Connect with us

4 layer PCB (from 2 layer) + array of designs on one board

Discussion in 'Electronic Basics' started by Vitaliy, Dec 25, 2006.

Scroll to continue with content
  1. Vitaliy

    Vitaliy Guest

    Hello,

    My appplication is light detection -> using photodiodes and
    transimpedeance amplifier (OPA657 from Texas Instruments). At this
    point I have 2-layer working design. I need to increase the bandwidth
    of the detector (from 10MHz to 40MHz) and try to reduce noise (also
    reducing noise is always welcome, of course). I'm thinking about using
    two inner layers for +5V and -5V power layers (I'm using free space on
    top and bottom layers for ground layer). +-5V is currently connected to
    the board from external power supply by soldering two wires (one for
    +5V and one for -5V). I am using +-5V to bias photodiodes and to power
    the opamp. The software I'm using is OrCAD. Even if going to 4 layer
    from two wouldn't give me a significant improvement in terms of
    reducing the noise level, I would like to know the answers for the
    following questions.

    1) Will traferring +-5V to separate layers (rather than just have the
    power traces with filters) work? Since the inner layer is most likely
    to be .5oz copper as opposed to 1oz copper of outer layers. There is no
    way to specify that in gerber file, right? Will creating a power layer
    give me more stable voltage (and high capacitance)? That's why people
    are using multilayers as opposed to two layers, right? I guess I will
    still need some decoupling capacitors at the vias.


    2) The price differential between 2 and 4 layer boards is quite steep,
    and I can easily fit a few prototype boards on one board and then cut
    them (or have it cut by manufacturer). What is the easiest way to place
    array of differemt designs on one board? I only have access to OrCAD,
    but it can generate gerber files, so maybe some other software can be
    used. Are the manufacturers ok with this? I would prefer them to cut
    the boards, if possible, since I probably wouldn't be able to do it as
    well without special equipment. (Something tells me they woudn't be
    willing to make x by x board, and then cut it in y pieces, but just
    checking). I do realize I might be able to place three designs side by
    side and not require any cutting, but that might not always work for
    me.

    Merry Christmas,
    Vitaliy
     
  2. Jamie

    Jamie Guest

    single sided Ceramic daughter board for the OP-AMP and INPUT?
    Also a hole in the board so that the chip is suspended via the
    rails and output legs only also may help. I did something like that
    years ago to remove the cap around the structure.
     
  3. Vitaliy

    Vitaliy Guest

    All components are smt (except for photodiodes). I also have the
    components (resistors and capacitors) placed on both bottom and top
    layers (2 layer board), with opamp being on the top layer. Top and
    bottom are just relative terms in my case.


    Vitaliy
     
  4. Gerber files only specify the copper patterns that are to appear on
    the board. Any other construction details, including copper weight,
    and the order of layers on a multi-layer board, must be specified
    separately. I have a standard format for a text file that includes
    such information.

    When laying out a multi-layer board, you should put a wide track at
    the edges of the board on the power or ground plane layers to keep the
    copper on those layers away from the edge of the board. (Anything you
    place on a plane layer will end up as "no copper" on the finished
    board.)
    Discuss the matter with your board shop. If I have two or more boards
    that I want built on a common panel, I'll usually produce separate
    gerbers for each board, then ask the board maker to combine them on a
    single panel. However, a co-worker places multiple boards on a panel
    himself, and sends gerbers for the full panel to the board shop.
    Either way, the board shop will separate the individual boards if
    asked. If you panelize the boards yourself, you should first ask the
    board shop what separation they want between boards - they need some
    unused space to leave room for the router bit to go between boards.
    --
    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
     
  5. The power planes on 4 layers boards are more useful for high switching
    current and high speed digital stuff. There is a good chance it may
    make little or no difference for application depending on your layout.
    4 layers will give you greater ability to achieve a lower noise layout,
    but if you don't know exactly how to achieve this then it's not going
    to help you much, it could even make things worse, I have seen that
    happen before.
    Simply ask the manufacturer to do it, do waste time and effort
    yourself. Just supply them the layout for one board and tell them you
    want X number of boards. For the prototype services they will usually
    fit as many as they can on the one panel for you, you pay per panel.

    For high production designs it's usually different, you have to worry
    about panel handling and tooling hole/marks etc.
    Some manufacturers will do up to say 3 different designs on the one
    prototype panel for you, if that's what you want.

    Dave :)
     
  6. These requirements tend to be mutually exclusive... i.e., more
    bandwidth lets in more noise.

    What is the source of the "noise"? E.g. source noise, photocurrent
    shot noise, transimpedance amplifier noise, external interference?

    Until you do this it seems pointless to speculate about numbers of
    layers in boards.
     
  7. John  Larkin

    John Larkin Guest

    More layers won't necessarily improve speed or reduce noise. If you
    increase trace capacitance (from thinner dielectrics) it might make
    things worse.

    10 or even 40 MHz isn't very fast for a photodetector; I've got 180
    MHz from cheap opamps. What detector device are you using? Increasing
    the photodiode back-bias should help speed a bunch, maybe 2:1 if you
    go from 5 volts to something like 20.

    What's the application? How much noise do you see, in equivalent
    optical power?

    John
     
  8. Vitaliy

    Vitaliy Guest

    Gerber files only specify the copper patterns that are to appear on
    I think I'm missing something: should I leave some space between the
    edge of the board and power plane (which will be internal plane)?

    OK, I will look into panelizing the boards myself (also I would like to
    panelize different designs (same # of layers though) on the same
    board). If you can suggest a program that can take two gerber files and
    create one board will be great (I'll check if this can be done in
    OrCAD).


    PS. I will respond to other suggestions a bit later on today.

    Thanks a lot,
    Vitaliy
     
  9. Yes. If you let the copper on the planes extend to (and beyond) the
    edge of the board, you may get short circuits between planes or
    between a plane and a metal card guide.
    I use Protel, which does allow cutting-and-pasting from one board
    design to another, or within a board design. When I make a panel,
    I'll finish all the board designs in individual files, then copy and
    paste them into a new blank design. In Protel, when pasting designs,
    you have to use a "Paste Special" command, and tell the program to
    permit duplicate reference designators - otherwise Protel will
    re-number components on the second and later boards.

    --
    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
     
  10. Vitaliy

    Vitaliy Guest

    The power planes on 4 layers boards are more useful for high switching
    To start off, I will read you tutorial from pcb123 and hopefully
    improve a few things in my design from that manual. I want to add the
    power layers to reduce the length of power traces (I might need to add
    the 2nd stage to the detector, and that will definitely require
    more/longer power traces without power layers).
    Any recommendations, I'm using pcbexpress, will try to get a hold of
    them after New Year's day, local manufacturers are charging per panel
    (but I will see if they can put a few designs on the same panel).

    What I meant was: I must increase the BW but see if there is a way to
    reduce the noise (it does not have to be less than what I have right
    now).
    I was thinking differently: if I can provide more stable voltage to
    both opamp and photodiodes, I can get less fluctuations during current
    generation and amplifications and power plane should give more stable
    voltage, right? (I can be totally wrong about this)

    I'm using InGaAs PIN (Small Area/Fiber-Optic) photodiodes, which
    according to the datasheet should be biased at 5V, wavelenth of the
    signals varies between 800nm to 1700nm. NEP of the photodiode is <0.02
    pW/sqrt(Hz) @1550nm according to the datasheet.


    Vitaliy
     
  11. vasile

    vasile Guest

    PCB stack is an invention to minimise the EMI radiation and improve the
    speed of signals talking in terms of microwave or high frequency
    propagation.
    Jumping from 2 to 4 layers will not gave you many improvements in EMI
    as long the major signals are still routed on top and bottom. The first
    stack with some performance is a 4 layer stack (counted from top to
    bottom)as PWR-signal-signal-GND and 6 layer stack
    (top-signal-PWR-GND-signal-GND-bottom or other similar versions) where
    top and bottom are mixed signal/ground planes
    Will be no noise improvement if +5 and -5V routes becomes planes, could
    be worse.
    In analogic and RF design the supply lines are usually routed radially
    from the source (supply) to destination. This not means a contiguous
    supply plane could be worst as long is in the neigborhood af quiet
    ground planes.

    best regards,
    Vasile Surducan
    senior application engineer
    National Institute R&D for Isotopic and Molecular Technologies
    Cluj-Napoca
    Romania
     
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

-