8
\$\begingroup\$

What is the best way to connect ground planes together ?

I know that ground planes are connected together at multiple locations in order to keep a low impedance GND across the whole board and provide a return path for the signals.

But, in addition to the via put very close to every decoupling capacitors,

  • I have seen layouts where a lot of vias are added with a grid pattern, with a spacing of 1/20th of the maximum wavelength on the board.

  • On other boards the vias are put along the traces (like "Placement of Vias to Connect Ground Planes").

  • I have seen the vias scattered randomely.

  • There is also combination : Vias along the lines + scattered randomely on the GND planes.

Is there noticiable differences ?

What I would like to achieve is good signal integrity, low radiation and a good power supply decoupling.

\$\endgroup\$
  • 3
    \$\begingroup\$ What exactly is your application and what frequency you are working at? \$\endgroup\$ – abdullah kahraman Dec 31 '12 at 11:18
  • \$\begingroup\$ A heating controller. It has a MCU at 70Mhz and it has to switch load at very low frequency (one transition per minute). \$\endgroup\$ – Blup1980 Dec 31 '12 at 12:12
  • \$\begingroup\$ Take a look at this question and its answers, and if it doesn't address your questions, come back and refine your question here with additional details. \$\endgroup\$ – Dave Tweed Dec 31 '12 at 13:30
  • \$\begingroup\$ It's the question I have already quoted in my question : "Placement of Vias to Connect Ground Planes". It is specific for co planar transmission lines. I am talking about general rules to connect plane together. Regardless of the application. \$\endgroup\$ – Blup1980 Jan 1 '13 at 10:52
11
\$\begingroup\$

There isn't one.

That said, there are some thing I've gathered over time. What you do with the ground planes depends heavily on what you're trying to do. You could be trying to provide low impedance paths, or you could be trying to isolate one area from another, or you could be trying to deal with EMI.

There certainly is a performance penalty for doing it wrong, but you may not really care unless you're dealing either with high frequency circuits or precision analog work. The number of fluctuating bits of the ADC reading with inputs grounded, or the spectral purity of an RF signal as measured by a spectrum analyzer will tell you how wrong you are with any design. It's generally impossible to get it 100% right (datasheet spec) unless you've a system as simple as their test circuits.

The most complicated ground connection problems have to do with RF frequencies, and with signals that are either weak or are passing through traces which are susceptible to EMI coupling in that frequency. At microwave frequencies, a centimeter is enough to make a very effective antenna and mess with things. I remember a professor of mine once told me that when he was working in the industry, they'd leave plenty of points where two grounds could be shorted together, and then an engineer would test each of them one by one to see which gave the best performance. They were working with high frequency (microwave) circuits.

Typically, there's three kinds of 'ground plane' like elements you'd be wanting to short.

  1. Real ground planes. For some reason or the other you've got many of them, and you want to connect them together. This is probably the most common occurrence of the problem in the run of the mill circuits.

  2. Ground / guard traces that are running along with signal lines which may be providing a return path, guarding a high frequency signal or one bound to/from a high impedance source or sink. This could either be to prevent signal leakage or to prevent EMI coupling.

  3. Multiple ground planes which are actually the same ground.

To begin with, you should understand that there isn't really a universal ground, and also that different grounds in the same circuit arent necessarily the same ground. A typical example you'd come across is a datasheet for an ADC that talks about analog and digital grounds. This is to make sure that the oh so noisy digital circuitry doesn't mess with the high resolution ADC you've paid extra for. Different kinds of circuits have different characteristics when it comes to their interaction with the ground. Since digital circuits are characterized by a sudden spike in current at each clock, they tend to be particularly noisy at the clock frequency, and subsequently at harmonics and sub harmonics. Bypassing capacitors are supposed to deal with this, but they rarely do a thorough enough job to get milli or microvolt resolution possible from the ADC using a relatively quieter analog ground with much less switching going on.

Similarly, power grounds tend to be noisy because loads like motors and solenoids tend to be noisy, either because of effects of commutation or things like PWM. The high currents involved and the finite ground resistance (even a chunk of copper has some resistance) means that the transients showing up on the power ground tend to be higher. Sometimes high enough to completely screw up your encoder measurements while controlling a motor for instance.

The goal, then, is to isolate these grounds best you can. That means that they dont overlap, at all. You don't put analog ground on the top and digital ground at the bottom. Everything to do with analog goes with the analog ground, and everything to do with the digital goes with the digital ground in separate areas of the pcb. When the goal is isolation, you connect the planes together at a single point. More than one point can be disasterous since it leads to current loops and hence EMI problems and unintended antennae. The point where the grounds are all shorted is usually referred to as the star ground point of the circuit and is as close as you're going to get to a circuit wide ground. Generally, these should be shorted as close and centrally as possible to a place where the two circuits interact, usually an ADC or DAC. In truely haphazard designs, you'd short them near the supply and pray for the best. This is type 1.

In type 2, you have some sort of a guard trace. If the trace is at ground, then you're probably worried about EMI and not leakage. In the case of leakage, you'd want to drive the guard at close to the signal level. In both these cases, you want the guard to be as low impedance to the source as possible. This means multiple vias dropping down to the ground plane at regular intervals, if the trace is to be grounded.

The third and somewhat less exotic variety, and really is sort of just stating the obvious. This has to do with the vias taking decoupling caps to ground or the random vias shorting top and bottom ground planes. Once you've created a star ground and isolated the different areas, you want each ground to be as uniform as possible. For example, you don't want there to be a measurable potential difference between two corners of analog ground plane. You do this by providing a low impedance path to the star ground - each pin or pad that needs to be grounded goes to the plane which provides it a straight shot to the star ground point. Having the plane has the added advantage of providing a return path under each signal trace, which avoids current loops forming which may act as antennae. In cases where the ground plane must be broken, but you need to have a return path, you would provide an alternate route through another layer. If you have multiple planes with ground in the same area (note:these must be the same ground), periodic vias can help reduce impedance slightly.

\$\endgroup\$
  • \$\begingroup\$ Thanks for the deep answer! But about your type 1: What appends to the return current of the traces that connect things on the different GND islands? The high speed return current that is usually just bellow the trace would have to leave the trace, make an extra loop using the one point connection and come back to the trace on the other side of the cut. Right? \$\endgroup\$ – Blup1980 Jan 27 '13 at 7:58
  • 1
    \$\begingroup\$ Usually, you should not have traces crossing ground islands. If you do, you should make them cross at the single point connection, retaining the ground under them. If you have a specific instance, i can try to elaborate with example. \$\endgroup\$ – Chintalagiri Shashank Jan 27 '13 at 8:05

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.