What is signal to ground ratio? and how important it is, with respect to connectors

[rollaite]

Hi,

What exactly is signal to ground ratio? is it just ratio between the number of signal pins to the number of ground pins of a connector? If so, do we need to consider the power pins as signal pins? How important is this ratio to consider? I mean in what applications/scenarios this ratio becomes critical?

Thank you very much in advance!

- Rollaite

 

[marce]

If it is a standard connection such as USB, VME, PCI etc the pins will be defined. If it is your own connector they its up to the engineer, the type of signals being transmitted and quite often the type of cable used to carry the signals.
A general (and historical) rule of thumb was; "sig-gnd-sig-gnd..." used when we relied on ribbon cables to carry signals. But if you use LVDS then this changes as you need to keep the diff pair signals together; "sig+/sig-/gnd/sig+/sig-/gnd..." or "sig+/sig-/sig+/sig-..."
Then you get onto power requirements and possibly connector resistance.

 

[ServoAmp]

If ground ratio does refer to the ratio of signal to ground pins in a connector. The assumption is that it refers to single ended signals like TTL or CMOS. This can be a complicated calculation. The general rule of thumb that I use is this. For interconnect between PCBs in the same chassis and common power supply. Must have a low impedance ground connection between the boards preferable with a ground plane. Use one ground per signal. Never use single ended signals to connect between circuits that do not have a common power supply and low impedance ground connection. For example you would never Run CMOS between two chassis with different power supplies.
I will attempt to explain why.
A single ended signal is one that used the ground for the return path like TTL or CMOS. RS422 is a good example of a differential signal. It does not use the ground for a return. The high input impedance of the receiver approx 4-12 K ohms breaks the ground connection between the two chassis. There are many other differential drivers and receivers. See reference below.
The problem with single ended signals is that power supply currents flow in the signal return and the signal current flow in the power supply return. This is the definition of a ground loop. Two methods of eliminating ground loops are a Star ground topology and using isolated power supplies. If you run a signal ground across the star topology it causes a ground loop.
Now to calculate the ground loop current required to cause a logic error.
The noise margins for the various logic famlies are shown below:.
Noise margin = Voh-Vih or Vil-Vol which ever is less. = 0.4volts for all but 1.8VCMOS.
If your ground connection in the signal cable has a resistance of 0.1ohms it will take 4 amps of power supply current flowing in the signal return to cause an error. This could happen if you had a Motor sharing the power with a start up current of 8 amps and a .1ohm ground resistance. Half of the moter current would flow in your signal cable causing the error. If your cable has a resistance of 1 ohm then it would only take 400milliamps of current. This could happen if enough signals of the same polarity switched at the same time. Now you see why a low impedance ground is beneficial.

For more detailed info see these two documents.
Logic Guide 2009
**broken link removed**
Advanced Bus Interface Logic Selection Guide
https://www.ti.com/litv/pdf/scyt126

HCT ACT HC AC LV-A LVT AUP LV-A AUC LVC AVC AUC AUP LVC GTLP
5V 5V 3.3-V 2.5V 1.8V 1.8V
Logic Family TTL CMOS LVTTL CMOS CMOS CMOS
Voh 2.4 4.4 2.4 2.3 1.2 1.5
Vih 2 3.5 2 1.7 1.17 1.05
Vil 0.8 1.5 0.8 0.7 0.63 0.95
Vol 0.4 0.5 0.4 0.2 0.45 0.55
noise margin high 0.40 0.90 0.40 0.60 0.03 0.45
noise margin low 0.40 1.00 0.40 0.50 0.18 0.40

 

[rollaite]

Thanks a lot Servo Amp and Marce....

Both of these were helpful. I will go through suggested documents for further reading.

 

[marce]

The ratio of grounds to signal is more important for signal integrity and EMC these days. On the subject of grounding I would strongly reccomend Henry Otts book, Electromagnetic Engineering Compatability.
I would also look here as there are a lot of articles referecing grounding schemes, by Keith Armstrong and others.
EMCIA - EMC Industry Association, Products and Members
EMC Information Centre - The EMC Journal (Free in the UK)

Some points I'd like to discuss:
Resistance is not as important as inductance for todays digital signals, it is the inductance elemnt of the overall track/cable impedance that is the dominating factor.
I do not like the term star ground, historicly the term is star point for any grounds and refers to a single point where various "grounds" can be connected. This has led to some very complex grounding schemes to be proposed that do not cater for an understanding of what is the cause of problems such as ground loops and how signals couple.
The following presentation by Tony Waldron is a good starting point:
Designing for Interference-free Audio System Components
A Practical Interference Free Audio System (Part 2)
A good link to how signals and the return path couple:
http://www.x2y.com/filters/TechDay0...log_Designs_Demand_GoodPCBLayouts _JohnWu.pdf
I'd also reccomend Ralf Morrisons book, "The fields of Electronics"
Standard Links:
beTheSignal.com
Tech Tips
**broken link removed**
Speeding Edge consultants specialize in high-speed PCB and system design disciplines
**broken link removed**
**broken link removed**
Slightly off topic, but still relevant:
http://focus.ti.com/lit/ml/slyp167/slyp167.pdf
Basics:
**broken link removed**

Generaly if you are driving a signal through a connector and a cable you would use some sort of driver IC designed for the job, you would also never carry high current signals (driving a motor) using the same grounds as low level signals, I would also look round connector manufacturers sitse such as Smatec. Here is a link to their Technical Documentation library, an excellent source of answers to many questions regarding interconnects:
Samtec | Technical Library

Some basics on differential signaling, not as simple and clear cut as it first seems, they are also quite complex in their relationship to ground (return current paths) and while adding noise immunity their routing and cabling requirements are more complex than single ended signals.
http://www.ultracad.com/articles/differentialsignals.pdf
http://www.cdnusers.org/community/allegro/Resources/resources_pcbsi/si/tp_insidediffsignals.pdf
**broken link removed**
**broken link removed**

Basicly grounds (return current paths) are one of the more interesting aspects of PCB design and cabling, its been a hobby of mine for 25 years studying grounds, and over the years their have been some interesting changes as instruments have improved and signal speeds have gone up. It is still one of the areas more bogged down by myths and personal viewpoints than any other aspect of electronics. There are still engineers today who demand seperate analogue and digital grounds on mixed signal boards with convertors!!!
Have fun
Marc

---------- Post added at 08:01 ---------- Previous post was at 07:58 ----------

Oh differential signals do couple to a ground plane if present, thier net effect is zero though as the opposite nature of their signals means the fields negate each other, that is if they (the signals) are routed in close proximity.