline file, for me, from that.

    This was the first time that I had had someone else make boards for
    me. This was for a 2-sided board, 9.75" x 2.9375". I did use's very nice "FreeDFM" check, first, which showed NO errors.
    And all of the PDF drawings of the copper layers, silkscreen, and
    soldermask layers, which their FreeDFM automatically creates from
    uploaded Gerber files and emails back, looked fine.

    Using Windows Notepad, I looked in the Gerber "dimensions" file that
    EasyPC had created. Here is the whole thing:

    G04 EasyPC Gerber Version 8.0.8 Build 2014 *

    I'd never seen the inside of a Gerber file, before this, and don't
    have a Gerber file viewer (YET). So I don't know if this looks
    reasonable, or not. But apparently it's not, or else there was a
    problem while transmitting it.

    I'm also wondering if maybe there is some setting, within EasyPC, that
    I need to change. If not, what could be the problem and what could I
    do about it? Anyone? Or maybe it's time to upgrade to EasyPC v10.


    - Tom Gootee

  2. Paul Burke

    Paul Burke Guest

    The Gerber file you posted is just a stripe 0.57mm long and 0.026mm wide
    according to GCPrevue ( This is worth
    downloading and using to check out your Gerbers before sending.

    Where did the "dimensions" Gerber come from? It's not part of the usual
    set, and there's an option in PCB plot to include the board outline in
    the plot.
    The Gerber is valid- it's just nonsense as a manufacturing file.
    Version 8 was just fine. So is version 10. I can't remember when they
    introduced it, but the big thing for a while has been 3D view, which I
    don't use being a sad git. The copper pour has also got a lot more reliable.

    Paul Burke
  3. Guest

    I'm sorry of two of these are posted. It looks like my first attempt
    has vanished.

    Thanks, Paul! I have downloaded it.
    The "dimensions" file was produced by EasyPC, with no special action
    on my part. (It does appear to be part of the standard set of
    Gerbers, in my EasyPC setup.)

    Oddly, maybe, when I highlight the "Dimensions" plot name and click on
    the "Layers" tab, the "Board Outline" line has its "Selected" column
    set to "No", by default. (But there is a "Dimensions" line that has
    "Selected" set to "Yes", by default.) Next time, I'll try also
    setting "Board Outline" to "Yes", for the Dimensions file, since the
    board outline is what the "CAM Hold" guys seemed to be wanting, from
    that file. I must have been too sleep-deprived to think to check
    that, at the time.

    I also don't know if a separate Dimensions file would have been
    required, if I'd simply included the board outline on some or all of
    the other plots. But I had just used the default settings that EasyPC
    had, which didn't include the board outline on ANY of the other plots,
    and did include the Dimensions plot.

    One thing that I did change, after my first "freeDFM" check, was to
    select "Hardware Fill" and "Hardware Arcs", in the "Output" tab's
    "Device Setup" dialog, under "RS-274-X (Extended Gerber)", because
    without "Hardware Fill", the poured copper areas were filled using
    _lines_, which, only in certain cases, caused freeDFM to complain
    about lots of very thin tracks. I could actually see them, too, on
    the PDFs of the artwork that were emailed back to me (at least at
    magnifications above something like 1200X). The Gerber files were
    also significantly larger, without "Hardware Fill". Using "Hardware
    Arcs" is apparently a good idea, too, since, otherwise, arcs are
    rendered using multiple line segments.
    You should try their free FreeDFM service! ( ,
    or, ) It's not just a Gerber syntax checker. It
    checks (apparently) ALL sizes and clearances, etc etc, and also
    automatically "thickens" all silkscreen artwork to meet their minimum
    line-thickness requirement. Then, usually within a few minutes, it
    emails back a fairly-well-detailed report, which includes a nice price
    quote with both prototype and production pricing, PDFs of the artwork
    for each layer (a free on-line Gerber viewer, in essence), and, an
    Error Summary, with the number (quantity) of each type of error found,
    and five samples of each type of error it found. Each error-sample
    includes three zoom views of artwork showing the error, with a text
    description giving the error margin/measurement and its coordinates,
    plus a description of the relevant manufacturing requirement that was
    not met. It seems like it probably saves their CAM engineers and
    their customers a ton of time and aggravation, at least for
    inexperienced customers like me. (But apparently they need to start
    also checking the Dimensions file, if it's used.)

    Aside: I didn't take advantage of any of their pricing "specials".
    But my prototypes' pricing seemed pretty good, although maybe a bit
    weird: They wanted $54 each for qty 5 ($270), but $30 each for qty 10
    ($300), for a three-day turnaround. I took the 10! But now I'm
    kicking myself for not checking the price for 20. (In the emailed
    price quote that's included with the freeDFM report, you can simply
    change a quantity and click to update the list of quotes versus turn-
    times, and can click on any unit-price to place an order.) Those
    prices, for 2.94" x 9.75" 2-sided .031" FR4, included lead-free
    solder plating, green solder mask on both sides, white silkscreen on
    top, board dimensions cut within .01", and other stuff. They must use
    lasers to do the drilling, because I didn't see anything at all about
    pricing versus number of drill sizes, or anything like that. And I
    also had some non-standard hole sizes, which were never mentioned.
    All-in-all, it was a relatively-painless first-timer experience (and,
    probably largely thanks to their freeDFM check, would have been almost-
    completely uneventful, had it not been for my Dimension file
    problem). I also liked being able to go to their website to track the
    progress of the boards' processing. (This is starting to sound like
    an advertisement. But no, I am not affiliated with Advanced Circuits
    or their people in any way. I just enjoyed their nicely-automated
    setup, and their very-attentive service.)
    Yes, I love EasyPC v8. The 3D and better-rendering stuff was just
    starting to be hinted-at, in my v8, but was only in a few of the
    examples, as far as I could tell, not being too interested at the
    time, as I was first learning it. I would actually like to have 3D,
    now, so I could more-easily check component clearances, etc. But I
    don't know if it could do what I need, since I'd like to be able to
    see the clearances between components on two boards that are at a
    right angle to each other. If they could provide that, I'd upgrade
    tomorrow, even though that would mean paying more, to also raise my
    pin limit above 1000, since one of the six boards I'd like to simulate
    in 3D together, at the moment, has something like 975 pins. I'll
    email them and try to find out more about the 3D capabilities.

    I'm REALLY glad to hear that the copper pouring is more reliable, in
    v10! That's one of the (few) main things in v8 that is fairly-often
    quite aggravating.

    I did just go to , and looked at a list of
    some of the improvements in v10. One that caught my eye was something
    about showing clearances on-the-fly, while editing tracks. I'd
    probably have given them my car, for that, a while back. I'm
    definitely going to upgrade, now.

    Thanks, Paul!
    Tom Gootee

  4. RHRRC

    RHRRC Guest

    I suspect there is a 'glitch' with this particular installation of
    easypc since this is- and has been for a very long time - a well
    known, capable, and respected pcb layout package.

    from the sample gerber given - it ain't all there!!

    I suspect that the 'dimensions' the pcb house was asking for is the
    aperture dimensions file - generally just referred to as the apertures
    file - in days of old, but not so oftennow, it was called the D codes
    sizing file (or similar).
    Normally easypc (and just about every other pcb package) produces 274X
    gerbers - they do not have a seperate apertures file. If the output is
    set to 274D gerbers then there must be a seperate aperture file.
    Since the pcb house could make no sense of the gerber file provided I
    guess they may have asked for the aperture dimensions file to see if
    that was the problem since this is the only other 'gerber' file there
    On the other hand it could be nothing to do with it.
  5. Guest

    Just for completeness' sake: The solution was to select the Dimensions
    plot and then select Layers and make sure that Board Outline was

    No more "Cam Hold" delays.

    - Tom Gootee

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