Connect with us

Help designing custom footprint in Orcad Layout 9.2

Discussion in 'Electronic Design' started by Will, Feb 11, 2004.

Scroll to continue with content
  1. Will

    Will Guest

    Ok, I'm pretty familiar with Layout so far and most of the parts I've
    been using that didn't fit a standard footprint I've managed to kludge
    together something that worked but I have a part that just will not
    seem to work. The part is a 2SD2457 silicon NPN transistor from
    Panasonic (got the datasheet from Digikey) and it has what Panasonic
    calls a MiniP3-F1 package. Sort of looks like some of the voltage
    regulators I've worked with in the past. Three legs across the bottom
    of the chip with the middle leg blossoming out into a big fat pad
    underneath the chip and sticking out slightly from the top of the
    ceramic. So how the heck do I make the middle pad in Layout? It's
    not a rectangle, and I'd rather not use my old trick of making two
    pads and linking them together in the schematic. I tried making a
    copper pour on the top layer of the board (it's a surface mount part)
    and that mostly works, but the soldermask layer doesn't like copper
    pours so I can't get it to mask that part off. How do I make
    non-recatangular/non-oval/non-circular shaped padstacks that are also
    masked in the top solder mask layer? Thanks for any help!!!
    -Will
     
  2. Look at how the SOT-89 package is handled in the library. I think it's
    a set of rounded-corner rectangle "copper area" obstacles on all
    relevant layers, attached to an ordinary rectangular SMT padstack.

    Best regards,
    Spehro Pefhany
     
  3. Paul S

    Paul S Guest

    Create the weird pin as a simple pad shape that fits within the weird
    shape. Then, create a copper area for the weird shape. In the
    properties for the copper area, you can specify a pin attachment for
    it.

    Paul
     
  4. He also needs to create similar shapes on the top mask and solder
    paste layers.

    Best regards,
    Spehro Pefhany
     
  5. Boris Mohar

    Boris Mohar Guest


    Make the middle pad out of three overlapping pads. One skinny rectangle,
    one square rotated by 45° and one large rectangle. Give them all same pin
    number and hope that Layabout does not moan to much.

    I do not use Layout so I do not know will it take multiple pins with same
    number.



    Regards,

    Boris Mohar

    Got Knock? - see:
    Viatrack Printed Circuit Designs http://www3.sympatico.ca/borism/
     
  6. qrk

    qrk Guest

    If you need to make an irregular pad (regular = circular or
    rectangular) to do the following:

    1. Place a pin in the center of your pad-to-be. In your case, I would
    make the middle pin just like your outer pins and place it as if the
    tab didn't exist.

    2. To make up the rest of the pad, you need to use Obstacles. Use Free
    Track or Copper Area. These obstacles need to touch your pin to make
    electrical connectivity. In your case, copper area is appropriate.

    3. Here's the clincher, you must associate the Obstacle(s) with the
    pin. Use the Pin Attachment button in the Obstacle properties. This
    will keep your DRC from reporting the obstacle touching your pin and
    trace on the top layer. In your case, you will have obstacles on the
    top, soldermask, and solderpaste layers.

    Mark
     
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

-