Connect with us

OrCad Capture

Discussion in 'CAD' started by Vitaliy, Jan 9, 2006.

Scroll to continue with content
  1. Vitaliy

    Vitaliy Guest

    Hello,
    I am using OrCAD 10.5 full suite for my school project. I'm fairly new
    to it as well. I got stuck with the following problems:
    1) From what I read, the schematics and pcb footprint aren't exactly
    correlated. I am using Capture CIS. I could not find how to represent
    PCB footprint for OPA655 (SOIC) from TI.
    http://focus.ti.com/docs/prod/folders/print/opa655.html
    In fact, I am not sure what the PCB footprint code for any opamp is. Or
    should I use SOG.050/8/WG.something/L.something. I am not sure what 050
    in SOG represents, because there are different options (i.e. 025 as
    SOG.025), so I do not know which one to use. Also, if I were to use SOG
    and
    http://focus.ti.com/general/docs/lit/getliterature.tsp?literatureNumber=msoi002c&fileType=pdf
    is my opamp, which dimensions am I supposed to match? Chip with the
    pins or chip without the pins? Or somewhere in the middle so it is
    easier to solder.
    2) I am also supposed to use OPA657 (SOIC)
    http://focus.ti.com/docs/prod/folders/print/opa657.html. However, there
    is no electrical model for it in the libraries. So, I downloaded this
    opamp library from TI website. The model looks ugly though with some
    pins in the middle of the chip. I can move the pins around, also it
    still wouldn't look like an opamp after that. Is there a way to make it
    look like opamp, not a rectangle. As far as I understand it wouldn't
    matter for Layout.

    Thanks,
    Vitaliy
     
  2. The 050 is the pin pitch in mils, .001 inches. The 8 means it has 8
    pads for an 8 pin part. WG is the width of the gull-wing leads; be sure
    to find a foot print with a larger number here than the TI spec sheet
    shows for the maximum width of the part. L is the length of the molded
    body of the part; this really only affects the silk-screen, place
    outline, etc. of the foot print, so be sure to use foot print with the
    same or larger length than the actual part. Note that similar packages
    from different vendors can have different dimensions. Foot prints that
    have their basic dimensions specified in mm instead of inches, usually
    have an "m" in the numbers.

    You will be advised by others, and I would second that advice, to learn
    to make your own foot prints, or at least to check the Orcad supplied
    foot prints carefully against the vendors recommended layout. It is not
    that hard. Foot prints are made in the Library Manager of the Layout
    package.

    I am not sure about CaptureCIS 10.5, I use CaptureCIS 7.2, but the
    Capture package needs to know how to find the footprint libraries
    (separate from the schematic symbol libraries) in order to display the
    foot print when selecting parts from the database. This was/is done by
    creating a layout.ini file with the Layout package that contains all the
    foot print libraries you want to use, and then copying the layout.ini
    file from the Layout installation directory to the Capture installation
    directory.
    The pads in the foot print need to extend farther than the maximum
    spread of the leads.
    I am not familiar with that part, so I don't know if it has a standard
    8-pin opamp pinout, but you can use any library symbol that looks good
    to you and that contains numbered pins for every pin you want connected
    on the layout. The only information transfered from the schematic
    symbol to the layout is the pin numbering information that is used to
    create the netlist. The netlist is what transfers information about the
    schematic to Layout. It makes no difference what the name of the symbol
    is, so long as the pin numbers match the functions, AND there is a foot
    print available that matches the pin numbers to the right physical pins
    on the package (SOT-23 and TO-92 packages, amongst others, are often
    numbered in conflicting ways by various vendors, so be careful about
    this). If you don't like the look of the available symbol, and there is
    no standard available, make your own. I rarely use any Orcad supplied
    symbols, except for simple things like standard gates and op-amps.

    Note that there is other information in the netlist for each part, such
    as the name of the footprint to be loaded (but which can be overridden
    once the design is in layout), the "value" of the part, the reference
    designator, etc.

    --
    NOTE: to reply, remove all punctuation from email name field

    Ned Forrester 508-289-2226
    Applied Ocean Physics and Engineering Dept.
    Oceanographic Systems Lab http://adcp.whoi.edu/
    Woods Hole Oceanographic Institution, Woods Hole, MA 02543, USA
     
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

-