Connect with us

Multilayer PCB Notes.

Discussion in 'CAD' started by GMM50, Feb 3, 2005.

Scroll to continue with content
  1. GMM50

    GMM50 Guest

    Hello:

    I'm about to release for manufacturing a 4 layer PCB
    1. Top Signal
    2. Ground
    3. Power
    4. Signal

    The design rules are 8 mil lines and 8 mil spacing. And it's mostly
    SMT devices.
    THe board size is 16 x 10 inches.

    It's been a while since I specified such a complicated (expensive) PCB
    and my notes are old.
    My question is where should I look for a set of notes to add to the
    detail drawing for the board.

    Specifying itmes such as silk screen, soldermask, solder mask over bare
    copper, dimensions and warp and twist.
    And all the other things I forgot.
    THanks
    George
     
  2. Leon Heller

    Leon Heller Guest


    Most manufacturers sort all that stuff out for you, I just supply the
    Gerbers and they get on with it. The default values with my PCB software
    work OK.

    With a big board like that warp and twist might be a problem, I had problems
    with a four-layer double-eurocard design some years ago from one supplier.

    Leon
     

  3. This is what I use to use at a company that I worked for. Include it
    as a readme.txt file with your gerbers.

    Fabrication Information from Light & Sound Design.


    PCB Part No: 5689302A-AW

    PCB Description: Control Panel Assembly

    Number of Track Layers: 2
    Number of Power Planes: 2
    PCB Material: FR4
    PCB Thickness: 0.062 inch
    Copper Weight: 1 Oz finished
    Top Silkscreen: White
    Bottom Silkscreen: White
    Solder Mask Both Sides: Liquid photoimagable
    Minimum Track Width: 0.008 inch
    Minimum Clearance: 0.007 inch
    Solder Mask Expansion: 0.0003 inch (radial)
    Pad Finish: Hot Air Solder Leveling



    Fabrication Tools:
    (layer order to be as follows)

    5689302A-AW.GTO Top Silkscreen
    5689302A-AW.GTS Top Solder Mask
    5689302A-AW.GTL Top Layer Copper Tracks
    5689302A-AW.GP1 Internal Plane 1 Copper ( v)
    5689302A-AW.GP2 Internal Plane Copper (ground)
    5689302A-AW.GBL Bottom Layer Copper Tracks
    5689302A-AW.GBS Bottom Solder Mask
    5689302A-AW.GBO Bottom Silkscreen

    ---------------------------------------------------------------------------
    NCDrill File Report For: 5689302A-AW.pcb 31-Dec-2002 12:15:01
    ---------------------------------------------------------------------------



    Layer Pair : TopLayer to BottomLayer
    ASCII File : NCDrillOutput.TXT
    EIA File : NCDrillOutput.DRL

    Tool Hole Size Hole Count Plated Tool Travel
    ---------------------------------------------------------------------------
    T1 32mil (0.8128mm) 2 2.29 Inch (58.29
    mm)
    T2 37mil (0.9398mm) 78 16.12 Inch (409.35
    mm)
    T3 55mil (1.397mm) 8 2.16 Inch (54.93
    mm)
    T4 125mil (3.175mm) 2 NPTH 3.64 Inch (92.52
    mm)
    ---------------------------------------------------------------------------
    Totals 90 24.22 Inch (615.09
    mm)


    Contact: Patrick T. Caezza
    Phone: (805) 499-XXXX
    Fax: (805) 499-XXXX
     
  4. Robert Baer

    Robert Baer Guest

    Properly made PCBs will not warp or twist, unless you cycle them over
    a large temperature range.
     
  5. So how do you spec the required flatness? I've only seen problems
    after soldering.


    Best regards,
    Spehro Pefhany
     
  6. GMM50

    GMM50 Guest

    That's a good format for a start.

    Now what about alignment accruacy/tolerance? I used to use +/- 0.005"
    but I suspect it can be tighter without adding cost.

    Board dimensions? Could be covered on the fab drawing.

    Warp and twist. I've seem 0.005" per inch of board dimension measured
    by holding one corner of the board to a surface plate and measuring the
    highest point above that surface. With a larger PCB it needs to be
    flat enough so the pick and place machine can accurately do it's job.

    There used to be test cupons used to measure solderability
    (delamination) on multilayer PCB. We would shock the cupon (no prehead
    and dip in solder pot) and if it delaminated then we would do a proper
    test (proper preheating). This gave us a margin.

    I also need to be sure the solder is level enough to keep the placement
    accuracy.

    Any one else??

    THanks
    George
     
  7. vax, 9000

    vax, 9000 Guest

    I am fighting with myself whether I want to design for 4 layers or 2 layers.
    Is a 4 layer board supposed to be less likely to twist than a 2 layer board?
    I want my boards to last long and keep in good shape even that means some
    more investment. Thank you.

    vax, 9000
     
  8. Leon Heller

    Leon Heller Guest

    Try to have equal amounts of copper on the top and bottom, evenly
    distributed, with most of the tracks on the top running at right angles to
    the tracks on the bottom. That should minimise the problem.

    Leon
     
  9. Chuck Harris

    Chuck Harris Guest

    The twisting and warping is mostly due to poor workmanship when they are thermo
    laminating the boards together. Multilayer boards are etched as individual one and
    two sided boards using very thin board stock. They are smeared with a thermo setting
    adhesive, and run through a hot press. If this stage isn't done correctly, you will
    get a big warp. As I understand it, the key is to making sure that all the boards
    are evenly, and thoroughly heated when they are in the press. Success, or failure,
    is entirely in the hands of your board manufacturer.

    -Chuck
     
  10. Tom Loredo

    Tom Loredo Guest

  11. JeffM

    JeffM Guest

  12. doppan

    doppan Guest

    I normally include a Layer Stack-up legend that gives all the
    information about the board (Copper Thickness, Core Thickness, Prepreg
    thickness, Solder Mask thickness, etc).

    --D
     
  13. The items that define the board, such as number of layers, number and color
    of silkscreen layers, type of soldermask, etc., you will have to specify.

    But the Quality stuff you should not have to make up yourself, nor should
    you have to write it all out explicitly. It's all been worked out before.
    Just write "Boards to be fabricated to meet IPC-A-600G Class 2" or whichever
    class is appropriate for your situation.

    (See www.ipc.org . The web site is so hopeless that I can't give a sensible
    link to the standard itself, you will have to browse or search for it. A
    printed copy will set you back about $90.)
     
  14. Mathew's comments are good.
    Regarding the IPC-A-600G spec though I would have a
    suggestion. Do not list the revision of IPC specs, just use
    "IPC-A-600", then have a statement in your notes that states to
    "...use the latest revision of all IPC specifications."

    Down the road when IPC specs are revised, your notes are not
    outdated and any IPC spec improvements will be automatically
    incorporated on your behalf.
     
  15. GMM50

    GMM50 Guest



    Here's what I've come up with.
    -------
    Notes:
    1.) PCB material: (put your material here I'm using FR4)
    2.) Fabricate board in accordance with IPC-6012 (latest Revision)
    Performance class 2. Board acceptability per IPC-A-600 (latest
    revisi0n)
    3.) Unless other wise specified tolerance - +/- 0.005"
    4.) HASL finished pads.
    5.) (Specify the solder mask here)
    6.) (specify the silkscreen here)
    7.) Boards will be 100% electrically tested.

    ---------
    I ordered a copy of IPC-A-600 and all the requirements I'm interest in
    are contained in that documents.


    Thanks to all who add their 2 cents on this one.

    George
     
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

-