Connect with us

pcb design rules

Discussion in 'CAD' started by [email protected], Feb 22, 2007.

Scroll to continue with content
  1. Guest

    Hi all

    I'm trying to get a feel for what pcb design rules to use. I have
    found various manufacturers sites which define their minimum track,
    gap and drill size but I'm trying to work out in what order I should
    be reducing each of these to get my pcb routed.

    Any thoughts or links most appreciated.

    Colin
     
  2. engcif

    engcif Guest

    Hi,
    I depends on mostly the PCB manufacturer. If you are going to produce
    mass productions ask some of the firms that you are working with I
    suggest. We have different types of PCB rules for different projects
    and different manufacturers. You may send your Gerber files to the
    manufacturers and they usually check whether it is proper or not
    before production.
    Engin
     
  3. Paul Burke

    Paul Burke Guest


    I always make track and gap equal (unless there's an electrical reason
    to do otherwise). I've found that decent PCB makers have no problem with
    6 thou tracks/ gaps, but it helps to keep the minimum hole a bit up, say
    0.4mm or 0.5mm, if you can.

    Why by the way are tracks always in thou and holes in millimetres?

    Paul Burke
     
  4. qrk

    qrk Guest

    In 'merica, we use mils (thou) for drill holes.
    Most decent PCB houses can deal with 5/5 mil rules. Below that, you
    need to find a good house and pay more. Any wanker PCB house can
    handle 10/10 rules. I routinely use 8 mil via holes for my crammed
    boards. The board house will be happier if your via holes are more
    like 13 to 20 mils. Before commiting to a PCB house, see if they can
    show you a sample of their work. Talk to the PCB houses and find out
    what rules you should follow, especially if you're trying to hit a
    price target.
     
  5. Leon

    Leon Guest

    That's quite common in the UK. I find them easy to visualise, for some
    reason.

    Leon
     
  6. James Beck

    James Beck Guest

    He stated "always" and that isn't true.
    We do all our design in mils, traces, holes, pads, spacings.
    I think it is more of a use whatever works for you kinda' thing.

    Jim
     
  7. It would help to know what sort of board you are designing.

    For simple boards using only through-hole components, I normally use
    10 or 12 thou tracks and spaces, and 62 thou pads with 35 thou holes
    for most parts. Vias are usually 50 thou pads and 25 thou holes.

    Holes for component leads are usually 5 - 10 thou larger in diameter
    than the leads, and pads 20 - 30 thou larger than holes (this leaves a
    20 - 15 thou wide annular ring around the pad).

    --
    Peter Bennett, VE7CEI
    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
     
  8. Guest

    What I am trying to understand is for a certain track and gap what via
    size I should use. Presumably the two go hand in hand so that if a
    design doesn't quite fit I would be able to reduce both for the same
    incremental rise in costs but all I find is "ideally use this" and
    "worst case we can cope with this" but the grey area between doesn't
    get a mention.

    Colin
     
  9. Dave Pollum

    Dave Pollum Guest

    I use EAGLE for PCB design. All of my boards have been prototypes (2
    layer and 4 layer). I typically use 10 mil (0.010") wide traces and
    10 mil wide spaces. For power runs (i.e. 5v) I use 24 or 32 mil
    traces. For vias, I specify a 20 mil (0.020") drill. Eagle's
    standard via drill size is ~ 25 mils. To connect a heavy trace on one
    side to the corresponding heavy trace on the other side, I usually use
    2 20 mil vias instead of 1 large via.
    HTH
    -Dave Pollum
     
  10. ghl

    ghl Guest

    Maybe this link helps.
    http://www.smps.us/pcb-design.html

    BTW, there is a worldwide shift to the metric system, according to IPC.
    The driving force is an EC regulative.

    150 micrometres width and space is common for most professional board
    makers with vias as small as 0.3/0.7 mm final dimension. Minimum is 75
    micrometres for larger production quantities with vias as small as
    0.1/0.3 mm (bore/ring) - so called microvias. Only a few can do this.
    E.g. in Germany you might find around 5 PCB manufacturers doing this.
    Utmost minimum is 50 micrometres, but with a high count of unrectifiable
    rejects. I know one manufacturer.

    200 micrometres with 0.4 mm bores is standard low cost. There is almost
    no exemption.

    Greetings
    GerhartH
     
  11. At some time in a previous century, the board shop charged extra
    because I had specified 24 thou vias instead of my usual 25 - this
    made me standardize on 25 thou. However, the board shops I use are
    now willing to go down to 16 thou or less at no extra charge -
    however, from habit, I still stick with 25 thou unless I really need
    to conserve space.

    --
    Peter Bennett, VE7CEI
    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
     
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

-