Groundplain and Powerplain... did I cross the streams?

__red__

I have a simple two-sided board which contains a simple propeller circuit and a charlieplexed LED array.

In bottom-copper I did a copper pour for Ground.
In top-copper I did a copper pour and connected it to 3.3V.

My reasoning was that I heard that on multi-layer boards power plains were common.

The circuit functions perfectly.

Did I break a best practice? Should I have done GND on both sides?



Red

SRLM

There are no "best practices", just good practices for a particular situation. In your situation, with what appears to be a fairly low speed circuit, you're fine. Here is a good thread on these very forums: http://forums.parallax.com/showthread.php/119491-Ground-Power-plane-on-PCB-need-advice

I highly recommend the book The Circuit Designer's Companion by Peter Wilson. It covers ground planes and more. http://www.amazon.com/gp/product/0080971385/

ps: it's "plane", not "plain".

LoopyByteloose

There are advantages to having a big copper ground plane parallel to an opposing supply voltage plane, but in many cases it is not absolutely necessary. I think the big planes are better in the middle layers of a 4 layer board than in a 2 layer board. Then the outside layers are generally for high speed communications.

The main advantage for doing so in a DIY situation is you just don't have to etch as much copper off the board.. production is faster.

Even the most sophisticated motorboard designs are a product of extensive trial and error. You will often see areas that provide potential fixes for problems that don't have any components in them as the board worked well and didn't require additional fixes. Still, the designer is reluctant to remove the art work as it just might result in a board that doesn't work.

In other words, the pros know that boards are a tedious process and when you get a stable one, don't mess with what you have.

tonyp12

For basic design: Top copper pour is Volt and bottom copper pour is Ground.

But if you are doing radio or heat transfer, having Ground on both sides is good.
You can use a second smaller section pour for Volt (set to priority 0 and large snap-to-board-outline pour to 1) .

If you have both motor,digital and analog ground,
they should be kept separated with route-keep-out and meet at one spot close to main ground connection.
Digital and Analog ground should have a narrow passage between each other and also a narrow path to main ground.


See pics of my new Prop Motor and Relay Board where I do both a smaller Vcc pour (purple) and separate digital ground.

LoopyByteloose

And so, what you mention is what I have long expected. Different kinds of projects have to adapt to different design solutions in printed circuit boards. It is rather impossible to generalize and say, "Yes, you should always do this."

Duane C. Johnson

When I use a "pour" function the resultant plane is often broken up quite a bit, especially with a 2 sided board.

I often add short jumper foils on the opposite side to kind of "stitch" the planes back together.
Often the vias used with these jumpers can be used to add power plane decoupling capacitors between the planes.

Ya, "rules" can be quite vague, but good power planes rarely get one in trouble.

The exception is where power circuitry resides on the same board as sensitive analog circuits.
Keep these isolated so the high currents don't pass through plane areas near the analog stuff.

Duane

LoopyByteloose

The Propeller 2 is going to offer ADC and DAC on every i/o. So planning for isolation of the ADC and DAC regions will become more important.

tonyp12

>plane is often broken up quite a bit, especially with a 2 sided board.
>I often add short jumper foils on the opposite side to kind of "stitch"

I spend many minutes (maybe hours) to avoid this, start bunching traces up so they use less space.
May have to go a longer route to go around a ground-via to make sure this via is not an island.

Duane Degn

tonyp12 wrote: »

>plane is often broken up quite a bit, especially with a 2 sided board.
>I often add short jumper foils on the opposite side to kind of "stitch"

I spend many minutes (maybe hours) to avoid this, start bunching traces up so they use less space.
May have to go a longer route to go around a ground-via to make sure this via is not an island.

This is all very interesting to me. I've recently been using DipTrace to make some boards so I'm trying to get this all figured out.

Aren't there lots of occasions were you'd want the ground pour to "flow' between traces? For example if you have a SPI interface, wouldn't it be a good idea to have the clock line surrounded by the ground copper to reduce the crosstalk to the data lines?

I speed minutes (maybe hours) trying to get the ground copper between my other traces.

tonyp12

>flow' between traces? For example if you have a SPI interface, wouldn't it be a good idea to have the clock line surrounded by the ground copper to
Yes with high speed data, ground that don't have to be wider than the trace itself is recommended.
You can still bunch traces together like a freeway with exit ramps and let ground pour flow in between at one end on both sides of this highspeed clock trace.

Mark_T

For digital logic the two planes are equivalent - every point power is decoupled to ground is essentially a zero ohm connection (at the frequencies
of interest for decoupling). So conceptually you want to ensure the combined plane has good coverage so it can provide a low-inductance
return path for each signal trace across the board. With ground plane both sides you'd use a via, with power and ground you add a decoupling
capacitor to link them (call it an AC via!).

With two layer boards its often simpler to use ground plane only since you don't have to fiddle with extra capacitors to cope with avoiding
islands and missing areas, just route ground on whichever side you can.

With high current circuitry you may need planes for each rail just to carry the current.

Duane Degn

tonyp12 wrote: »

>flow' between traces? For example if you have a SPI interface, wouldn't it be a good idea to have the clock line surrounded by the ground copper to
Yes with high speed data, ground that don't have to be wider than the trace itself is recommended.
You can still bunch traces together like a freeway with exit ramps and let ground pour flow in between at one end on both sides of this highspeed clock trace.

Thanks Tony.

I'm often amazed at how clean yours and others boards look. I'm generally pleased just to get all the connections that need to made, made. I am finding this (routing traces) is becoming easier as I practice at it.

I still think it's pretty darn cool how easy it is to have my virtual PCBs turned into real boards using the online fab houses.

tonyp12

And also try to avoid that the power and ground have a Daisy chain look to its path, try to go for a tree look.