Hello forum.
I see many very well made & meticulously designed PCBs used in Audio products that rely on star pointing to a ground reference. In previous years I used to think that this was 'the thing to do', because it just 'looked right'.
But is this still the moden way of thinking?
For me, ground planes negate the use of star pointing. The only time I don't use the ground plane is Kelvin points for current measurements in my high current designs.
I am an electronics engineer, but unfortunately not Audo (different kettle of fish).
I would love to hear peoples insight into this!
Cheers,
Andy
I see many very well made & meticulously designed PCBs used in Audio products that rely on star pointing to a ground reference. In previous years I used to think that this was 'the thing to do', because it just 'looked right'.
But is this still the moden way of thinking?
For me, ground planes negate the use of star pointing. The only time I don't use the ground plane is Kelvin points for current measurements in my high current designs.
I am an electronics engineer, but unfortunately not Audo (different kettle of fish).
I would love to hear peoples insight into this!
Cheers,
Andy
You have to know where the currents are going. Mixing power and control on one ground plane will now work. If part placement is done properly, for say control, then ground plane all the way.
I designed many many boards over the past 15 years and moved to ground planes for control about 10yrs ago.
I designed many many boards over the past 15 years and moved to ground planes for control about 10yrs ago.
I too have thought in the past that star ground would be good, and it would be beneficial to isolate "AGND" and "DGND". However...
...After 8 years of working with real world EMC-problems, I'd now say that contiguous ground plane is generally the best approach for the most cases. This is very important when there are high edge rates involved (digital signals, switch-mode power supplies, D-class amplifiers, to name a few), but it might improve the noise immunity of the low-frequency circuits also. The concept of edge rate is far more important than operating frequency. Plane almost never produces bad results, provided that partitioning is done even remotely correct. The correct partitioning of the PCB is much more crucial than trying to split the ground. However, splitting the ground may produce better results if the ground is poor to start with, for example a mixed-signal system on two-layer board.
I'm somewhat surprised that no-one seems to challenge the "star ground" myth. It is still surprisingly recommended approach by many datasheets. See Henry Ott's paper. At higher frequencies, it becomes impossible to isolate just about anything - even creating a effective short circuit at, say 1 GHz is very difficult. 1 nH inductance (which is inductance of just few millimeters of trace) becomes now 6.28 ohms of reactance. Quite far from the short.
I recently re-designed Tripath TA0104-based switching amplifier using multilayer board and used just one contiguous ground plane. The result was that besides the ground EMI levels dropped at best 30 dB, the amplifier is now audibly much more silent, although according the "star ground myth" it should now pick up all the noise. I'm disturbed by the fact that Tripath recommended using separate ground planes for "AGND" and "PGND". By doing so, the voltage difference (and EMI-noise level) between those two grounds will be maximized in the ground system. This created common mode noise will interfere with low-level bipolar circuits (RF will be rectified) and it causes higher noise level.
A nice thing about high-frequency currents flowing in the ground plane is that the current tends to localize just under the signal trace. This is a consequence of the energy minimization principle, since then the loop area is at minimum (minimum inductance). If the plane is broken, then the return current will be forced to divert this minimum loop area, and the inductance of the loop will be much higher. That means more radiation from the loop and the loop will become more susceptible to external fields. The last thing is important with audio. Although the circuit won't use high-frequency signals, it can be disturbed by external fields. Magnetic field pickup is reduced by small loop areas. Star ground usually means that signal loop area against the ground is quite large. By using the plane near the signal trace, the loop area is very small and thus it is very immune to external interference.
Note that this technique requires almost invariably a multilayer construction, since the distance between ground plane and signal trace must be about same than the signal trace width for the ground plane to be effective. For 1.6 mm thick PCB that would require so thick traces that routing the board all but for most simple boards would be impossible. For mechanical reasons using very thin PCB is also quite unfeasible. Top/bottom ground fill does not substitute as ground plane. It is too far from the signals to be effective as a return path for RF. It is, however, practical thing to do for balancing the copper weights of the layers, which makes it easier for PCB manufacturer.
There are probably number of specialized circuits that require star ground, but for general use, the plane is better for noise emission/immunity.
Sorry for the long babbling text, but this subject is one of my personal interests.
Regards,
Janne
...After 8 years of working with real world EMC-problems, I'd now say that contiguous ground plane is generally the best approach for the most cases. This is very important when there are high edge rates involved (digital signals, switch-mode power supplies, D-class amplifiers, to name a few), but it might improve the noise immunity of the low-frequency circuits also. The concept of edge rate is far more important than operating frequency. Plane almost never produces bad results, provided that partitioning is done even remotely correct. The correct partitioning of the PCB is much more crucial than trying to split the ground. However, splitting the ground may produce better results if the ground is poor to start with, for example a mixed-signal system on two-layer board.
I'm somewhat surprised that no-one seems to challenge the "star ground" myth. It is still surprisingly recommended approach by many datasheets. See Henry Ott's paper. At higher frequencies, it becomes impossible to isolate just about anything - even creating a effective short circuit at, say 1 GHz is very difficult. 1 nH inductance (which is inductance of just few millimeters of trace) becomes now 6.28 ohms of reactance. Quite far from the short.
I recently re-designed Tripath TA0104-based switching amplifier using multilayer board and used just one contiguous ground plane. The result was that besides the ground EMI levels dropped at best 30 dB, the amplifier is now audibly much more silent, although according the "star ground myth" it should now pick up all the noise. I'm disturbed by the fact that Tripath recommended using separate ground planes for "AGND" and "PGND". By doing so, the voltage difference (and EMI-noise level) between those two grounds will be maximized in the ground system. This created common mode noise will interfere with low-level bipolar circuits (RF will be rectified) and it causes higher noise level.
A nice thing about high-frequency currents flowing in the ground plane is that the current tends to localize just under the signal trace. This is a consequence of the energy minimization principle, since then the loop area is at minimum (minimum inductance). If the plane is broken, then the return current will be forced to divert this minimum loop area, and the inductance of the loop will be much higher. That means more radiation from the loop and the loop will become more susceptible to external fields. The last thing is important with audio. Although the circuit won't use high-frequency signals, it can be disturbed by external fields. Magnetic field pickup is reduced by small loop areas. Star ground usually means that signal loop area against the ground is quite large. By using the plane near the signal trace, the loop area is very small and thus it is very immune to external interference.
Note that this technique requires almost invariably a multilayer construction, since the distance between ground plane and signal trace must be about same than the signal trace width for the ground plane to be effective. For 1.6 mm thick PCB that would require so thick traces that routing the board all but for most simple boards would be impossible. For mechanical reasons using very thin PCB is also quite unfeasible. Top/bottom ground fill does not substitute as ground plane. It is too far from the signals to be effective as a return path for RF. It is, however, practical thing to do for balancing the copper weights of the layers, which makes it easier for PCB manufacturer.
There are probably number of specialized circuits that require star ground, but for general use, the plane is better for noise emission/immunity.
Sorry for the long babbling text, but this subject is one of my personal interests.
Regards,
Janne
Star grounds are ideal iff (if and only if!) you only have dc currents and the entire circuit is in a shielded enclosure (impervious to E and H fields). This makes star grounds really useful for battery powered LEDs but not much else.
The other related myth is that analog and digital grounds should be separated under DACs and ADCs.
But please don't talk too loudly ... I do very nicely (on a professional level) from engineers that still believe these myths.
One thing to remember though: ac currents will take the path of least impedance to complete the circuit. So component placement over a SOLID groundplane is critical to successfully busting the myth.
In some specialised cases, the dc performance of the circuit is more important than the emi performance. An example is very high current (30A-50A) switch mode power supplies, where a compromise between dc accuracy and emi performance must be made.
The other related myth is that analog and digital grounds should be separated under DACs and ADCs.
But please don't talk too loudly ... I do very nicely (on a professional level) from engineers that still believe these myths.
One thing to remember though: ac currents will take the path of least impedance to complete the circuit. So component placement over a SOLID groundplane is critical to successfully busting the myth.
In some specialised cases, the dc performance of the circuit is more important than the emi performance. An example is very high current (30A-50A) switch mode power supplies, where a compromise between dc accuracy and emi performance must be made.
Star grounding is great for preventing ground loops but only for requencies at which PCB trace inductance may be considered negligible. This may include audio op-amp circuits, class A/AB amplifiers and any linear LF circuit not involving fast switching.
However, when higher frequencies (actually rise and fall slopes) are involved, a continuous ground plane is more effective in keeping ground potential as uniform as possible. PCB tracks alone are very inductive, particularly thin ones. For example, in a fast switching class D amplifier with bad layout you can easily get 10V of inductive voltage drop spikes across a 10cm long PCB track (high speed oscilloscope is required in order to see it happen).
However, when higher frequencies (actually rise and fall slopes) are involved, a continuous ground plane is more effective in keeping ground potential as uniform as possible. PCB tracks alone are very inductive, particularly thin ones. For example, in a fast switching class D amplifier with bad layout you can easily get 10V of inductive voltage drop spikes across a 10cm long PCB track (high speed oscilloscope is required in order to see it happen).
Good stuff. My kind of thinking too.
I am lucky enough to be in the postion in my engineering role where I work (Penny & Giles Drives Tech) that because Emissions & Susceptabilty are so important to our designs (for accreditation etc) that I have a nice big chamber next to me in which I can 'play'. I can measure emissions and can zap my circuits from 100MHz up to 1G to a level up to 50V/M for susceptabilty testing.
Having this kit to hand does give one a useful insight into design layout, component choice and PCB design.
For PCB design therefore I go with:
o Single ground plane that goes as far beyond the components as possible to create an infinte plane in the middle of my PCBs (inductance of the plane increases nearer to its edge).
o Keep the plane continuous, but if unavoidable never track across splits in a plane (avoid at all costs discontinuities).
A common cause for split ground planes is designers' enthusiasm to keep analog & digital planes separate. There is a good reason for this, particularly with sensitive and wideband analog circuits, the digital currents flowing in the DGND section may be sufficient to produce enough ground noise to 'infect' the analog circuit.
The problem is avoided if the two circuit 0Vs are kept separate witha single-point connection between them, so that currents in one cannot flow in the other. Such a solution is nearly always advised by the manufactures of ADCs
- Although it is a simple enough solution by itself, it runs into problems when more than one connection is needed because of multiple ADCs on a single board (read 'star point' here) and it invariably worsens the external EMC - RF emissions and immunity - of the system, because of the dipole effect of the two 0V segments.
o Analog & digital grounds share the SAME ground plane. However group the analog & digital components separtely as if separte analog & digital gorund planes were used:
Q) So why do mixed signal ICs have separate AGND & DGND pins then if we're not going to use them???
A) Because of bond wire inductance: The principle reason for separate pins is that they allow for separation of the high level digital transient supply current from the quiet analog section. Bond wires & pinouts form an unavoidble extra inductance between the chip itself and its point of connection to the ground plane. Segregation of AGND & DGND bond wires & pins prevent 'ground bounce' across this inductance cause by delta-I's from infecting the analog section. However, this does NOT need to be maintained out into the PCB system provided that the PCB ground plane is well constructed for low inductance.
o Use of surface mount components recommended where possible due to minimal 'leg inductance', espcially for decouplers (that sould be taken stright to the ground plane).
o No tracks near the edge of the plane - maintain a ground plane edge 'keep-out'.
o Power planes (segmented & isolated where appropriate) next (in the layer construction) to & fully overlapped by a continuous ground plane:
I am lucky enough to be in the postion in my engineering role where I work (Penny & Giles Drives Tech) that because Emissions & Susceptabilty are so important to our designs (for accreditation etc) that I have a nice big chamber next to me in which I can 'play'. I can measure emissions and can zap my circuits from 100MHz up to 1G to a level up to 50V/M for susceptabilty testing.
Having this kit to hand does give one a useful insight into design layout, component choice and PCB design.
For PCB design therefore I go with:
o Single ground plane that goes as far beyond the components as possible to create an infinte plane in the middle of my PCBs (inductance of the plane increases nearer to its edge).
o Keep the plane continuous, but if unavoidable never track across splits in a plane (avoid at all costs discontinuities).
A common cause for split ground planes is designers' enthusiasm to keep analog & digital planes separate. There is a good reason for this, particularly with sensitive and wideband analog circuits, the digital currents flowing in the DGND section may be sufficient to produce enough ground noise to 'infect' the analog circuit.
The problem is avoided if the two circuit 0Vs are kept separate witha single-point connection between them, so that currents in one cannot flow in the other. Such a solution is nearly always advised by the manufactures of ADCs
- Although it is a simple enough solution by itself, it runs into problems when more than one connection is needed because of multiple ADCs on a single board (read 'star point' here) and it invariably worsens the external EMC - RF emissions and immunity - of the system, because of the dipole effect of the two 0V segments.
o Analog & digital grounds share the SAME ground plane. However group the analog & digital components separtely as if separte analog & digital gorund planes were used:
Q) So why do mixed signal ICs have separate AGND & DGND pins then if we're not going to use them???
A) Because of bond wire inductance: The principle reason for separate pins is that they allow for separation of the high level digital transient supply current from the quiet analog section. Bond wires & pinouts form an unavoidble extra inductance between the chip itself and its point of connection to the ground plane. Segregation of AGND & DGND bond wires & pins prevent 'ground bounce' across this inductance cause by delta-I's from infecting the analog section. However, this does NOT need to be maintained out into the PCB system provided that the PCB ground plane is well constructed for low inductance.
o Use of surface mount components recommended where possible due to minimal 'leg inductance', espcially for decouplers (that sould be taken stright to the ground plane).
o No tracks near the edge of the plane - maintain a ground plane edge 'keep-out'.
o Power planes (segmented & isolated where appropriate) next (in the layer construction) to & fully overlapped by a continuous ground plane:
I think there is confusion here about EMI reduction and the separation current paths.
Star grounding isn’t supposed to be an alternative to a ground plane and they both serve different functions.
In most of my mixed signal instrumentation stuff I use a combination of star grounding and ground planes / spilt ground planes - not just due to an engineering preference but because it is absolutely essential in many applications.
High current ground returns must be isolated from the ground returns of sensitive circuitry amplifying/processing low level signals otherwise the voltages induced will be amplified/processed along with the desired signals.
This applies equally for DC currents and AC currents – all pcb tracks and ground planes have finite resistance.
Cheers,
Glen
Star grounding isn’t supposed to be an alternative to a ground plane and they both serve different functions.
In most of my mixed signal instrumentation stuff I use a combination of star grounding and ground planes / spilt ground planes - not just due to an engineering preference but because it is absolutely essential in many applications.
High current ground returns must be isolated from the ground returns of sensitive circuitry amplifying/processing low level signals otherwise the voltages induced will be amplified/processed along with the desired signals.
This applies equally for DC currents and AC currents – all pcb tracks and ground planes have finite resistance.
Cheers,
Glen
Interesting subject.
I am not involved with pcb design, however I am professionally involved with low voltage electrical systems, their integration and the distribution wiring hardware. I'll often have DC signals running next to a CAN bus, next to a PWM actuator feed, next to the audio wiring. Experience has indicated that the most appropriate grounding scheme depends entirely upon the application... sometimes using our equivalent of 'ground plane' and sometimes star-ground.
My professional experience directly benefits my audio endeavours when it come to PSU, input, output and other internal wiring. The keys being:
1. regard impedance as king
2. remember that current flows in loops
3. choose the design based upon the application (and not upon the sentiment that one approach is universally superior to another)
4. remember that ground is actually either; a) a safety point, b) a reference point, or c) a signal return path
5. each channel needs to exhibit exactly the same characteristics if you want to optimise your system
Good luck to all,
G.
I am not involved with pcb design, however I am professionally involved with low voltage electrical systems, their integration and the distribution wiring hardware. I'll often have DC signals running next to a CAN bus, next to a PWM actuator feed, next to the audio wiring. Experience has indicated that the most appropriate grounding scheme depends entirely upon the application... sometimes using our equivalent of 'ground plane' and sometimes star-ground.
My professional experience directly benefits my audio endeavours when it come to PSU, input, output and other internal wiring. The keys being:
1. regard impedance as king
2. remember that current flows in loops
3. choose the design based upon the application (and not upon the sentiment that one approach is universally superior to another)
4. remember that ground is actually either; a) a safety point, b) a reference point, or c) a signal return path
5. each channel needs to exhibit exactly the same characteristics if you want to optimise your system
Good luck to all,
G.
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.