2

I have a two layer PCB. The bottom layer is mostly ground tracks and some signal tracks. The top layer is signal tracks and power tracks.

I want to pour copper ground since it helps noise issues and is free as far as I learned and for the sake of learning.

But some questions bother me from what I asked yesterday (Some questions from a first PCB design attempt) and I couldn't find any answer on net.

Here are my questions:

  1. Which layer should I pour copper? And if this "copper pour" is on the other layer it will be connected to ground of the circuit by a via, right? And if copper pour is at the same layer it will be connected by a track? I mean at which particular point and how will the copper pour and the circuit ground will be connected? I'm totally confused.

  2. This is a confusion between the "copper pour ground" and the "ground plane". I already have many ground tracks on one layer of the PCB. Ground pour has nothing to do with decreasing the ground tracks and making PCB manufacturing faster right? By using copper pour the ground tracks will remain the same? But by using "ground plane" instead we avoid using ground tracks and connect the ground pads directly to the ground plane by vias. Is that true and does that make the manufacturing faster?

Community
  • 1
floppy380
  • 1,715
  • 7
  • 33
  • 67
  • 2
    AFAIK you've never stated how you are going to manufacture your boards. I send all my boards to china, they don't care if you have a ground plane or if you've drawn a horse. – pipe Mar 19 '17 at 17:22
  • at which layer should the cooper pour be used? and how will the copper pour be connected to the circuit ground(at which point and how)? still no one answered these questions. – floppy380 Mar 19 '17 at 17:31
  • Floating "pour" is also a trash-spreader. If delicate signals are on the other side, or merely along-side (same layer), tie the Pour to GND. – analogsystemsrf Mar 19 '17 at 23:05
  • ok so floating pour is no good. so bottom layer i have mostly ground tracks. and i will pour copper to this layer. but does it matter at which point i tie the pour to ground tracks? and how is that done i mean tying the pour to a ground track? – floppy380 Mar 20 '17 at 00:52
  • You need to check your pcb software manual. I'm sure it covers the subject somewhere. They differ from package to package. – Trevor_G Mar 20 '17 at 02:17

2 Answers2

5

Manufacturing a board, from the customers point of view, is no different no matter what you draw, unless you add excessive numbers of holes to the board. It is much more involved to make a 4 or 6 layer board than a 2 layer board, and the cost and time will be greater. Multilayer boards allow a ground plane and power planes to be used. Once you settle the manufacturing (number of layers, layer stackup, minimum space and trace width, maximum hole density, 'via' technology and minimum size, minimum annular ring, etc.) the cost will not vary much.

Assuming you have a two layer PCB you don't really have the option in most cases of a complete ground plane, because otherwise you would have to lay out your circuit as a single layer (excepting only ground). So your options are pouring or not pouring.

If all or most of your parts are on the 'top', you can often pour a ground on the bottom that is mostly integral. If you care about EMI it's better not to have high speed signals crossing a break in the ground pour or ground plane (you can split planes). You may also choose to pour on the top (where the parts are). In circuits where there is mostly one ground and one supply, it may make sense to pour a ground on the bottom and a supply on top. The benefits of the latter in particular are not so great so you may want to make sure you leave a generous clearance so the yield is not unduly adversely affected. In other words, if the PCB maker says they can do 6 mil clearance, use 15 or 20 mils for the pour clearance, not 6 mils.

The distinction between a 'plane' and a 'pour' on a multilayer (4 or more layers) board is partly the way they are drawn- a plane is drawn in the negative and you may split it (for example to provide a second ground for galvanically isolated parts) whereas a pour is put overtop of conventionally (positive) drawn traces and pads and connected to a net. Either can provide connectivity, so you can eliminate any traces that were there providing connectivity. If you neglect removing those traces you can muck up the thermal reliefs a bit but it should still work.

Either eliminate dead copper (unconnected islands) in the pours or stitch it to connected sections with vias and short traces. In this way you can get a mostly integral ground layer and improve the power distribution at no additional cost.

Spehro Pefhany
  • 376,485
  • 21
  • 320
  • 842
  • regarding copper pouring you wrote: "it may make sense to pour a ground on the bottom and a supply on top" Trevor says copper pour is isolated from ground and Vcc. If I pour copper on bottom layer it will not be connected to circuit ground right? And what is "pouring supply"? Is that also an isolated copper pour on the top? And why is that called different name? We are exactly at the point what Im confused about now. – floppy380 Mar 19 '17 at 17:48
  • **You** have the option to connect a pour to whatever net you like. It would likely be beneficial in your case to connect the pour on the bottom layer to ground and to use it for connectivity. A floating pour would not be beneficial in most cases and it could cause problems. – Spehro Pefhany Mar 19 '17 at 17:51
  • What I mean by pouring a supply is to put a pour on the top and connect it (say) to Vcc (if that's the supply that goes to the most points or is most important). That way you get lower impedance distribution of Vcc and the capacitance from top to bottom layers helps. – Spehro Pefhany Mar 19 '17 at 17:56
2

Neither method makes any difference to manufacturing time. Copper is deposited and etched at the same time across the entire board surface. It makes no difference how much area is added or left.

Copper pour per-se is an isolated copper plate. This is not really a good idea since it buys you little benefit. A ground plane improves noise immunity and gives you much greater grounding uniformity. However, it also adds some capacitance to signal traces which can be a problem for high frequency signals.

In most cases use a ground plane. Ground connections from components should be made directly to the plane via relieved pads to make soldering easier.

On a two sided board, Which side you put it on will depend on which side gives you the most "uniform" plane. That is, if the backside has few signals, use that, and vica-versa.

Note 1: It is sometimes necessary to add vias and traces on the other side to reconnect "islands" in the ground plane or to break over large gaps or loops.

Note 2: Copper-pour simply means fill all the blank area with copper... It's not connected to anything unless you specifically add connections. A power plane is like a copper pour, but your PCB layout software knows to connect things to it automatically. How your particular software handles that you need to check and or do some tests.

Trevor_G
  • 46,364
  • 8
  • 68
  • 151
  • Oh so you mean if I use copper pour it should not be connected to the circuit ground? which layer should the cooper pour be used? and how will the copper pour be connected to the circuit ground(at which point and how)? still no one answered these questions. – – floppy380 Mar 19 '17 at 17:33
  • Copper-pour simply means fill all the blank area with copper... It's not connected to anything unless you specifically add connections. A power plane is like a copper pour, but your PCB layout software knows to connect things to it automatically. How your particular software handles that you need to check and or do some tests. – Trevor_G Mar 19 '17 at 17:35