Hi Thorsten
So if i read correctly, digital and analog ground are tied together at pin 5?
Hi,
Maybe, maybe not, my definition of analog pin may differ from Philips. I';d have to look at the drawings at the office to be sure how I tied things up (I'll be there in a few weeks).
Just get the full transistor level circuit of the TDA1541 and it will be clear.
Ciao T
Maybe, maybe not, my definition of analog pin may differ from Philips. I';d have to look at the drawings at the office to be sure how I tied things up (I'll be there in a few weeks).
Just get the full transistor level circuit of the TDA1541 and it will be clear.
Ciao T
Hi Thorsten, just wondering if you had a chance to find the info regarding digital/analog ground planes.... thanks!
Hi,
I had a look. My latest design used an analogue groundplane on the underside of the PCB. The decoupling capacitors are SMD Film capacitors placed inside of the pins for lowest inductance.
The top of the PCB is the digital groundplane, tied together with the analogue plane at pin 4 & 5 (4 is grounded) for low connection impedance.
The power supplies are placed on the side of the of the 1541 opposite to the digital inputs, the digital inputs connect into the rest of the digital section on the other side. General digital routing is below the PCB as the top is digital ground plane, but digital supply decoupling caps are SMD 0402 and 0603 up top, so that have a really impedance link into the groundplane...
Ciao T
I had a look. My latest design used an analogue groundplane on the underside of the PCB. The decoupling capacitors are SMD Film capacitors placed inside of the pins for lowest inductance.
The top of the PCB is the digital groundplane, tied together with the analogue plane at pin 4 & 5 (4 is grounded) for low connection impedance.
The power supplies are placed on the side of the of the 1541 opposite to the digital inputs, the digital inputs connect into the rest of the digital section on the other side. General digital routing is below the PCB as the top is digital ground plane, but digital supply decoupling caps are SMD 0402 and 0603 up top, so that have a really impedance link into the groundplane...
Ciao T
Thanks Thorsten.
So...
Top --> digital gnd plane, digital decoupling caps, analog circuity, power supply circuitry
bottom --> analog gnd plane (including tda decoupling caps), digital circuitry
If this is my correct interpretation, I am surprised to see a sort-of reversal: the digital/analog gnd planes are on the opposite pcb side of their corresponding circuitry. I would have thought the ground planes surround their corresponding circuity, ie. are on the same pcb side....
So...
Top --> digital gnd plane, digital decoupling caps, analog circuity, power supply circuitry
bottom --> analog gnd plane (including tda decoupling caps), digital circuitry
If this is my correct interpretation, I am surprised to see a sort-of reversal: the digital/analog gnd planes are on the opposite pcb side of their corresponding circuitry. I would have thought the ground planes surround their corresponding circuity, ie. are on the same pcb side....
I have a few ieee papers that describes the 14bit predecessor and the dynamic element matching used but I have not been able to find any transistor level schematic of the 1541 can anybody point me in the right direction?
Hi,
Well, almost. Top has the digital IC's, the decoupling caps and the ground plane. Signal traces are via'd to the bottom. Some power "polygons" (think of them as small ground planes for the power) also end up on top, as do electrolytic caps etc, plus some routing jumpers.
Bottom just the analogue plane and DEM decoupling cap's plus the SMD cap's on the supplies.
No, the analogue ground plane is below, as the TDA1541 is through-hole, so it is no real drawback to have the analogue plane on the bottom.
All the rest of the circuitry is above, but the traces are routed below...
The object is in all cases to minimise the loop impedance for the relevant current loops.
Ciao T
Well, almost. Top has the digital IC's, the decoupling caps and the ground plane. Signal traces are via'd to the bottom. Some power "polygons" (think of them as small ground planes for the power) also end up on top, as do electrolytic caps etc, plus some routing jumpers.
Bottom just the analogue plane and DEM decoupling cap's plus the SMD cap's on the supplies.
No, the analogue ground plane is below, as the TDA1541 is through-hole, so it is no real drawback to have the analogue plane on the bottom.
All the rest of the circuitry is above, but the traces are routed below...
The object is in all cases to minimise the loop impedance for the relevant current loops.
Ciao T
Putting analogue and digital ground on top of each other is pointless and not good layout practice. The analogue and digital sections shpould be seperate areas of the board and signals from either section should not cross the other section, grounds are best left as one contigous ground, or if you insist on two grounds then ensure they do not overlap.
http://www.hottconsultants.com/techt...gnd-plane.html
http://www.elmac.co.uk/pdfs/Lord_of_the_board.pdf
An intuitive, practical approach to mixed-signal grounding
http://focus.ti.com/lit/an/sbaa052/sbaa052.pdf
http://focus.ti.com/lit/ml/slyp167/slyp167.pdf
http://www.ieee.org.uk/docs/emc1206a.pdf
http://www.icd.com.au/articles/Split...s_AN2010_6.pdf
http://www.analog.com/static/importe...0Grounding.pdf
http://www.analog.com/static/importe...als/MT-031.pdf
http://www.eetimes.com/design/autom...-practical-approach-to-mixed-signal-grounding
http://www.hottconsultants.com/techt...gnd-plane.html
http://www.elmac.co.uk/pdfs/Lord_of_the_board.pdf
An intuitive, practical approach to mixed-signal grounding
http://focus.ti.com/lit/an/sbaa052/sbaa052.pdf
http://focus.ti.com/lit/ml/slyp167/slyp167.pdf
http://www.ieee.org.uk/docs/emc1206a.pdf
http://www.icd.com.au/articles/Split...s_AN2010_6.pdf
http://www.analog.com/static/importe...0Grounding.pdf
http://www.analog.com/static/importe...als/MT-031.pdf
http://www.eetimes.com/design/autom...-practical-approach-to-mixed-signal-grounding
Hi,
You are familiar with the various challenges in circuit design, layout and routing the grounds for the TDA1541 and the internal design of the TDA1541?
And it is your considered opinion that your layout technique is better?
Be my guest.
Based on my analysis of the TDA1541 down to individual transistor level I must demur and will still do things my way...
Ciao T
You are familiar with the various challenges in circuit design, layout and routing the grounds for the TDA1541 and the internal design of the TDA1541?
And it is your considered opinion that your layout technique is better?
Be my guest.
Based on my analysis of the TDA1541 down to individual transistor level I must demur and will still do things my way...
Ciao T
If you reseach PCB design and especialy mixed signal design you will find that putting an analogue and digital ground over each other is pointless and not recommended, read the info out there, try designs and have them tested to the nth degree.
And yes my layout techniques are better than yours if you place analoge grounds over digital grounds and have signals over running over the different sections, it totaly removes the point of having seperate ground.
You want to try and read the wealth of info that is out their on PCB mixed signal design and the information regarding the use of analog and digital grounds, ALL the experts in EMC signal integrity disagree with you. Of course you may educate me and tell me why your way is better, and why you place the planes on top of each other.
You can post your layout if you want and I will provide you with a free critique.
And yes my layout techniques are better than yours if you place analoge grounds over digital grounds and have signals over running over the different sections, it totaly removes the point of having seperate ground.
You want to try and read the wealth of info that is out their on PCB mixed signal design and the information regarding the use of analog and digital grounds, ALL the experts in EMC signal integrity disagree with you. Of course you may educate me and tell me why your way is better, and why you place the planes on top of each other.
You can post your layout if you want and I will provide you with a free critique.
Hi,
However, despite all of this, these designs are not applicable directly to the TDA1541, as this a fairly unusual integrated circuit, so what applies in many places does not apply directly here..
Have you actually looked at the TDA1541 and evaluated exactly where and how signal and signal related supply currents do? And no, it does not remove the point of having separate grounds, at least not in my case.
Actually, first, what makes you think that I am unaware of this information?
Secondly, you have spoken with each and every expert in EMC signal integrity, they all know my precise design and layout and disagree that my approach is correct?
Or do you wish to say that what I am proposing appears in contradiction to what these experts recommend in "normal" circumstances?
My way is better in this specific case because of specific requirements by the specific IC central to the design and because of my specific application of this circuit.
That the planes end up on top of each other is a limit of the available geometry of this rather old DIP14 IC. More modern IC's that have smaller size and generally tend not to place directly related power and ground pins at the maximum possible distance but next to each other. They also clearly separate analogue and digital supply and ground pins, such an approach as mine would neither be necessary nor beneficial.
Thank you for your offer. The layout is not for publication.
I was merely answering questions directed to me, regarding how I did things and answered them. If you think you can do better, why do you not make a better layout then mine and publish it?
Note, my application has fully independent "floating" supplies (read there is no traditional "ground" in the design, the lookback impedance from all supplies are CCS with no ground in the classic sense) with local shunt regulators for the TDA1541 and incorporates my own design of re-clocking and I2S attenuators all of which is not for publication.
However you may use any that take your fancy from the thread of John Brown (ecdesigns). It may also be useful to review Mr Browns PCB designs.
Ciao T
However, despite all of this, these designs are not applicable directly to the TDA1541, as this a fairly unusual integrated circuit, so what applies in many places does not apply directly here..
Have you actually looked at the TDA1541 and evaluated exactly where and how signal and signal related supply currents do? And no, it does not remove the point of having separate grounds, at least not in my case.
Actually, first, what makes you think that I am unaware of this information?
Secondly, you have spoken with each and every expert in EMC signal integrity, they all know my precise design and layout and disagree that my approach is correct?
Or do you wish to say that what I am proposing appears in contradiction to what these experts recommend in "normal" circumstances?
My way is better in this specific case because of specific requirements by the specific IC central to the design and because of my specific application of this circuit.
That the planes end up on top of each other is a limit of the available geometry of this rather old DIP14 IC. More modern IC's that have smaller size and generally tend not to place directly related power and ground pins at the maximum possible distance but next to each other. They also clearly separate analogue and digital supply and ground pins, such an approach as mine would neither be necessary nor beneficial.
Thank you for your offer. The layout is not for publication.
I was merely answering questions directed to me, regarding how I did things and answered them. If you think you can do better, why do you not make a better layout then mine and publish it?
Note, my application has fully independent "floating" supplies (read there is no traditional "ground" in the design, the lookback impedance from all supplies are CCS with no ground in the classic sense) with local shunt regulators for the TDA1541 and incorporates my own design of re-clocking and I2S attenuators all of which is not for publication.
However you may use any that take your fancy from the thread of John Brown (ecdesigns). It may also be useful to review Mr Browns PCB designs.
Ciao T
Hi,
No, I set out the basic rules for the PCB design based on analysing the circuit, the actual (not assumed) behaviour of the IC's involved. I also analyse the results using a range of test equipment, including high speed, high sensitivity 'scopes (with custom designed low noise, wideband pre-pre's that allow evaluating potential differences between different points on a groundplane), an AP2 and others.
However if you prefer to tune things the way you suggest, be my guest...
Ciao T
No, I set out the basic rules for the PCB design based on analysing the circuit, the actual (not assumed) behaviour of the IC's involved. I also analyse the results using a range of test equipment, including high speed, high sensitivity 'scopes (with custom designed low noise, wideband pre-pre's that allow evaluating potential differences between different points on a groundplane), an AP2 and others.
However if you prefer to tune things the way you suggest, be my guest...
Ciao T
Hi T, I have only my ears, not an EE, no scopes etc. ECDesign's and your layout , as far as I can find them are among others my reference for my diy pcb layout, is it possible to show it to you?, most likely I've made mistakes there. I'll highly appreciate it if you could 🙂
Hi,
By all means, go for it.
I would suggest that especially this place already contains a wealth of information on the TDA1541 and it is worth reading it all. A lot of good info courtesy of HtP and others, plus loads of practice by John Brown. Some interesting snippets are about what are the actual reference points for some of the current loops are (hint, not the ground pins).
The other important thing to remember is that there is no such thing as ground. It is a convenient fiction, in reality it is a very complex combination of signal and power supply lines somehow most inconveniently lumped into one and connected to the same pin and potential...
And finally of course that currents always flow in loops and always follow the path of the least resistance, or more precisely in our case the path of least impedance (impedance comes from impeding current flow) as we deal with AC of quite high frequencies.
Almost all else will fall into place naturally from there.
Ciao T
By all means, go for it.
I would suggest that especially this place already contains a wealth of information on the TDA1541 and it is worth reading it all. A lot of good info courtesy of HtP and others, plus loads of practice by John Brown. Some interesting snippets are about what are the actual reference points for some of the current loops are (hint, not the ground pins).
The other important thing to remember is that there is no such thing as ground. It is a convenient fiction, in reality it is a very complex combination of signal and power supply lines somehow most inconveniently lumped into one and connected to the same pin and potential...
And finally of course that currents always flow in loops and always follow the path of the least resistance, or more precisely in our case the path of least impedance (impedance comes from impeding current flow) as we deal with AC of quite high frequencies.
Almost all else will fall into place naturally from there.
Ciao T
Thank you Thorsten, will pm you, I did this layout after many moons reading your posts, HtP, JB, etc. it's for my private use and for some of my friends.
Best, TeguhPS
Best, TeguhPS
ide2003.... I am currently working on a tda1541 pcb layout myself as well... I would greatly appreciate your and Thorsten's ideas out in the open (struggling here...)
thanks!
thanks!
Hi,
Sorry, I cannot really say more here than I have.
See if you can club in with ide2003, he seems ahead on the curve.
Ciao T
Sorry, I cannot really say more here than I have.
See if you can club in with ide2003, he seems ahead on the curve.
Ciao T
Still disagree, which ground are the digital signals going to couple to for their return currents etc etc. The main if not only reason for splitting the grounds is to stop digital noise apearing on the analog ground plane, and the detrimental effect this can have, having them interact both capacitivly and inductivly is not good design practice, full stop.
No I havent spoke to each and every one of the experts, but over the years I have spoke to some, having been on numerous courses regarding EMC and signal integrity, and have had my layouts reviewed by some of these peers.
I am not questioning your choice to have a seperate analog and digital ground plane I am disagreeing with them being on top of each other. I would be interested in doing a version of a TDA based layout send us a schematic and I do it for fun and free and let it be ripped apart on this forum as alot of my views on PCB design dont fit in with some views on here, such as spider legs star grounds🙂
Yes the chip hasn't got the optimum pin configeration, and I have read quite a few threads on this device, having done layouts for it many moons ago. I will as a point go and read some more that you have hinted at regarding the current reference points, curious though, how a convertor can work if it does not have a stable and equipotential reference point (this requirement for a equipotential reference point combined with both shrinking chip technology and reduced convertor voltages, is one of the factors why most current thinking is biased towards a single contigous single ground (reference plane)).
PS I do contract PCB design occasionaly, even Philips in the past, though I'll probably get no business of you now😀
No I havent spoke to each and every one of the experts, but over the years I have spoke to some, having been on numerous courses regarding EMC and signal integrity, and have had my layouts reviewed by some of these peers.
I am not questioning your choice to have a seperate analog and digital ground plane I am disagreeing with them being on top of each other. I would be interested in doing a version of a TDA based layout send us a schematic and I do it for fun and free and let it be ripped apart on this forum as alot of my views on PCB design dont fit in with some views on here, such as spider legs star grounds🙂
Yes the chip hasn't got the optimum pin configeration, and I have read quite a few threads on this device, having done layouts for it many moons ago. I will as a point go and read some more that you have hinted at regarding the current reference points, curious though, how a convertor can work if it does not have a stable and equipotential reference point (this requirement for a equipotential reference point combined with both shrinking chip technology and reduced convertor voltages, is one of the factors why most current thinking is biased towards a single contigous single ground (reference plane)).
PS I do contract PCB design occasionaly, even Philips in the past, though I'll probably get no business of you now😀
I'll go look at the ecdesign, any links please.
Agree ground is not a good term, it can cause confusion and misunderstanding.
For others looking at signal propagation please have a look at this link, it provides a visual explanation to how return currents flow>
http://www.x2y.com/filters/TechDay0...log_Designs_Demand_GoodPCBLayouts _JohnWu.pdf
Agree ground is not a good term, it can cause confusion and misunderstanding.
For others looking at signal propagation please have a look at this link, it provides a visual explanation to how return currents flow>
http://www.x2y.com/filters/TechDay0...log_Designs_Demand_GoodPCBLayouts _JohnWu.pdf
- Status
- Not open for further replies.