Shop OBEX P1 Docs P2 Docs Learn Events
Using Ground and Power Planes on 2-layer boards — Parallax Forums

Using Ground and Power Planes on 2-layer boards

Nick McClickNick McClick Posts: 1,003
edited 2010-03-14 04:19 in General Discussion
I think the consensus is it's a good idea to put a ground plane on one layer of your board. But what's the best practice on the other layer?

I've seen a few boards put a power plane, and a lot of boards only put signal traces, although I haven't seen many that put a full ground plane on both sides. What do most people do?

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Propeller Forums RSS Feed!

Gadget Gangster - Share your Electronic Projects

Comments

  • LeonLeon Posts: 7,620
    edited 2010-03-09 21:27
    You mean copper pour, rather than a ground plane, presumably. Power and ground planes really only apply to multi-layer boards.

    Copper pour on both sides of a board will help with EMC.

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    Leon Heller
    Amateur radio callsign: G1HSM
  • Nick McClickNick McClick Posts: 1,003
    edited 2010-03-09 23:44
    You're right - I mean pour.

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    Propeller Forums RSS Feed!

    Gadget Gangster - Share your Electronic Projects
  • BradCBradC Posts: 2,601
    edited 2010-03-10 02:44
    I pour top and bottom as GND usually and just use really fat VCC traces.

    I did hear once that putting GND on both sides can act as a waveguide in really high frequency circuits, but anything with a wavelength that short is beyond my skills anyway [noparse]:)[/noparse]

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    You only ever need two tools in life. If it moves and it shouldn't use Duct Tape. If it does not move and it should use WD40.
  • mctriviamctrivia Posts: 3,772
    edited 2010-03-10 04:19
    i usually pore both top and bottom as ground because there is seldom a good ground connection on any 1 layer. if there is a good ground layer on the bottom then I will pore top as power or leave it without a pore depending on if it will help or hinder cleaning the power traces.

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    24 bit LCD Breakout Board now in. $24.99 has backlight driver and touch sensitive decoder.

    If you have not already. Add yourself to the prophead map
  • LeonLeon Posts: 7,620
    edited 2010-03-10 05:57
    BradC said...
    I pour top and bottom as GND usually and just use really fat VCC traces.

    I did hear once that putting GND on both sides can act as a waveguide in really high frequency circuits, but anything with a wavelength that short is beyond my skills anyway [noparse]:)[/noparse]

    A waveguide is completely different. I think you mean stripline, which is a track with ground on the layers above and below it, which forms a transmission line. Microstrip, which just has a single ground on one side, is more commonly used.

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    Leon Heller
    Amateur radio callsign: G1HSM
  • Nick McClickNick McClick Posts: 1,003
    edited 2010-03-10 20:07
    After reading a few different articles, I've heard a few things;

    1 - The ground plane is the reference for DC, and a power plane is the reference for AC. Not sure exactly what that means, but it sounds good.

    2 - I've read in a few places that say it's a bad idea to flow a ground plane under a crystal because it can generate noise. It makes some sense, but it probably depends on how noisy your power source is.

    3 - Having a ground on one side, power on the other side creates a capacitor, although my quick calcs show it's pretty weak (something like 10pf for a 3" x 3" board on .062 FR4).

    @mctrivia - I think if you flow ground on both sides, you can run into impedance issues, although I think most of your boards have tons of vias connecting both pours.

    @Brad - yeah, this is probably more relevant at higher speeds, I'm mostly curious as to the best practices

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    Propeller Forums RSS Feed!

    Gadget Gangster - Share your Electronic Projects
  • Chris SavageChris Savage Parallax Engineering Posts: 14,406
    edited 2010-03-10 21:40
    Nick,

    Even now I still tend to call the copper pour a ground plane. =) Happens after years of conditioning. Our Engineering manager (who happens to be the PCB layout guy) is still trying to break me of it.· According to wikipedia:

    A ground plane in PCB assembly is a layer of copper that appears to most signals as an infinite ground potential. This helps reduce noise and helps ensure that all integrated circuits within a system compare different signals' voltages to the same potential.

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    Chris Savage

    Parallax Engineering
    ·
  • Phil Pilgrim (PhiPi)Phil Pilgrim (PhiPi) Posts: 23,514
    edited 2010-03-10 21:58
    Just remember, guys, that a copper pour isn't magic. If it's broken up by embedded traces, you still have to consider your current paths the same as if it were routed using traces. I often spend as much time analyzing my copper pours and moving vias as I do with the original routing. Even pours that are not broken up sometimes need to be so that heavy return currents get routed directly to the board's power connection, rather than via sensitive circuitry.

    -Phil
  • Tracy AllenTracy Allen Posts: 6,666
    edited 2010-03-11 16:59
    I'll second what Phil said. On a complex board with lots of traces on both sides, you end up with all those little islands that aren't connected to anything or a peninsula that is hanging on by a thread. But most annoying is the added possibility for short circuits when a board is soldered, especially when it is a prototype board without solder mask. The clearance around pads is only 10 or 12 mils, lots of opportunity for bridges. Does anyone do any special keep-out zone around pads?

    Some boards like the Propeller demo board run very few traces on the bottom and the entire bottom pour seems to serve as a very effective ground plane.

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    Tracy Allen
    www.emesystems.com
  • Nick McClickNick McClick Posts: 1,003
    edited 2010-03-11 18:45
    I realize why I confuse the plane and copper pour - because I haven't done any multi-layer boards. I also haven't done any high-speed designs.

    Yeah, I consider the copper pour a regular trace, and think about return flow, noise, etc. I use the 'route keepout' all the time in diptrace, and you can also do island removal in diptrace. All my boards have mask, but I've done a few barebones prototypes, and soldering is a pain when you have a copper pour. My concerns are impedance matching and noise.

    I never thought of doing a keepout around the pads (I've only done a mask-free proto twice), but that's a great idea. FR-4 isn't as 'hydrophobic' as mask, but it's a heck of a lot better than HASL!

    I think unconnected islands are better than having nothing, although I usually remove them for aesthetic reasons.

    Is it fair to say there's not usually a problem running a power pour on one side, and a ground pour on the other? Of course, it depends on a million things, but it sounds like the only specific side-effect is slight capacitance (a few pF).

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    Propeller Forums RSS Feed!

    Gadget Gangster - Share your Electronic Projects
  • LeonLeon Posts: 7,620
    edited 2010-03-11 21:12
    Unconnected copper areas can act as antennas and re-radiate signals. They should be removed.

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    Leon Heller
    Amateur radio callsign: G1HSM
  • Phil Pilgrim (PhiPi)Phil Pilgrim (PhiPi) Posts: 23,514
    edited 2010-03-11 21:13
    Nick McClick said...
    I think unconnected islands are better than having nothing...
    Actually, they're worse than nothing, since they're able to capacitively couple traces that are not otherwise adjacent.

    -Phil
  • mctriviamctrivia Posts: 3,772
    edited 2010-03-12 05:42
    ground pour on both sides is not a bad thing. but yes impedance and creating good grounding is why there is a million vias on my 2 layer board designs. I love 4 layer designs because you can have a solid ground and power plane. makes emi considerations almost non existent if you run power on bottom(4), and ground in the middle(2), leaving low frequency signals to top(1) and high frequency to middle(3). To bad prototype runs are so expensive I have not had the privileged of spinning 1 yet.

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    24 bit LCD Breakout Board now in. $24.99 has backlight driver and touch sensitive decoder.

    If you have not already. Add yourself to the prophead map
  • LeonLeon Posts: 7,620
    edited 2010-03-12 11:48
    4-layer prototype boards aren't expensive, they are about 2.5 x the price of 2-layer from my usual supplier.

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    Leon Heller
    Amateur radio callsign: G1HSM
  • Cluso99Cluso99 Posts: 18,069
    edited 2010-03-14 04:19
    Nick: As others have mentioned, it is not just a simple pour of a ground or power plane. It has to be understood what you are doing.

    I pour my designs in sections after all power and ground traces connect. That way I have ensured that the connections are as I required. I actually place the prop power and ground plane before anything else as this is critical for overclocking, which BTW means it is also required for normal operation. Unfortunately, it is something that has been learned from years of laying pcbs and testing in the emi labs (because they have all sorts of test equipment available including spectrum analysers).

    ▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
    Links to other interesting threads:

    · Home of the MultiBladeProps: TriBlade,·RamBlade,·SixBlade, website
    · Single Board Computer:·3 Propeller ICs·and a·TriBladeProp board (ZiCog Z80 Emulator)
    · Prop Tools under Development or Completed (Index)
    · Emulators: CPUs Z80 etc; Micros Altair etc;· Terminals·VT100 etc; (Index) ZiCog (Z80) , MoCog (6809)·
    · Prop OS: SphinxOS·, PropDos , PropCmd··· Search the Propeller forums·(uses advanced Google search)
    My cruising website is: ·www.bluemagic.biz·· MultiBlade Props: www.cluso.bluemagic.biz
Sign In or Register to comment.