Connect with us

OrCAD Layout - good ground

Discussion in 'CAD' started by Vitaliy, Jan 31, 2006.

Scroll to continue with content
  1. Vitaliy

    Vitaliy Guest

    Hello,
    I need to make all the unused area on PCB into ground (I have only two
    layers - top and bottom). So, there should be paths for whatever
    connections there are, and and there would be space between those paths
    and ground (layer?). Of course, some components are connected to the
    ground anyway, so they way I layed them out, they form the area which
    should be ground only (i.e. no other paths). I do not know terminology
    well, so it might sound a bit awkward.
    Thanks in advance,

    Vitaliy
     
  2. Leon

    Leon Guest

    Copper pour?

    Leon
     
  3. Chuck Harris

    Chuck Harris Guest

    Set a copper pour zone around the area you want to have the copper ground
    plane, set the button that says to use the copper pour for connectivity,
    and then set no fill zones around areas where you don't want the copper
    to leak into.

    -Chuck
     
  4. Vitaliy

    Vitaliy Guest

    Thanks,
    I will try that tonight.
     
  5. Paul Burke

    Paul Burke Guest

    And while you are about it, use extra vias (or holes, or whatever the
    CAD allows) to stitch together the fills on the two sides, wherever one
    will fit. The idea is try to make the flood fill approximate to a
    continuous ground plane, rather than a set of disconnected leaves.

    Paul Burke
     
  6. John Law

    John Law Guest

    ************************************************************


    If the PCB you are designing is going to be produced on a flow solder line

    then you should take extra care when incorporating earth or power planes.

    If your earth planes are large then you should fill them with a cross hatch
    fill and

    ensure that any via's or component holes connected to the earth plane are
    designed as

    thermal relief pads, otherwise the pads will wick and draw up solder and you
    will have

    lots of solder bulges around the pads on the soldered side of the pcb.


    John Law
     
  7. Chuck Harris

    Chuck Harris Guest

    That reminds me of something that he will have to deal with, and that is,
    left to its own devices, the autorouter will route the ground wires, in
    addition to the ground plane. This will add extra wires through the thermal
    reliefs it automatically adds to ground pads. You have to tell the router
    not to route ground.

    In the default condition, via's are covered with solder mask, so they don't
    need to be thermal releaved on the ground plane. In the default condition,
    all ground plane pins are already thermal releaved.

    A hash ground plane is a nice idea if you can afford the leakage, usually
    on my RF projects, it is not an option.

    Copper fills slow down the scrolling and refresh rate of the screen. You
    should leave the display copper fill option off, except when you specifically
    want to see copper pours.

    -Chuck
     
  8. Paul Burke

    Paul Burke Guest

    EasyPC must have a pretty good algorithm then. The fill scarcely slows
    things down, even on my increasingly- antique 800MHz system.

    I often do turn them off, but that's just because they get in the way of
    seeing where the tracks go.

    Paul Burke
     
  9. Chuck Harris

    Chuck Harris Guest

    I doubt that their algorithm is any better than Orcad's. Small boards are
    no problem. It becomes a problem when you do boards that are about one foot
    on a side.

    -Chuck
     
  10. qrk

    qrk Guest

    Orcad's V10.x release broke the copper fill display in "fast fill"
    mode. Now fast fill is extremely slow fill when zoomed in. Much faster
    to use skeleton or normal fill modes. I had a talk with a EDA rep and
    he was clueless. Orcad's new policy of doing programming in India has
    caused lots of problems in the new releases.
     
  11. Leon

    Leon Guest

    I just tried copper pour on a 1 ft square board with Pulsonix, it was
    almost instantaneous. I do have a 64-bit dual-core Athlon with 1 Gbyte
    of RAM, though.
     
  12. Joel Kolstad

    Joel Kolstad Guest

    In general I've found that the older a piece of PCB software is, the slower
    scrolling is! ...with notable exceptions for things like ORCAD 386/SDT, of
    course. Similarly, I'm actually surprised that most PCB packages still even
    have the option of drawing in "outline mode" -- I was told that came about
    primarily due to the slow speed of now-ancient computers and graphics
    terminals.
     
  13. Chuck Harris

    Chuck Harris Guest

    A good part of this performance problem is the older packages do their
    graphics with 16 bit I/O data transfers, while the newer packages use the
    most efficient block transfer methods that are available on new hardware.

    -Chuck
     
  14. Vitaliy

    Vitaliy Guest

    Thank you all for your replies.
    They board I am doing is going to be relatively small size (max 1.5''
    by 3.5'').
    I am not exactly sure what flow solder line is.
    I added copper pour.
    1. I would like to stich together the planes in the corners of the
    board, however, I ran into problem. "Free vias must attached to the
    net". For now, now mounting holes are planned. Does that mean I can not
    use free vias to stich the planes in the corner?
    Here are the qoutes from Orcad's help: "Free vias must have a net
    attachment, though they do not appear in a schematic or netlist. ...You
    can use free vias for special purposes, such as zero length fanouts of
    ball-grid array components and the "stitching" of plane layers. ..."

    2. Is it ok to use free vias under surface mountable components?

    3. When free via is created, does it mean that physically there will be
    a hole in the board, which would need to be filled up by copper?

    Thanks in advance,
    Vitaliy
     
  15. qrk

    qrk Guest

    Free vias are manually placed vias that take a little effort to
    delete, thus deleting traces to a free via will not remove the free
    via. Free vias must have a net associated with them. Double clicking
    on the free via in a routing mode will bring up a dialog box where you
    can change parameters of your free via.

    If you want to join planes in the corner of the board, you can use
    your mounting holes to do this if you don't mind connecting your
    ground plane to chassis. Simply define the holes in your schematic as
    a one-pin device and connect them to ground.

    If you want to use free vias to stitch the planes, then route out a
    ground trace from some pin and insert a free via at the end of the
    trace. Delete the trace to your free via and move it to the desired
    location. You can copy this free via and place the copies else where.
     
  16. 2) It is OK to use free via's under SMT components if you are getting
    the board manufactured at a PCB house where they plate the holes to
    connect the two sides, nice and flat. If however you are routing the
    PCB on a prototype milling machine that uses conductive glue to plug
    the vias it can leave a little 'tent' of glue which may interfere with
    placing the component flat on the PCB, likewise if you are actually
    hand-soldering the via's with wire (yes some people still do this!).

    3) Yes there will be a hole. It does not need to be 'filled' per se,
    but a PCB manufacturer will plate it with copper creating a barrel
    shape, if the diameter is big enough you will be able to look through
    it. If you are using conductive glue: fill it, hand-soldering: fill-it.

    Alan
    www.electronic-eng.com
     
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

-