Connect with us

Some questions regarding board design

Discussion in 'CAD' started by [email protected], Mar 12, 2009.

Scroll to continue with content
  1. Guest

    Hi,

    I have been designing boards for myself for quite awhile BUT I am
    using a mechanical etch process to fabricate them on an IBC2222
    BoardMaker machine. This process is quite different than going to a
    vendor. My day has finally arrived that I have to rely on a vendor to
    produce some one off boards for me. I have read the David L Jones
    document available on the web but I still have a few questions I am
    hoping that I can get some help on so here goes......

    1.) How are non-plated thru holes handled? Do they still require a pad
    ring to allow the plate thru process to work and then they get drilled
    to the finished size.

    2.) My CAD system is lacking in area fill capability. Do the PCB
    vendors allow using a combined layer negative for the fill.planes and
    combining it with a positive artwork layer to get the connections in.
    Same goes for ground plane layers, do the vendors accept them as
    negatives?

    3.) What are typical clearances for solder mask artwork? Can the
    openings go right up against the edge of pads? Can this artwork be a
    negative too?

    4.) How do I define the cut-out shape as the boards are circular so a
    simple shear cross hairs in the corners won't do it. Do I provide a
    layer with the shape to be cut-out?

    5.) I require countersunk mounting holes around the periphery. How to
    I indicate that? Would it be a see Note ### for more information?

    Many thanks to all who are able to help me out.

    regards,
    al
     
  2. Rich Webb

    Rich Webb Guest

    Take a look at the pre-order checklist and FAQs at
    http://www.pcbexpress.com/index.php. That's just one vendor but the
    general capabilities and limitations are similar.

    You're probably far better off (in cost and in eventual satisfaction)
    the less you depend on manipulation of your files by the board house.

    It's possible to use tools like ViewMate http://www.pentalogix.com/ to
    "swell" the pads in a Gerber layer to make a new Gerber for a mask
    layer. Not available in the free version, though. Try 10 mils (0.01")
    for your mask clearance.
     
  3. My vendor says just to label them "NONPTH" on the drill chart. You
    don't need a pad.
    Yes it is normally a negative. Not sure about clearance - ask
    them. Mine seem to increase the clearances themselves...
    I usually do it as part of the drill chart, just a thin line
    whose center represents the edge of the board. I used to ask them what
    router they use and carefully draw in a channel that wide, but don't
    bother now. They seem to figure it all out themselves. You should ask
    them though. They may need to leave little bits that keep the circle
    attached to the rectangular panel.
    Guess so, never tried asking for countersinking.
    The Chinese vendor I use does each job separately, so it is no
    problem. Some of the lower cost European and US services may offer low
    prototype prices because they can combine your job as part of a larger
    panel. They therefore have stricter rules about what you can and
    cannot do while remaining in the low-cost scheme.
     
  4. qrk

    qrk Guest

    No pad required. Note in the Drill Drawing which holes are non-plated.
    I assume they drill after the final plating process is done. We supply
    a separate drill file for NPTH, but that isn't necessary.
    Ask your vendor. They should have the capability to merge layers, even
    flip a negative, then merge with positive. I've done this in the early
    days using PCAD.
    Ask your vendor. A good vendor can hold 2 mil clearance. Don't use
    zero or you will get mask on your pads. The clearance is for
    registration issues.
    You can show this in the Drill Drawing. Show the board outline and
    dimensions. Complicated outlines, I include a drawing of the outline
    showing all the dimensions. Some places will route along an outline
    you provide on one of the layers, good board houses will go off a
    drawing. Shear cross-hairs aren't necessary. The board house will use
    their own targets and drill holes to align the stackup. The final
    board is routed out of the panel, not sheared.
    Ask you vendor if they can do this. Put that in the drill drawing or a
    separate mechanical drawing. Also, note it verbally in your readme
    file that explains each layer name and how you want those layers
    processed (copper weight, layer separation, material, special
    features, layer merging, ...). We have a blind drill hole in one of
    our boards thats done after the final lamination. They're pretty good
    at controlling the depth.
    Bottom line, you need to talk to your vendor. If they are a quick-turn
    prototype house, much of what you want can't be done at cheap prices.
    You'll need to resort to their full service offering.
     
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

-