I'm trying to avoid the added expense of a 4 layer board, and would like some opinions on the compromise I've arrived at. My circuit uses several OP amps and some analog switch ICs, and mostly deals with medium level audio signals, around 100mV or more. There are no cases where there is any gain (all OP amps are simple unity gain buffers). So my shielding needs are light, but not completely absent. Before I get to my board layout, my develops a virtual ground consisting of an op-amp, with a voltage divider, and an output to a resistor and capacitor, like this...
So that VCC/2becomes ground for all points within the circuit that need it.
The two photos below are of 2 sides of a board whose approximate dimensions are really about 4" x 2-1/2" (no telling how they'll show up on screen). In the layouts below, even though you can't see the schematic, it should be apparent that there are a considerable number of traces on both sides of the board, running to a single large pad that shows up white. (For some reason my layout software isn't showing the hole on the bottom layer (blue) , but I'll fix that). So all those traces are going to places where an analog ground is needed, and in keeping with the rules of good OP-Amp design, they all mostly run to the same point, which is also very close to the point there that R3 and C2 (V-Gnd) meet in my first drawing.
So here's my question. I know if I really want to shield the board with such a copper pour connected to ground, it would obviously be best to make a 4 layer board, and dedicate one of the planes completely to the copper pour. But as i said, this particular circuit will mostly deal with medium level audio signals, with no gain at all. 4 layer boards are always more expensive, and so I'd like to get by with a 2 layer board. The question is, is there any shielding value in this copper pour approach at all?
An externally hosted image should be here but it was not working when we last tested it.
So that VCC/2becomes ground for all points within the circuit that need it.
The two photos below are of 2 sides of a board whose approximate dimensions are really about 4" x 2-1/2" (no telling how they'll show up on screen). In the layouts below, even though you can't see the schematic, it should be apparent that there are a considerable number of traces on both sides of the board, running to a single large pad that shows up white. (For some reason my layout software isn't showing the hole on the bottom layer (blue) , but I'll fix that). So all those traces are going to places where an analog ground is needed, and in keeping with the rules of good OP-Amp design, they all mostly run to the same point, which is also very close to the point there that R3 and C2 (V-Gnd) meet in my first drawing.
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
Now notice That pn the bottol (blue) layer, I've done a copper pour, around all of the circuitry that will have anything to do with analog signals. I want this copper pour to be at V-Gnd too, but I don't want the layout software drawing connection "spokes" willy-nilly to all available V-Gnds! So I've given that copper pour a different "net" name, so the PCB software will keep it isolated. The only connection point to that copper pour is to a single large yellow pad, right next to that first White one I described. When I know I'm done with the layout, I will bridge that V-Gnd pad to the Cooper Pour pad with a trace.
So here's my question. I know if I really want to shield the board with such a copper pour connected to ground, it would obviously be best to make a 4 layer board, and dedicate one of the planes completely to the copper pour. But as i said, this particular circuit will mostly deal with medium level audio signals, with no gain at all. 4 layer boards are always more expensive, and so I'd like to get by with a 2 layer board. The question is, is there any shielding value in this copper pour approach at all?
Last edited:
Since you're using the layer as a shield rather than as a ground plane that must conduct current, it's usable as a quasi-shield even with all the cuts.
However, the "single point ground" is a common misconception and is not the right way to lay out this board. With the numerous long traces,
the parts layout should be improved first, and then the grounding system.
Last edited:
So by "quasi shield", you do think it will have some value?
About the current flow, if I only connect the "poured" area to ground at the one point, no current should flow through any part of it. But please explain what you mean about single point ground being a common misconception. It contradicts everything I've ever learned about avoiding ground loops, so I'd certainly would like to see any papers or discussion to the contrary. Not saying i don't believe you, but I wouldn't be much a designer if I didn't approach things as a skeptic.🙂 Can you point me to any links about this?
There is some shielding value in the existing layer, but it will be inferior to a solid plane.
Single point grounding was sometimes used in simple hard wired tube amps as an improvement over multiple point chassis grounding or a ground bus wire.
In wide bandwidth circuitry, single point grounding is inadequate. Instead, study the local current flow in each stage of the circuit and minimize the loop area of each. Power supply pins must be bypassed directly to the local ground plane with minimum lead lengths. Again, component placement must be carefully optimized
to take best advantage of good layout.
Here's a good start.
http://www.ti.com/lit/ml/sloa089/sloa089.pdf
http://www.ti.com/lit/an/sloa046/sloa046.pdf
Last edited:
Ground loops on a PCB are a bit of a misnomer....once you have more than one block of circuitry you have current loops, if you create a ground loop problem on a PCB then you are really doing things wrong.
A circuit diagram and layout with component outlines would be a help as the layout looks very complex in relation to the circuit diagram.
As to shielding/ground in the above design, both sides copper pour with ground tied to the respective pins and stitching vias, ditch the silly spiders leg ground.
@Marce : Ah! putting some copper pour on the top layer too! Good idea.... But as far as the idea of single point grounding (which you're calling silly, and rayma said was an idea from some vacuum tube circuits), I'm willing to read more and learn, but everything I've found on the subject so far seems to be reinforcing what I had learned years ago. For audio frequencies, single point grounds still seems to be the recommended practice. It avoids ground loops which can cause oscillations in OP-AMP circuits, and can eliminate some sources of crosstalk too. I DO see where its not considered a good scheme for higher frequency circuits where the long runs can contribute to EMI, and add more unwanted inductance and capacitance. But since most of my analog designs are in the audio range, I think its still good practice.
But my main point is still to understand the value of copper pours to help with audio shielding, in a 2 layer board.
But my main point is still to understand the value of copper pours to help with audio shielding, in a 2 layer board.
A circuit can have wide bandwidth even with only audio signals at the input, and good practices should be followed.
Decoupling capacitors cannot function without proper layout, and device data sheets will stress this. Large loop areas
caused by attempts at single point grounding will cause problems, not prevent them.
The function of a ground or power plane is to provide low inductance connections. Shielding is primarily the function of the enclosure.
Where are you getting your info from....
Look at the guidelines for precision analogue etc from the likes of Ti, Analog Devices etc
I do PCBs for all sorts of analogue (and digital and RF) designs from the mundane (including audio) to the incredibly sensitive and they ALWAYS have a ground plane. The rather silly spider legs ground scheme (it looks like a multipole antenna physically) I have only seen promoted on DIY audio sites and guidelines, never in the professional world of electronics.
I have never heard of an on-board ground plane causing loops that will upset an op-amp, again I never do PCBs with analogue without a ground plane.
The first two text documents have some basic links, I use for generic PCB based replies, the final txt file (filelist) lists all the PDFs I have relating to PCB design in my main design directory, many of these such as slyt010b.pdf are analogue based notes or guides (some go back years). One day I am going to sort my documentation out, but I do have rather a lot of PCB, PCB layout, signal integrity etc. related documentation, many that I still refer to and the list is forever growing as new things come to light...I have to have a good knowledge of all this as I am often sent on site to design (or do it in house) and advise on layout practice, signal integrity etc. to quite bespoke customers, so my collection is broad based.
Look at the guidelines for precision analogue etc from the likes of Ti, Analog Devices etc
I do PCBs for all sorts of analogue (and digital and RF) designs from the mundane (including audio) to the incredibly sensitive and they ALWAYS have a ground plane. The rather silly spider legs ground scheme (it looks like a multipole antenna physically) I have only seen promoted on DIY audio sites and guidelines, never in the professional world of electronics.
I have never heard of an on-board ground plane causing loops that will upset an op-amp, again I never do PCBs with analogue without a ground plane.
The first two text documents have some basic links, I use for generic PCB based replies, the final txt file (filelist) lists all the PDFs I have relating to PCB design in my main design directory, many of these such as slyt010b.pdf are analogue based notes or guides (some go back years). One day I am going to sort my documentation out, but I do have rather a lot of PCB, PCB layout, signal integrity etc. related documentation, many that I still refer to and the list is forever growing as new things come to light...I have to have a good knowledge of all this as I am often sent on site to design (or do it in house) and advise on layout practice, signal integrity etc. to quite bespoke customers, so my collection is broad based.
I urge Peter Pan to pay close attention to what Marce says, he is a seasoned professional and knows what he is talking about.
Cheers, I am an old pro then🙂
Peter, don't forget you also have to cater for the abundance of electrical noise in the environment (RF). For low level audio layout follow precision analogue guidelines, when you start getting power devices then you have to look at high and low current return paths, but again I would just separate the high and low current, I don't subscribe to some that use different paths for bypass, power signal etc. and seem to overcomplicate the return paths without really understanding how and where these return currents go. That is why a dedicated ground plane is best, it provides a low impedance return route for signals at all frequencies' (low frequency like path of least resistance as the frequency increase the return path prefers the path of least impedance and will track under the signal trace closely if there is a solid ground plane.
I do tend to often have different views than many on this site regarding return paths (ground planes mainly, though power planes can also be used, the return path does not have to be ground(0V)), but my experience is not limited to DIY Audio...I am a special brew swigging old pro!!!🙂
Peter, don't forget you also have to cater for the abundance of electrical noise in the environment (RF). For low level audio layout follow precision analogue guidelines, when you start getting power devices then you have to look at high and low current return paths, but again I would just separate the high and low current, I don't subscribe to some that use different paths for bypass, power signal etc. and seem to overcomplicate the return paths without really understanding how and where these return currents go. That is why a dedicated ground plane is best, it provides a low impedance return route for signals at all frequencies' (low frequency like path of least resistance as the frequency increase the return path prefers the path of least impedance and will track under the signal trace closely if there is a solid ground plane.
I do tend to often have different views than many on this site regarding return paths (ground planes mainly, though power planes can also be used, the return path does not have to be ground(0V)), but my experience is not limited to DIY Audio...I am a special brew swigging old pro!!!🙂
@Marce I'm reading your links now. Its very possible I'm just the victim of old school teaching, and unfortunatly its been long enough that most of my text books are long gone or MIA. Probably the first reference book I ever used for audio OP amp design was a "Sams" book (remember them?) called "Audio IC OP-Amp applications". The last printing of that was like 1886. This and other books did discuss both ground loop issues, and of course recommended ground planes too when available. But I had actually experienced ground loop oscillation problems before, and this habit I got into, of bringing all grounds to a single point was one that worked for me.
So all that to say, I just ask your patience here. Single point grounding is both something I did not come up with on my own, AND something that so far has solved problems I've had, and didn't create any new ones. Of course I very much appreciate the advise of those with more experience than I that are willing to advise. Its just that In my world, a PC board is usually something that comes out of my limited budget DIY pocket, so of course there is a strong tendency to stick with what has worked for me in the past.
Now all that said, if its time to abandon that thinking I'm willing to listen. Certainly my layout in this case would be vastly simpler, even with just 2 layers, if I could simply tie all analog grounds to a copper pour via the nearest and shortest routes possible. (I assume that's what everyone is suggesting here? )
And again, I ask for your patience, and realize you're educating me is purely voluntary. I would just ask that you help me by starting with what I now understand. It would help me a great deal if we could start with some acknowledgement that the idea and philosophy of single point grounding in OP amp circuits is not something I dreamed up, and start from there. As it turns out, this particular design has only a couple of signal routing chips, a couple of OP amps and none with any gain. So it probably wouldn't matter. But it certainly won't be the last circuit I ever need to do, and since all this has come up, I don't want to miss the opportunity to learn AND understand. Ground loops are a real hassle, so I'd like to start by understanding why a ground plane deals with it better.
So all that to say, I just ask your patience here. Single point grounding is both something I did not come up with on my own, AND something that so far has solved problems I've had, and didn't create any new ones. Of course I very much appreciate the advise of those with more experience than I that are willing to advise. Its just that In my world, a PC board is usually something that comes out of my limited budget DIY pocket, so of course there is a strong tendency to stick with what has worked for me in the past.
Now all that said, if its time to abandon that thinking I'm willing to listen. Certainly my layout in this case would be vastly simpler, even with just 2 layers, if I could simply tie all analog grounds to a copper pour via the nearest and shortest routes possible. (I assume that's what everyone is suggesting here? )
And again, I ask for your patience, and realize you're educating me is purely voluntary. I would just ask that you help me by starting with what I now understand. It would help me a great deal if we could start with some acknowledgement that the idea and philosophy of single point grounding in OP amp circuits is not something I dreamed up, and start from there. As it turns out, this particular design has only a couple of signal routing chips, a couple of OP amps and none with any gain. So it probably wouldn't matter. But it certainly won't be the last circuit I ever need to do, and since all this has come up, I don't want to miss the opportunity to learn AND understand. Ground loops are a real hassle, so I'd like to start by understanding why a ground plane deals with it better.
Marce, Well of course my interest is now peaked, and just to show I'm not blowing smoke, here are some revised plots of the same PCB, in which I've pretty much removed all those long grounds. In my case I'm trying to save some money on a fairly simple low gain circuit, so I'm using a copper pour instead of a whole plane, so I can route SOME traces along with the psudo ground plane when necessary. Obviously this layout is, if nothing else, a lot easier on the eyes, and likly i could make some further tweaks...
So of course, this passes a design rules check too, because electrically its all the same to the PCB cad. (I'm using designspark PCB, by the way). But... will it be as good from an "OP-AMP' design point of view. More important, in a more complex circuit involving stages with gain, filters that like to oscillate and other circuits, will I get away with this kind of thing?
The question would be the same if I were springing for a 4 layer board, and could dedicate a whole layer to my ground plan (which in this, and other designs of mine, is usually NOT 0 volts, by the way! Its 1/2V ).
I'm inclined to give this a try. I'd just like to hear as much confirmation as I can get on this forum that I'm not going in the wrong direction, accepting a copper pour (or plane) in place of that spider web single point ground approach"
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
So of course, this passes a design rules check too, because electrically its all the same to the PCB cad. (I'm using designspark PCB, by the way). But... will it be as good from an "OP-AMP' design point of view. More important, in a more complex circuit involving stages with gain, filters that like to oscillate and other circuits, will I get away with this kind of thing?
The question would be the same if I were springing for a 4 layer board, and could dedicate a whole layer to my ground plan (which in this, and other designs of mine, is usually NOT 0 volts, by the way! Its 1/2V ).
I'm inclined to give this a try. I'd just like to hear as much confirmation as I can get on this forum that I'm not going in the wrong direction, accepting a copper pour (or plane) in place of that spider web single point ground approach"
I'll reply more in detail later, probably tomorrow, had a hard day at work, just started a new design lots of analogue sections, highish current motor drive circuits, digital and over 4000 pins and 4000 connections! I'm going to be laying it out for at least a month. So rather drained at the moment.
Have you got a schematic of the design, it would help and I would be interested in looking at it and how the layout relates to it.
On oscillations decoupling is one of the main tools to prevent it, I do somewhere have (again) some relevant documents I'll have a dig through tomorrow when I am back at work.
Regarding other views, there are many on this forum, many do support the spiders legs 0V as it is an ingrained view often found in The DIY audio community. As I said earlier there is also the possibility of RF noise pickup these days (op-amp oscillations are often high frequency related) so having a scheme that allows you to handle and control the loops for high frequency will help supress and limit these problems, and here a GND plane is your friend. There will be a division of views regarding this🙂
One excellent thread is this:
http://www.diyaudio.com/forums/chip-amps/252436-lm3886-pcb-vs-point-point-data.html
there are others (including one where due to tiredness,stress and overeating I make a complete plonker of myself) some that have got rather heated. At the end of the day Audio is analogue design (and analogue/digital when DACs etc. are involved) and there is tons of info out there as my eclectic mix of documents shows.
Have you got a schematic of the design, it would help and I would be interested in looking at it and how the layout relates to it.
On oscillations decoupling is one of the main tools to prevent it, I do somewhere have (again) some relevant documents I'll have a dig through tomorrow when I am back at work.
Regarding other views, there are many on this forum, many do support the spiders legs 0V as it is an ingrained view often found in The DIY audio community. As I said earlier there is also the possibility of RF noise pickup these days (op-amp oscillations are often high frequency related) so having a scheme that allows you to handle and control the loops for high frequency will help supress and limit these problems, and here a GND plane is your friend. There will be a division of views regarding this🙂
One excellent thread is this:
http://www.diyaudio.com/forums/chip-amps/252436-lm3886-pcb-vs-point-point-data.html
there are others (including one where due to tiredness,stress and overeating I make a complete plonker of myself) some that have got rather heated. At the end of the day Audio is analogue design (and analogue/digital when DACs etc. are involved) and there is tons of info out there as my eclectic mix of documents shows.
That is much better, but you still have some long traces on the back of the board that could be made shorter by tweaking things on the top, this gives you a more solid plane.
You will want to look closely at the alignment of tracks and pads, as you seem to have tracks entering pads so they partially overlap the edge of the pad, this makes soldering harder then it needs to be, especially if doing a two layer job yourself and working without resist.
You have bussed together a load of pins on the 20 way dual row thing (Header I suspect), but then do not connect them to anything, could be right, looks suspicious.
Your decoupling appears to be rail to rail, which contrary to Doug Self is not a good plan if you have opamps any faster then the 5532 (Good opamp but you can get away with it there, more modern parts not so much), the current loop for an opamp is output->load->ground -> supply pin via decoupling cap (Which one changes depending on which quardrant the drive is in), and you want to keep loop areas small.
You have acid traps (Acute angles between copper where etchant can become trapped).
Don't worry, my first efforts were worse (Done on acetate with black tape and a scalpel....).
A physical rule to bear in mind at all times when laying out a board: "Current flows in loops, always", the objective is to minimise the area (And thus make the loop minimally effective as an aerial), and to minimise impedances and thus voltage drop (Or to be careful about where you reference circuits.
My usual approach for small signal audio is a plane which has the supplys decoupled to it, then run audio and a reference connection from the output of one stage to the input of the next, with the reference connection tied to the plane near the previous stages local decouplers.
Regards, Dan.
You will want to look closely at the alignment of tracks and pads, as you seem to have tracks entering pads so they partially overlap the edge of the pad, this makes soldering harder then it needs to be, especially if doing a two layer job yourself and working without resist.
You have bussed together a load of pins on the 20 way dual row thing (Header I suspect), but then do not connect them to anything, could be right, looks suspicious.
Your decoupling appears to be rail to rail, which contrary to Doug Self is not a good plan if you have opamps any faster then the 5532 (Good opamp but you can get away with it there, more modern parts not so much), the current loop for an opamp is output->load->ground -> supply pin via decoupling cap (Which one changes depending on which quardrant the drive is in), and you want to keep loop areas small.
You have acid traps (Acute angles between copper where etchant can become trapped).
Don't worry, my first efforts were worse (Done on acetate with black tape and a scalpel....).
A physical rule to bear in mind at all times when laying out a board: "Current flows in loops, always", the objective is to minimise the area (And thus make the loop minimally effective as an aerial), and to minimise impedances and thus voltage drop (Or to be careful about where you reference circuits.
My usual approach for small signal audio is a plane which has the supplys decoupled to it, then run audio and a reference connection from the output of one stage to the input of the next, with the reference connection tied to the plane near the previous stages local decouplers.
Regards, Dan.
Thanks Dmills. And just to offer you a giggle, I too remember the days of acetate tape PC boards. In fact to really make you choke, how about single sided board 'stencils", made by drilling holes in plastic, connecting traces with a coping saw, then spray painting the design down to copper clad (AHHHGGG!). Should you want to hear more pain, my first PCB cad was on an ATARI system, and it used CHARACTER graphics to build its traces and pads. Its fortunate I have considerable hair to pull out of my head, but I digress!
Several things you mentioned I've already been touching up, bust some (like getting the trace to pad angles right) are a little tough when I'm adjusting things. My current PC cad, DesignSpark-PCB, is absolutely amazing for the price (its free!), but it does make it tedious to really optimize things.
This board is only about 4 x 2.5, so I'm hopeful the long runs will be tolerated. The problem in this case is that There is a great deal of I/O, and all those jacks ( 10 audio, plus the header you mentioned) must be at the board edges. So while some adjustment is now possible (with so much clutter removed from all my former 'single point' ground runs) there is still the limitation of how close you can space these I/O jacks. But I will consider everything you said.
The real sad thing, which I've ranted about in another thread, is that it can be so cost prohibitive for the DIY budget to make prototype PC boards, it becomes impossible (except through the passing of many years and many dollars), to develop a good instinct for what works best in various situations. Even the original discussion thread here, about the merits of single ground grounds vs a solid ground plane seems less contentious than the US congress, as I poke around more and more discussions on the subject. You can see why I'm so hesitant to abandon the practice. Fortunately my "rant" did prove fruitful, as I seem to have discovered at least a few VERY affordable PCB prototyping places. Now I can TRY new approaches with a little less pain. 🙂
Several things you mentioned I've already been touching up, bust some (like getting the trace to pad angles right) are a little tough when I'm adjusting things. My current PC cad, DesignSpark-PCB, is absolutely amazing for the price (its free!), but it does make it tedious to really optimize things.
This board is only about 4 x 2.5, so I'm hopeful the long runs will be tolerated. The problem in this case is that There is a great deal of I/O, and all those jacks ( 10 audio, plus the header you mentioned) must be at the board edges. So while some adjustment is now possible (with so much clutter removed from all my former 'single point' ground runs) there is still the limitation of how close you can space these I/O jacks. But I will consider everything you said.
The real sad thing, which I've ranted about in another thread, is that it can be so cost prohibitive for the DIY budget to make prototype PC boards, it becomes impossible (except through the passing of many years and many dollars), to develop a good instinct for what works best in various situations. Even the original discussion thread here, about the merits of single ground grounds vs a solid ground plane seems less contentious than the US congress, as I poke around more and more discussions on the subject. You can see why I'm so hesitant to abandon the practice. Fortunately my "rant" did prove fruitful, as I seem to have discovered at least a few VERY affordable PCB prototyping places. Now I can TRY new approaches with a little less pain. 🙂
You might wish to investigate turning on whatever 'snap to grid' or 'snap to pad' functionality your tool has, use a 1mm or so grid for placing footprints, followed by switching the grid to match your min track and gap.
As a hobbiest you can usually aford to wait a week or so for a board, at which point China becomes a real possibility, even via a reseller (seeed or suchlike).
My view of hobby things is that just like my professional boards I generally start at 4 layers (And am not that bothered by going to 6) because the time saving is worth more then the incremental cost of so doing.
Regards, Dan.
As a hobbiest you can usually aford to wait a week or so for a board, at which point China becomes a real possibility, even via a reseller (seeed or suchlike).
My view of hobby things is that just like my professional boards I generally start at 4 layers (And am not that bothered by going to 6) because the time saving is worth more then the incremental cost of so doing.
Regards, Dan.
Post a schematic. The layout is critically related to the component and circuit functions. You're asking for help, and tying the hands of the helpers. Why? I have my suspicions. Trying to get free help for a commercial project without disclosing details?
Post your layouts with the layers superimposed. It should be possible to see where tracks overlap, you can in most software I've used. Blue/Red is good, overlap shows purple.
Print the silkscreen on the same layout, so we can see the component orientation. Orient the labels, don't leave them under components, somebody may need to debug this at some point.
Always aim for the smallest populated area. This will automatically minimise strays. You've used SMT, good, now exploit it. The component spacing is limited by the skill of the assembler, or the P&P machine.
A print with ground, or the power rails highlighted makes evaluating the work much easier.
Single-point ground is not that disastrous, it's frequently seen in point-to-point wired tube circuits. It's frequently resorted to on PCBs in an attempt to reduce the brainwork required to analyse the return currents in detail, and in the absence of experience of component placement for the best power supply decoupling. In large organisations such skills are frequently passed on, often embedded in existing designs, although unfortunately it is not always the case that what is passed on is really best practice.
There has been a lot of discussion here about layout for optimum performance, but the failings of a single-point ground admitted, performance will not be far suboptimal.
Rail-to-rail decoupling will in any case be superior to what is being obtained with 5532s and leaded caps, as long as you make the effort to keep the traces short. If the decoupling is truly too slow, the usual response is to double up using caps a couple orders magnitude smaller, 100n||1n?
Post your layouts with the layers superimposed. It should be possible to see where tracks overlap, you can in most software I've used. Blue/Red is good, overlap shows purple.
Print the silkscreen on the same layout, so we can see the component orientation. Orient the labels, don't leave them under components, somebody may need to debug this at some point.
Always aim for the smallest populated area. This will automatically minimise strays. You've used SMT, good, now exploit it. The component spacing is limited by the skill of the assembler, or the P&P machine.
A print with ground, or the power rails highlighted makes evaluating the work much easier.
Single-point ground is not that disastrous, it's frequently seen in point-to-point wired tube circuits. It's frequently resorted to on PCBs in an attempt to reduce the brainwork required to analyse the return currents in detail, and in the absence of experience of component placement for the best power supply decoupling. In large organisations such skills are frequently passed on, often embedded in existing designs, although unfortunately it is not always the case that what is passed on is really best practice.
There has been a lot of discussion here about layout for optimum performance, but the failings of a single-point ground admitted, performance will not be far suboptimal.
Rail-to-rail decoupling will in any case be superior to what is being obtained with 5532s and leaded caps, as long as you make the effort to keep the traces short. If the decoupling is truly too slow, the usual response is to double up using caps a couple orders magnitude smaller, 100n||1n?
@CC: I will post a layered shot, as soon as I finish a few more tweaks. Been a long day. As far as your suspicions, I'll freely admit I often ask for help on things I'd like to think I can sell someday, and I'd gladly offer my experience to anyone else doing so if I felt it would be helpful. One hand washes the other.
But MY reason for not jumping to post schematics is usually not because I'm hiding some rocket science secret. Rather, I try my best to confine a discussion to a particular point. Its been my experience that the more of an entire system I see anyone post, the more scattered and splintered the discussion becomes. Before you know it, one specific principal becomes so convoluted, the original point gets totally lost.
Back on the original subject, back in Tube days I seldom saw discussions like this. I didn't do a lot of design work back then, but I serviced a lot of music equipment, guitar amplifiers and such, and I rarely saw anything resembling a "single point" grounding scheme. maybe I wasn't exposed to "high end" gear, but most circuit construction seemed to just favor the nearest point on a chassis for ground, or a wide band of trace running around the edge of the board. Single point grounding was something that never dawned on me until I saw it in OP amp design books, amid explanations about avoiding ground loop oscillations. Maybe I've been adhering to something recommended by authors, who's audience was very likely to be doing point to point hand wiring on simple perf boards. But the fact that some builders still seem to swear by it means it must have still some merit in some applications. I'm willing to try the "plane" approach this time, but I'm not quite ready to conclude its always better than single point.
By the way and as an aside,you mentioned that the component spacing is limited by the skill of the assembler. Unfortunately these days, my skills have diminished. My aging eyesight can be aided by glasses and magnifiers, but hands much less steady then they once were have been another handicap. Hence, I avoid both ICs with a pitch smaller than 0.050in, and passives smaller than 805. We all do what we can. There are a few things I've built that I'd like to see eventually become 1/2 the size they are now.
But MY reason for not jumping to post schematics is usually not because I'm hiding some rocket science secret. Rather, I try my best to confine a discussion to a particular point. Its been my experience that the more of an entire system I see anyone post, the more scattered and splintered the discussion becomes. Before you know it, one specific principal becomes so convoluted, the original point gets totally lost.
Back on the original subject, back in Tube days I seldom saw discussions like this. I didn't do a lot of design work back then, but I serviced a lot of music equipment, guitar amplifiers and such, and I rarely saw anything resembling a "single point" grounding scheme. maybe I wasn't exposed to "high end" gear, but most circuit construction seemed to just favor the nearest point on a chassis for ground, or a wide band of trace running around the edge of the board. Single point grounding was something that never dawned on me until I saw it in OP amp design books, amid explanations about avoiding ground loop oscillations. Maybe I've been adhering to something recommended by authors, who's audience was very likely to be doing point to point hand wiring on simple perf boards. But the fact that some builders still seem to swear by it means it must have still some merit in some applications. I'm willing to try the "plane" approach this time, but I'm not quite ready to conclude its always better than single point.
By the way and as an aside,you mentioned that the component spacing is limited by the skill of the assembler. Unfortunately these days, my skills have diminished. My aging eyesight can be aided by glasses and magnifiers, but hands much less steady then they once were have been another handicap. Hence, I avoid both ICs with a pitch smaller than 0.050in, and passives smaller than 805. We all do what we can. There are a few things I've built that I'd like to see eventually become 1/2 the size they are now.
Though I still have some tweaks to complete, mostly edge positioning of some parts to better fit an enclosure, I'm posting a layered screenshot of this board just for contextual reference. I'm still open to everyone's thoughts, especially on the original topic regarding single point grounding layouts vs. solid ground plane layouts, as I've now migrated to the latter for this design.
For reference, the top 8 shapes are 1/8" stereo jacks, used with Y-Insert cables to plug into various guitar effect pedals. The large left and right shapes are 1/4" jacks where a guitar plugs in, and an output to an amplifier goes, respectively. A1 and A2 are dual OP amps used for input and output buffers, with 1/2 of the left OP amp also used to create a virtual ground for all audio I/O. Virtual Gnd is also connected to the copper pour area (my 2 layer version of a ground plane). U1 and U2 are quad analog SPDT switches made by Maxim and/or Intercil, and the header at the bottom is for digital external contact closure inputs from another circuit/system, enabling external control over which guitar effects are in-use or bypassed.
I'm still not posting a schematic, since its irrelevant. Doing so could never include the vast array of devices that could plug into this board, and I wish to confine the discussion to the routing issues. But I will email a schematic to anyone interested who contacts me personally.
Again, the actual dimensions of the board are about 4" x 2.5". This image, when expanded, is about 2:1
For reference, the top 8 shapes are 1/8" stereo jacks, used with Y-Insert cables to plug into various guitar effect pedals. The large left and right shapes are 1/4" jacks where a guitar plugs in, and an output to an amplifier goes, respectively. A1 and A2 are dual OP amps used for input and output buffers, with 1/2 of the left OP amp also used to create a virtual ground for all audio I/O. Virtual Gnd is also connected to the copper pour area (my 2 layer version of a ground plane). U1 and U2 are quad analog SPDT switches made by Maxim and/or Intercil, and the header at the bottom is for digital external contact closure inputs from another circuit/system, enabling external control over which guitar effects are in-use or bypassed.
I'm still not posting a schematic, since its irrelevant. Doing so could never include the vast array of devices that could plug into this board, and I wish to confine the discussion to the routing issues. But I will email a schematic to anyone interested who contacts me personally.
Again, the actual dimensions of the board are about 4" x 2.5". This image, when expanded, is about 2:1
An externally hosted image should be here but it was not working when we last tested it.
Guesing the SOIC20s are DG333 or similar analog switches, and the SOIC8s more or less have to be '072s (It is a guitar box after all).
Seems likely to click when switching (Charge injection into high Z guitar pedal inputs), also possible offset voltages at pedal outputs, guess R11,12 and friends are an attempt to supress this.
A Diode on the DC input jack would help real world reliability and a few hundred uF of bulk decoupler would be a good idea....
Also maybe some ESD clamps or at least some series resistance, going straight from the outside world to a cmos input is seldom a great idea.
Circuit Diagrams? I don't need no steenking diagrams.
Regards, Dan.
Seems likely to click when switching (Charge injection into high Z guitar pedal inputs), also possible offset voltages at pedal outputs, guess R11,12 and friends are an attempt to supress this.
A Diode on the DC input jack would help real world reliability and a few hundred uF of bulk decoupler would be a good idea....
Also maybe some ESD clamps or at least some series resistance, going straight from the outside world to a cmos input is seldom a great idea.
Circuit Diagrams? I don't need no steenking diagrams.
Regards, Dan.
- Status
- Not open for further replies.