Star grounding Vs. Ground Pour in PCB Layout

[Veryveryfamous]

I'm in the middle of a PCB design project and I'd love to hear some thoughts on approaches to grounding. This PCB is for a synthesizer so it has some things that are more in the digital realm and draw a bit of current (gate signals and status LEDs that switch pretty quickly) and some things that are more analog (input preamps and VCAs).

To keep switching noise from the digital elements from leaking into sensitive analog areas, my strategy has been to run separate ground paths to digital and analog areas which lead back to the power supply where they connect in a star ground.

On the other hand, on many PCBs I see, there is just one big ground pour all over the board which I assume has the benefits of being a super low resistance path to ground and some sort of beneficial shielding (coupling?) affect on the other paths it runs along (approaching the benefits of a whole ground plane layer).

When does it make more sense to run individual long and skinny ground paths out do different areas in a star ground and when is it better to just combine those ground paths into the big overall ground pour?

 

[abbey road d enfer]

I'm in the middle of a PCB design project and I'd love to hear some thoughts on approaches to grounding. This PCB is for a synthesizer so it has some things that are more in the digital realm and draw a bit of current (gate signals and status LEDs that switch pretty quickly) and some things that are more analog (input preamps and VCAs).

To keep switching noise from the digital elements from leaking into sensitive analog areas, my strategy has been to run separate ground paths to digital and analog areas which lead back to the power supply where they connect in a star ground.

On the other hand, on many PCBs I see, there is just one big ground pour all over the board which I assume has the benefits of being a super low resistance path to ground and some sort of beneficial shielding (coupling?) affect on the other paths it runs along (approaching the benefits of a whole ground plane layer).

When does it make more sense to run individual long and skinny ground paths out do different areas in a star ground and when is it better to just combine those ground paths into the big overall ground pour?

What makes sense is keeping separate paths and managing the contours of the copper pours so the different "grounds" don't mix. This is how you take advantage of the lower resistance AND keeps the various "grounds" separate.

 

[Rochey]

Henry Ott. Go read articles by him. He talks about sensible partitioning on the board, so that large high speed return currents do pass or go near sensitive analog circuitry.

Thats the one thing I always think about when I'm laying out boards. What path does high speed return currents take to go back to the PSU.

 

[JohnRoberts]

I'm in the middle of a PCB design project and I'd love to hear some thoughts on approaches to grounding. This PCB is for a synthesizer so it has some things that are more in the digital realm and draw a bit of current (gate signals and status LEDs that switch pretty quickly) and some things that are more analog (input preamps and VCAs).

To keep switching noise from the digital elements from leaking into sensitive analog areas, my strategy has been to run separate ground paths to digital and analog areas which lead back to the power supply where they connect in a star ground.

On the other hand, on many PCBs I see, there is just one big ground pour all over the board which I assume has the benefits of being a super low resistance path to ground and some sort of beneficial shielding (coupling?) affect on the other paths it runs along (approaching the benefits of a whole ground plane layer).

When does it make more sense to run individual long and skinny ground paths out do different areas in a star ground and when is it better to just combine those ground paths into the big overall ground pour?

Circuit board "design" is an extension of circuit design since PCB traces have impedance and there can be consequences from co-mingling signal currents.

How fat and how direct depends on the signal that ground lead is carrying.

Simple ground strategies can lead to poor results.

JR

 

[Veryveryfamous]

Many thanks for these suggestions!

Abbey road - that does seem like a good idea doesn't it. I guess I've been holding off because adding the ground pour seems to create many 'loops' in the ground traces within these partitioned areas. I know the term ground loop refers to currents and not copper but it somehow seems like the ground pours and star grounding are opposed in this respect - perhaps I'm mistaken?

Rochey - Henry Ott indeed! His book Electromagnetic Compatibility Engineering looks like just what I've been looking for, some seriously heavy stuff (and thank god I'm not interested in much above 20Khz). I was hoping to find grounding theory and PCB layout guidelines in Douglas Self's small signal audio book but it seems like this might be just what I was missing. Does anyone else have other books or papers they draw on for PCB layout questions?

 

[Rochey]

his articles are free

 

[abbey road d enfer]

Many thanks for these suggestions!

Abbey road - that does seem like a good idea doesn't it. I guess I've been holding off because adding the ground pour seems to create many 'loops' in the ground traces within these partitioned areas. I know the term ground loop refers to currents and not copper but it somehow seems like the ground pours and star grounding are opposed in this respect - perhaps I'm mistaken?

Indeed, indiscriminate copper pour is the enemy of hierarchical ground. You start with hierarchical ground (gound follows signal) and create the polygons in accordance.

 

[warpie]

Does it make sense to use two separate ground planes ? For example, top layer ground plane for analogue signal and bottom layer ground plane for digital stuff. Then connect these two ground planes at the PS?

 

[JohnRoberts]

Avoid the temptation to reduce PCB design to simple rules.  While I am not arguing that this is overly complex.  PCB layout is not some mysterious dark science...

It all comes into sharp focus after a given prototype board introduces unwanted noise.

Experience helps us anticipate problems by remembering all our old mistakes we've made over the years. Think of current flowing in pipes..  big current needs bigger pipes, keep the clean water separate from the sewage.  ;D ;D

JR.

 

[Chris_V]

It really depends on the pcb you are designing, and the numbers of layers.
With a 4 layer PCB and up, you don't even think, you use one layer or more as plain ground planes and make shortest connections with vias to the ground plane(s). In very specific cases you can separate grounds, but it is less and less true with modern electronics (I have never done that for years in mixed signal boards)
With a single layer PCB, ground pours are not good ground planes (lots of loops, slits, split) so you have to be carefull with your layout, trying to isolate and visualize digital and analog path.
With a two layer PCB, it is the same, but you can potentially have two "not so good ground planes", and if you connect them together in several optimal points with vias, it can be "not so bad" ;-)

 

[Dan Mills]

These days my starting point is pretty much 4 layers unless it is something utterly trivial.

I favor a nice solid plane to minimize loop areas with intelligent placement to keep the digital stuff away from the analogue and with single ended references being taken down to the plane at carefully considered points.

Series resistors in the digital control lines really help to keep the edge rates low (You do not need ns edge rates on something like a pad relay control line).

Differential pairs are your friends for both analogue and any required fast digital, and impedance balanced is still quite acceptable for this.

Remember that return current will tend to flow in the plane directly under the signal track, more so if the plane to signal layer spacing is small, and more so as the frequency rises.

Now there are places where a judicious slit in a plane or even full up star earthing makes sense, but IME you are far more likely to get a usable result first time starting with a plane and concentrating on placement and what the loops are then you are starting with a spiders web  of star earthing, except possibly for power stages where large currents are involved. 

One really key thing to recognize is that the output current loop is probably NOT what you think it is, consider an opamp, the output loop is opamp -> load -> return -> opamp supply pin (Which one depends on what the opamp is doing), this typically involves the decoupling caps at least as much as it does the main power supply, opamps are 5 terminal devices, not 3 terminal ones. 

Now mostly I do mixed signal rather then pure analogue, so maybe the star thing makes more sense if you only have DC - 20K on the board,  but who really does these days?

Regards, Dan.

 

[Matador]

Now there are places where a judicious slit in a plane or even full up star earthing makes sense, but IME you are far more likely to get a usable result first time starting with a plane and concentrating on placement and what the loops are then you are starting with a spiders web  of star earthing, except possibly for power stages where large currents are involved. 

This has been my experience as well:  you can get 90% of where you need to be for most pre-amp designs (not involving 100's of mA of circulating currents) by minimizing ground impedance, and simply keeping 'clean' and 'dirty' grounds separate except at a single bridge point.  In other words, decoupling caps get dumped to a 'dirty' ground (I use the digital ground net in Eagle, or 'DGND'), and a 'clean' ground for everything else ('GND').  I often use a 1206 resistor layout that has the pads bridged in the middle between each pad, in case I want to Dremel out the bridge and break them apart for experimentation/testing.

This often means you get a solid pour for GND, and DGND gets routed with a thick trace back to wherever the PSU connects.  This both optimizes ground impedance, and gives you a shot at a clean layout with the minimum of breaks.

But to John's point about, this is just as much of an art as a science:  you make your best (educated?) guess, and prototype, test, and tune if needed.

 

[buildafriend]

his articles are free

Thanks : )

http://www.hottconsultants.com/techtips/split-gnd-plane.html

 

[abbey road d enfer]

In other words, decoupling caps get dumped to a 'dirty' ground (I use the digital ground net in Eagle, or 'DGND'), and a 'clean' ground for everything else ('GND').

Currents dumped by decoupling caps into the "dirty ground" are the image of the current delivered to the load, right?
So, this technique of separating "ground" into dirty and clean, should also consider "dumping" the load return currents to the dirty ground, IMO.

 

[dmills]

Yep, usually the return current actually goes to the opamp decoupling caps, if you make it chase all over the board (Back to the power supply, then via a bus cap to the relevant rail) you are just creating a big loop with at least part of it carrying pulsating currents, not a good scene.

Better to just pin everything straight to the plane, but be locally smart about it, things like references for inverting buffers can be tracked alongside the signal trace to the previous stage and pinned down there for example.

Now pretty much everything I do is differential input and output so I don't deal a lot with single ended audio (Except locally on a board), so the rules may differ if doing single ended IO (Shudder!).

You will end up prototyping, but a plane is usually more likely to be at least mostly ok then star earthing without a lot of careful thought and calculation.

Regards, Dan.

 

[abbey road d enfer]

Yep, usually the return current actually goes to the opamp decoupling caps, if you make it chase all over the board (Back to the power supply, then via a bus cap to the relevant rail) you are just creating a big loop with at least part of it carrying pulsating currents, not a good scene.

I'm with you 100%; that's the reason I regard the separation of "dirty" and "clean" grounds as a poor concept, as I have always observed in equipment that had implemented this concept. Now I would keep different "grounds" (audio, digital, RF, led's, safety, electrostatic) separate and join them only if necessary and at carefully and wisely selected points.

Better to just pin everything straight to the plane, but be locally smart about it, things like references for inverting buffers can be tracked alongside the signal trace to the previous stage and pinned down there for example.

That's genuine hierarchical ground; it's an art, almost rocket science: it takes a good understanding of Ohm's and Kirchoff's laws  ;D

Now pretty much everything I do is differential input and output so I don't deal a lot with single ended audio (Except locally on a board), so the rules may differ if doing single ended IO (Shudder!).

Agreed; that's where noise optimization and RFI/EMI protection often conflict.