A question about PCB design and star grounding.

[Ice-9]

I've been doing some PCB work lately which has all my components mounted on the pcb , ie effect and all jacks switches and pots.  These have all been signle sided boards and i have used a copper pour as the ground pane. I also have a schematic and pcb layout of my old Fender super 60 amp which has all the grounds running back seperately to a single point on the pcb (star ground)

My concern is does using a copper pour to connect the ground net run the possibility of generating problems such as hum and other noise ?

[alanlan]

I would use a ground fill but ensure that you also have effectively a star ground i.e. all stages of the circuit having a path straight to the ground connection/decoupling cap through the fill (if that makes sense).  Another way of putting it is to create a star ground and then fill out as much copper as possible just to get the resistance down and avoid return current paths from different circuit stages having to pass through the same narrow bit of copper.

[Ice-9]

Yes that does make sense to me, What i have been doing is to make all the routing/ tracks including the ground traces and then doing the copper pour/ fill asking the pcb cad program to connect the ground net to the fill. This is giving me maximum amount of copper in the ground fill but i can't see it as star grounding. I have no noise problems yet but i am looking at making some valve circuits and don't want to build any unnessasary problems in the layout due to the way i have been designing the PCB's

[Andi]

I tend to do a ground plane across the whole PCB (with routed PCBs it's much easier that way) but I then cit it at strategic points so that there's only one path back to the main ground "inlet" point from any given ground connection.

That's following advice I got here some years back and it's worked well.

[Ice-9]

Cheers Andi, I like the sound of that, it is keeping a maximum ground fill while keeping a star config to a large extent.
I supose its not every component in a circuit needs a seperate return to ground. I wonder what  the criteria is  for keeping certain grounds apart. Would it be each stage is best kept seperate from the next ?

[alanlan]

A full ground plane is the ideal and if you can afford multi-layer PCBs then this is the way to go, otherwise it's something to aim towards.

[R.G.]

A full ground plane is the ideal and if you can afford multi-layer PCBs then this is the way to go, otherwise it's something to aim towards.

Actually, star grounding and ground planes are for different uses. Star grounding works best at low frequencies and as you get into ultrasonic frequencies, you really start needing ground planes, although you can get by without it. As you get further into RF, ground plane becomes a necessity instead of an option, and in the higher RF - especially sharp-edged logic signals - you simply have to have constant impedance stripline traces.

Star is really better for audio, with the exception of when you have a capacitive radiation source on one side of the PCB that can be blocked by the plane. The point for audio is to keep ground return currents from polluting signal reference grounds. Star grounding is a sufficient but more than necessary way to do that; it's just easier than discovering the exact mix of non-star that's as good. With star grounding you absolutely know what currents flow on the ground returns, and can be sure that exactly zero of the return voltages from other sections flow there. In a plane, currents will follow the lowest resistance path, which tends to be a straight line, but because wide areas of copper can be as low resistance as a single straight line path, the current actually has a distribution which is humped in the straight line path and tails off in both directions away from the straight line path. The tail off is pretty fast, so you generally get away with it, and the overall resistance is quite low, so just lowering the resistance lowers the interfering ground-current-induced voltages too.

At RF, the inductance of a single trace gets significant, and at some frequency dominates the resistance. The only way to get low-voltage loss returns at RF is with low inductance techniques, including planes. Even higher, you have to go for constant impedance when a quarter wave is comparable to the length of the trace and you can get reflections and standing waves.

[Ice-9]

Thanks for all the infos. and thanks R.G. as usual a fully detailed explanation of the differences to planes and star grounding.

and in the higher RF - especially sharp-edged logic signals - you simply have to have constant impedance stripline traces.

Slightly OTT as far as audio effects are concerened, although it could be connected with DSP effects.
Would this be the reason that on computer pcb's, especilly motherboards between memory and related cpu's the multiple traces that run parallel with each other you can usually see a few traces that run off in a 'S' wavey patern. I assumed this was to keep the traces exactly the same length for logic timing issues.

[R.G.]

Actually, you were right the first time. I didn't get into equal-length paths because that tripped my Off-Topic-o-Meter.

The S curves is to equalize length. The lines are all done as constant impedance microstrip lines over an internal ground plane, and further have their lengths equalized so that the skew between an edge arriving on one line versus another line is kept down to some minimum.

In microstrip lines on PCB, the rule of thumb is that the speed of light (i.e., an EM signal) is about one nanosecond per foot. So with signals running at 500MHz and up, a full cycle is two nanoseconds. A difference of 6"/300mm is enough to delay a signal a whole quarter of the cycle. Even smaller differences can cause you to miss a critical clock edge, or worse yet miss it only sometimes. Things get sticky in PCB design these days. 

[Ice-9]

Thanks for the extra info there, i'm quite happy i was on the right track to why those traces are that way. Anyway here is a pic of one of the effect boards i have been doing recently it will give an idea of how i am linking all the grounds and adding a fill. This particular PCB is for a BSIAB2 with some modifications i wanted to add.
Any comments or feedback as to ways of improving on PCB design is welcome.

[Minion]

I notce that even with proper star grounding you can still get PSU Noise injected into the audio signal ,To overcome this keep all of you power and signal grounds seperate and use a small Value resistor (0.1ohm to 10 ohm) to connect Signal ground to PSU Ground... if there is a small ammount of resistance between Signal and PSU ground it is less likely that the noise from the PSU ground will leak into signal as it will take the path of least resistance...


Cheers

[R.G.]

I notce that even with proper star grounding you can still get PSU Noise injected into the audio signal ,To overcome this keep all of you power and signal grounds seperate and use a small Value resistor (0.1ohm to 10 ohm) to connect Signal ground to PSU Ground... if there is a small ammount of resistance between Signal and PSU ground it is less likely that the noise from the PSU ground will leak into signal as it will take the path of least resistance...

This is one of those "Mother Nature is trying to tell you something" situations.

The point of star grounding if done correctly, is that there is only one path to the place you're calling "ground" or zero volt reference for each circuit to be referenced against. If there is no circular path for electricity to follow, then there can be no signal injection.

"But wait" you say, "I've seen this happen!" Yes, it does. It does happen when the "open circuit paths" are not really open circuit. That's when your signal ground gets connected to, say, earth ground somewhere, and the power supply is causing the star point to wiggle up and down with respect to earth ground. Or when those open circuit paths are completed by parasitic capacitance or radiated magnetic field, in which case it's not really a star grounding problem but instead a noise reception problem.

True, introducing a low value resistor can cause the problem to be masked. It also is vulnerable to the low value resistor burning out on ground faults.