Schematic layout/design question...

Discussion in 'General Electronics Chat' started by osx-addict, Jul 4, 2012.

  1. osx-addict

    Thread Starter Member

    Feb 9, 2012
    122
    9
    Hi all.. I ran across a schematic the other day that had something I hadn't really noticed in other schematics before.. Namely that the PIC32 in the schematic was broken up into logical circuits (look for IC5 on the schematics -- there are pieces of it on the 2nd-to-4th pages.. It really makes the schematic easier to read since these PIC chips have so many overloaded pins..

    Has anyone done this sort of thing and how do you go about doing it in a program such as Eagle or Diptrace -- if it's possible? Ultimately the layout should include only 1 part -- not 3,4,5,etc.. in the PCB layout.
     
  2. JohnInTX

    Moderator

    Jun 26, 2012
    2,341
    1,024
    In EAGLE, you could create the PIC sections as gates (like a quad NAND in one package). Each 'gate' symbol would be your representation of the functional block (drawn in the symbol editor). In the device editor, bring in all of those symbolic blocks along with power and ground into the symbol window, the package into the package window and use CONNECT to hook em up.

    In use, use the ADD/INVOKE functions to get the symbolic pieces to the schematic.

    A caveat, be sure to invoke ALL of the pieces of the PIC. The DRC can help some if you leave off a section with dedicated input pins (flags unconnected input) but won't help with I/O or output pins.

    I usually drag a the big PIC to a page, hook up only the processor stuff directly (power, reset circuit, ISCP, OSC etc) then use net labels for all of the I/O to avoid mess and make it easier to check off pins as they are hooked up.

    Interesting idea... thanks for bringing it up.
     
  3. WBahn

    Moderator

    Mar 31, 2012
    17,718
    4,788
    Yes, this is done all the time. You may already have this if, when you plop down a NAND gate, you can plop down the symbol and then set an attribute to indicate which of the quad-NAND gates this particular one is a part of and also which of the four gates this particular one is.

    Different schematic capture tools have different ways of doing it. Most that support it probably also have a way to automatically package the design for you; so you just plop down your seven NAND gates and then, before starting layout, you package the design and it automatically assigns the seven NAND gates to two ICs. But watch out for this, because it probably doesn't know what to do with that eighth gate and will probably be happy just leaving all three of those pins unconnected. That's one of the many reasons why I always packaged my designs myself.
     
  4. osx-addict

    Thread Starter Member

    Feb 9, 2012
    122
    9
    Thanks guys.. I'm not actually using either Eagle or Diptrace -- but am actually using a mac specific design tool called McCad Schematic Plus but figured most would have a similar way to do this sort of thing.. After reading your comments I went back to re-read the docs and found it covered a bit in one of the chapters.. I'll give it a shot -- this seems like a great way to compartmentalize logic and to keep schematics tidy!
     
  5. osx-addict

    Thread Starter Member

    Feb 9, 2012
    122
    9
    Just a quick reply.. I did end up using Eagle after all and am getting more comfortable with it.. Last night I created two parts -- one of them was a PIC32 with different logical blocks (Power, PORTA, etc) and used the connect feature to plug the logical into the physical.. Worked like a charm.. I didn't quite finish up yet since I hadn't put in all of the logical blocks I wanted before it was bedtime (1am).. I'll finish it tonight but it looks good! Thanks all!
     
Loading...