EEVblog Electronics Community Forum
Electronics => Projects, Designs, and Technical Stuff => Topic started by: Plecto on May 16, 2015, 07:13:52 pm
-
I've now stripped my design down to this:
(http://www.electronics-radio.com/articles/analogue_circuits/operational-amplifier-op-amp/op-amp_non_inv_with_capinput.gif)
Op-amp is OPA551 (http://www.ti.com/lit/ds/sbos100a/sbos100a.pdf (http://www.ti.com/lit/ds/sbos100a/sbos100a.pdf)).
C1 is removed for debugging purposes.
R1=4.7kOhm
R2=100kOhm
R3=100kOhm
Power supply is a 50VA +/-18VAC linear transformered followed by a SMD rectifier chip followed by 2x4700uF rectifying caps. There's also 2x470nF ceramic caps near the supply pins of the op-amps. Here's what the output looks like:
http://i61.tinypic.com/2079teg.jpg (http://i61.tinypic.com/2079teg.jpg)
The 100hz hum will depend on gain and voltage ripple (which is about 1V), but it also depends on the value of R3, if the input is shorted to ground the hum goes almost completely away which shows that the hum isn't caused by the lack of PSRR, right?
The PCB has a nice star ground with almost every current return path meeting up at the exact same point. I've also made loads of different jumper wires to try and change the ground layout (I was getting desperate), but nothing I did made a difference. I think this shows that the hum isn't caused by a ground loop as there are no ground loops.
Right now the PCB and transformer are just laying on my desk with about 15cm of wire between them. Moving the transformer and/or PCB around makes absolutely no difference to the hum which I think shows that the hum isn't coupled from the air, right?
I really need some help to think of other my amp can output humming like that, I'm just completely clueless. One last important point to make is that the humming is exactly the same for both channels. Thank's in advance for any advice :) Best regards, frustrated and slightly depressed engineer |O
-
Looks like you are having fun with common-mode noise - noise that creeps up between ground and your input signal.
In this case, it looks like your output dips might be caused by the current peak from your transformer and rectifiers when the capacitors get topped off. High resistance in the neutral/ground path combined with those current peaks creates voltage between input and ground, gets amplified ~20X by your op-amp and you get what you get.
-
Could you explain a little further, I don't get how that could happen? My grounding scheme looks like this:
(http://i58.tinypic.com/ibif4x.jpg)
Any voltage drop created by the charging of the rectifying caps will be present for both the input resistor, feedback return resistor and output gnd so I don't see how the voltage at the input with respect to ground can change?
-
Photos ?
-
current to the device should go through the leg of the cap, then to the device pin, in the case of your 470nF caps, how you have drawn it looks wrong,
perhaps post either your schematic, or your pcb layout, it will be easy enough to tell from both of those.
-
I think the schematic and board layout will be misleading and hard to understand as there are a lot of components shown that are not soldered to the board. I've highlighted ground:
(http://i60.tinypic.com/11v36eo.jpg)
-
Hi;
your GND wires are much too thin and long.
They will pick up any radiated noise.
Go double sided, use the top as ground, and use a ground fill.
Mick M
-
The PCB has a nice star ground with almost every current return path meeting up at the exact same point.
Looks more like spiderweb. And I don't see current return paths meeting same point at all.
-
(http://i57.tinypic.com/f1w0v4.jpg)
I've now pointed to where the 470nF caps, feedback return and input resistor for both amplifiers meet up at the same point. Output ground is connected further along the line as I showed previous.
Hi;
your GND wires are much too thin and long.
They will pick up any radiated noise.
Go double sided, use the top as ground, and use a ground fill.
I have though about going double sided, but it's more expensive and it takes longer to make, I would rather use a couple of jumper resistors than to go two sides. How do I know if the humming I hear is caused by radiated noise? Shouldn't the noise vary in intensity when moving the board around if that was the case? Why are the traces too thin, they are hardly carrying any current?
-
Scoping both channels. It's AC coupled and I put on a 250hz digital filter to remove the static. The output hum is identical for both channels which can't be a coincidence, right?
(http://i57.tinypic.com/2gy3uxz.jpg)
-
What's up with all the floating copper? Go two sided, ground it all, and stitch everything!
How much of your equipment is grounded?
Tim
-
What's up with all the floating copper? Go two sided, ground it all, and stitch everything!
How much of your equipment is grounded?
Tim
It's just to preserve my developer and etching solution, some boards have a lot of free space :) I don't yet see the reason for going two sided though? Unless my board was extremely difficult to layout and required a lot of jumpers, a two sided board is more expensive and takes longer to make.
Do you mean what components on my board that's connected to ground? Nothing other than what's in the schematic shown in the opening post. C1 (the cap above the attiny84) is also removed. If you mean grounded as in connected to mains earth? Nothing is, there's no mains earth in here:
(http://www.maison.lv/res/WDE001040.jpg)
-
Could it be related eventually to the double of the mains' frequency, (if it is 50Hz locally)? I recall a technician telling me something about that.
In my case, poor grounding in a negative voltage generator using the ICL7660, IIRC.
-
I've now pointed to where the 470nF caps, feedback return and input resistor for both amplifiers meet up at the same point. Output ground is connected further along the line as I showed previous.
The issue is you selected some really strange point where all currents "meet" (actually don't meet at all) and call this star ground. Putting output between input and power GND (4700uF capacitors) means that significant current will flow through the signal ground too. Star ground means that all currents return to the same ground point and don't interfere with each other.
Moreover your PCB design is spaghetti filled with insane number of very long and thin traces.
http://www.lh-electric.net/tutorials/gnd_loop.html (http://www.lh-electric.net/tutorials/gnd_loop.html)
Ground Loop can be described as unwanted signal pickup from shared-ground connections. In audio equipment it is evident as hum or other interference in the speakers. Ground Loop is best explained in Figure 1. below.
Exactly your case:
(http://www.lh-electric.net/img/gnd1.gif)
The microphone and the loudspeaker share a common line between node N1 and N2. A small signal voltage is generated due the loudspeaker relatively high current and some resistance in the line (wire). The voltage equals i * Rl. The sensitive microphone input will pick-up this unwanted signal and amplify it further in the amplifier stages. In the worst case, there could be a positive feedback, resulting in spontaneous oscillations. Damage to speakers and/or amplifier may occur. At best, feedback signal will modify the overall frequency response of the audio equipment.
Fig.2 shows a correct common ground wiring of the same device..
(http://www.lh-electric.net/img/gnd3.gif)
-
Some years ago when I started doing some PCB's, I'd send the layout to my PCB mentor, a Dr of EE.
He invariably called them "gawd awful" and offered a hint to make them better.
Back and forth until he thought I had learnt something.
I learnt a lot about simple layout and the last one I sent him there was only praise.
Yours is gawd awful......sorry, start again from scratch.
Place components THAT CAN'T be moved, power devices, jacks etc. and think carefully about the remaining component orientation and placement NOT ONLY for signal path BUT VCC and GND connection too.
Now all this can take real time, your PCB might take me a good day until I was happy. :popcorn:
A nice SS PCB is a thing of beauty, often tricky too, to get minimal links on the other side.
Use a few TH passives to open paths for routing. Manually route, it's the only way to get the board nice. Use Autoroute only to provide clues and guidance.
Aim to do a SINGLE GND pour to finish(no dead copper), that pour connecting to the GND's required directly or via short traces. Where possible keep ALL traces as short as possible.
Trace length matching if needed for HF or buss'es, best ask others for help. ;)
-
The issue is you selected some really strange point where all currents "meet" (actually don't meet at all) and call this star ground. Putting output between input and power GND (4700uF capacitors) means that significant current will flow through the signal ground too. Star ground means that all currents return to the same ground point and don't interfere with each other.
Moreover your PCB design is spaghetti filled with insane number of very long and thin traces.
http://www.lh-electric.net/tutorials/gnd_loop.html (http://www.lh-electric.net/tutorials/gnd_loop.html)
I can't seem to see the issue. I guess I've attempted a sort of quasi-star ground by at least having every ground path that matters connected to the same point, the only thing deviating from this is the output which is connected further down the line. I've been aware of this and I know that any current flowing to and from my 470nF caps will effectively change the ground potential from the output thus creating hum, but removing the 470nF caps makes no difference, nor did it to cut the output ground and jumper wire it to the same point as everything else. The hum also varies with gain which proves that it's not caused by the output ground not being connected to the 'quasi-star'. With the 470nF caps removed I don't see how there's any current flowing in my ground leads at all, other than the input bias current and feedback current+output current caused by the tiny offset voltage. What difference would it make if I were to also connect the 4700uF caps to my star ground point? That would make it truly star ground though, wouldn't it? Only with a single trace running from the meet-up point to the edge of the board back to the transformer which would effectively just act as an extension of the transformer wire.
Some years ago when I started doing some PCB's, I'd send the layout to my PCB mentor, a Dr of EE.
He invariably called them "gawd awful" and offered a hint to make them better.
Back and forth until he thought I had learnt something.
I learnt a lot about simple layout and the last one I sent him there was only praise.
Yours is gawd awful......sorry, start again from scratch.
Place components THAT CAN'T be moved, power devices, jacks etc. and think carefully about the remaining component orientation and placement NOT ONLY for signal path BUT VCC and GND connection too.
Now all this can take real time, your PCB might take me a good day until I was happy. :popcorn:
A nice SS PCB is a thing of beauty, often tricky too, to get minimal links on the other side.
Use a few TH passives to open paths for routing. Manually route, it's the only way to get the board nice. Use Autoroute only to provide clues and guidance.
Aim to do a SINGLE GND pour to finish(no dead copper), that pour connecting to the GND's required directly or via short traces. Where possible keep ALL traces as short as possible.
Trace length matching if needed for HF or buss'es, best ask others for help. ;)
What makes the board so awful? I'm not doubting that massive improvements could be made :p But just because something has the potential of being improved doesn't mean that there are any benefits from doing so for this particular circuit, is it?
-
What difference would it make if I were to also connect the 4700uF caps to my star ground point? That would make it truly star ground though, wouldn't it? Only with a single trace running from the meet-up point to the edge of the board back to the transformer which would effectively just act as an extension of the transformer wire.
If you connect 4700uf capacitors and power supply ground to this point there might be some difference. But your design is awful overall, therefore not guaranteed that it will fix the issue.
-
What's up with all the floating copper? Go two sided, ground it all, and stitch everything!
How much of your equipment is grounded?
Tim
Why is your board so awfull? ^^^^^^^
Copper antennas, capacitively coupled to your signal paths.
-
I cut some traces, added some jumpers and made a true star ground with the output, transformer and 4700uF caps meeting up at the same point, it made no difference to the level of hum.
If I were to make another board and have it two sided, what would I do different? Even if I were to make a board that was hum free, it would be really satisfying to know what it particular was faulty with this board as I don't want to do the same mistake in the future :(
Copper antennas, capacitively coupled to your signal paths.
The only input I have are a couple of mm of copper trace as the input caps are removed, I don't see they can be an issue.
I really appreciate all the replies I'm getting though, I really really want to fix this thing :P
-
As you didn't post the schematic, no one can guarantee that the issue doesn't lie in it. However if you make 2 layer PCB, safest for you will be to use one side mostly for the ground plane. Also route all tracks as short as possible, you can put some of them on second (GND) layer. Just try to not split ground plane too much.
-
I'll give it a go then. How should the second layer look? Thick traces forming a star ground or just fill the whole layer as a ground plane? I have to router around the through hole components so it won't be completely filled. About the talk of having a ground plane, I've tried this in the path and it almost always leads to a ground loop as there are always parts of the plane that's thin enough to form enough of a drop to cause hum.
The schematic was posted in the opening post, just multiply it by two to get both channels :)
-
That is not real schematic. Just stripped down something, therefore don't tell anything. Put solid ground. Making star ground might be worth only if you are really understanding why you need it and how it is done properly.
-
What makes the board so awful?
I haven't looked at the actual circuit but:
Unconnected chunks of copper all over the board leap out at me (to preserve etching solution?). Those things will pick up RF signals and add random capacitance all over the place.
Mix in a lack of understanding about what ground loops are and it's not surprising the thing hums.
If I were to make another board and have it two sided, what would I do different?
Making it double sided isn't a magic fix. You need to understand the basics first. Start by eliminating all ground loops and connect all those copper pads to ground (or just remove them - they don't do much on a single layer board).
-
I'll give it a go then. How should the second layer look?
If you go with a ground plane for your second layer, then it should simply be a copper pour to fill all space not used for other traces. In some cases where there might be significant ground currents going across the board, you may need to adjust your layout to keep sensitive circuits out of current return paths or surround the sensitive circuits with a gap to direct unrelated ground currents away from it.
Since your main reason to go single-sided is to preserve etchant, doing a copper pour should eliminate 95% of that concern - the whole bottom layer will be copper except for the clearances for whatever non-ground nets you might share it with.
-
Have you tried powering the setup with batteries? Often, hum comes from non-isolated external PSU. If the hum disappears either you need a better designed external PSU or isolated those ground loops.
-
The 100hz hum will depend on gain and voltage ripple (which is about 1V), but it also depends on the value of R3, if the input is shorted to ground the hum goes almost completely away which shows that the hum isn't caused by the lack of PSRR, right?
Your amplifier picks up hum if you leave the input open (only shunted by R3) and you're surprised?
-
I haven't looked at the actual circuit but:
Unconnected chunks of copper all over the board leap out at me (to preserve etching solution?). Those things will pick up RF signals and add random capacitance all over the place.
Mix in a lack of understanding about what ground loops are and it's not surprising the thing hums.
I haven't really thought of the chunks of copper picking up RF and adding capacitance, but aren't having a ground plane and star ground mutually exclusive? Not having a ground plane gives me freedom to choose where the ground current flows, having a ground plane will make the ground current flow wherever there is space for it to flow and to me that looks like it adds to the likeliness of ground loops occurring unless the components are correctly placed on the board. Take my board as an instance, if I were to fill every empty space with ground copper, both the input and output will be grounded at different points with their difference in potential depending on how thick of a copper trace that's between them (which again I don't have much control over). Am I not correct about this?
I don't think I have a lack in an understanding of what ground loops are, I just don't see why 'every' current return path has to meet at the same point.
That is not real schematic. Just stripped down something, therefore don't tell anything. Put solid ground. Making star ground might be worth only if you are really understanding why you need it and how it is done properly.
Why isn't it a real schematic? The only thing missing is the transformer, rectifier and caps?
Surely only the parts that matters has to be taken special care of? I see no way of humming becoming an issue as long as the input resistor, feedback return, input, pot and output are connected to the same point and all have the same potential. It doesn't matter if the charging of the caps is causing massive voltage drops due to tiny ground traces since the voltage drop is equal for all the points mentioned above. I don't see how it matters where or how all other ground points are connected, please help me understand.
Have you tried powering the setup with batteries? Often, hum comes from non-isolated external PSU. If the hum disappears either you need a better designed external PSU or isolated those ground loops.
No I haven't, but the humming goes away if I turn the amp on so it's Humphrey in the short period where the amp is powered by the caps (which is sort of like powered from batteries :P )
Your amplifier picks up hum if you leave the input open (only shunted by R3) and you're surprised?
Yes I am? :P Why wouldn't I?
I'll try and make a new board with one layer being a complete ground plane and see how it goes, hope it's going to work :)
-
Your amplifier picks up hum if you leave the input open (only shunted by R3) and you're surprised?
Yes I am? :P Why wouldn't I?
Because the hum doesn't come from your amplifier, but it's simply picked up by the open input.
-
Because the hum doesn't come from your amplifier, but it's simply picked up by the open input.
Picked up from where? And can a tiny piece of 16mil copper trace pick up 90uV of hum? If so, shouldn't the humming vary with the length of the trace?
-
It's not so much a question of physical size (although it matters, too, but not too much. A 2 cm long trace doesn't pick up twice as much hum as a 1 cm long trace, for example), but of impedance of the open input node, which is 100 k? in your case.
90 uV for a 100 k? node on a PCB just laying around (unshielded) on your bench doesn't seem much or exceptional to me.
As from the source of hum, it's simply everywhere. The power grids of cities are huge antennas radiating lots of 50, 100, 150, ... Hz interference. LED light strips radiate the frequency of their SMPS, many laptops radiate lots of stuff, phones occasionally put out 2+ W bursts in the GSM band and so on.
-
Just finished making a new two layer board with one layer being a complete ground plane with a bunch of vias going to it (making vias is boring). It didn't make any difference other than perhaps reduce the static noise:
(http://i61.tinypic.com/2wpjd5w.jpg)
It's not so much a question of physical size (although it matters, too, but not too much. A 2 cm long trace doesn't pick up twice as much hum as a 1 cm long trace, for example), but of impedance of the open input node, which is 100 k? in your case.
90 uV for a 100 k? node on a PCB just laying around (unshielded) on your bench doesn't seem much or exceptional to me.
As from the source of hum, it's simply everywhere. The power grids of cities are huge antennas radiating lots of 50, 100, 150, ... Hz interference. LED light strips radiate the frequency of their SMPS, many laptops radiate lots of stuff, phones occasionally put out 2+ W bursts in the GSM band and so on.
Shouldn't the humming vary as I move the board around if it was picking the hum up from the air? Also, why have I never experienced this problem before? If the humming is coming from the air, it should vary massively with the position of the pot and even when I've used 100k pots in the past, I've never experienced humming varying with the volume. If this is the issue though, how is it fixed? Will it require a metal enclosure to shield it?
-
Shouldn't the humming vary as I move the board around if it was picking the hum up from the air? I've never experienced humming varying with the volume. If this is the issue though, how is it fixed? Will it require a metal enclosure to shield it?
If you were picking up hum from air, it would vary with orientation. The fact that it does not and is exactly 100Hz strongly indicates your 100Hz spikes are coming from rectified AC peaks, either from the supply or ground side.
If the supply hum gets picked up by the preamplifier stage of your circuit before the volume control knobs, that would make the hum scale with volume.
-
Just finished making a new two layer board with one layer being a complete ground plane with a bunch of vias going to it
Care to share it with us and a FULL schematic?
There is some REAL clever buggers here but we have to see the full story. ;)
I also wonder if your scope use methodology is or isn't responsible for your findings?
Rather than photos of the scope, screenshots are better, especially if they show scope settings.
Remember scopes CAN lie, or sometimes show erroneous results if the wrong settings are used.
Even CRO's.
-
(http://i61.tinypic.com/205xfuq.jpg)
(http://i60.tinypic.com/mal5xg.jpg)
(http://i62.tinypic.com/nn2u55.jpg)
I also wonder if your scope use methodology is or isn't responsible for your findings?
Rather than photos of the scope, screenshots are better, especially if they show scope settings.
Remember scopes CAN lie, or sometimes show erroneous results if the wrong settings are used.
Even CRO's.
The humming is audible so it's not just the scope. I think my scope has a function to store screen shots, I'll do I little digging to find out :)
-
:palm: :palm: :palm:
The schematic DOES NOT match the PCB.
DO YOU WANT HELP OR NOT?
Man are you reluctant to share your design.
Do you not understand the schematic design might be your problem.
Ommited components, wrong components etc.
Unless we have the full picture there's only so much we can do to help.
-
The schematic DOES NOT match the PCB.
DO YOU WANT HELP OR NOT?
Man are you reluctant to share your design.
Do you not understand the schematic design might be your problem.
Ommited components, wrong components etc.
Unless we have the full picture there's only so much we can do to help.
Do you want a schematic that doesn't match my design? I simply though that that would be very misleading.
This schematic is purely made to make the board layout so I've payed no attention to it being easy to read, device numbers or component values. It also has some 0Ohm jumper resistors and while it looks like the collectors of the transistors aren't connected to +/-V, they are. If you want I could shine it up and make it more correct, but that would be a little work.
-
The schematic DOES NOT match the PCB.
DO YOU WANT HELP OR NOT?
Man are you reluctant to share your design.
Do you not understand the schematic design might be your problem.
Ommited components, wrong components etc.
Unless we have the full picture there's only so much we can do to help.
Do you want a schematic that doesn't match my design? I simply though that that would be very misleading.
This schematic is purely made to make the board layout so I've payed no attention to it being easy to read, device numbers or component values. It also has some 0Ohm jumper resistors and while it looks like the collectors of the transistors aren't connected to +/-V, they are. If you want I could shine it up and make it more correct, but that would be a little work.
Surely for this PCB you have a schematic in your PCB CAD package?
Post it, we can work out the rest, links or whatever. ;)
-
If you move the power supply from the left part of the scematics to the right part of the schematics, your tendency to place sensitive op amp circuit between the power supply and output stage will be reduced and you don't have to route the high current traces around the board.
-
Cut the traces to the output power transistors (power supply and driving signals) and see what happens. Try to isolate the problem.
-
Sorry, I meant to post the schematic in my previous post. http://i.imgur.com/3OqSa8Q.png (http://i.imgur.com/3OqSa8Q.png)
(http://Cut the traces to the output power transistors (power supply and driving signals) and see what happens. Try to isolate the problem.)
I have. The schematic previously shown correctly matches the circuit and the board layout correctly matches the board.
-
Are you properly grounding your ground to mains ground?
-
Are you properly grounding your ground to mains ground?
There is no mains ground (old house).
-
Try a smoothing cap across the rectifier outputs (directly across outputs) and watch out for correct voltage cap. 50v 470uf might do it.
-
It didn't fix anything, it only reduced the hum a little bit which was expected :(
-
You can try to insert something like 22-33 ohm resistors in series with opamp power pins and put 47-100uF electrolytic capacitors from power pins to GND. But IMO it is not a good idea to power such a circuit from unregulated power supply in the first place.
-
Also, as I see on the 1 sided version, power rails (which have 1Vp-p ripple) are located very close to the input signal traces. Therefore if any ripple leaks there, it will be amplified by opamps. Putting rectifier on the same PCB close to the small signal area is a very bad idea too.
-
You can try to insert something like 22-33 ohm resistors in series with opamp power pins and put 47-100uF electrolytic capacitors from power pins to GND. But IMO it is not a good idea to power such a circuit from unregulated power supply in the first place.
WORD!
And if the power supply PCB traces are too thin, the op amp power supplies may catch noise from the power supply as the current is being transferred from the power supply to the high current output stage through too thing PCB traces.
-
Also, as I see on the 1 sided version, power rails (which have 1Vp-p ripple) are located very close to the input signal traces. Therefore if any ripple leaks there, it will be amplified by opamps. Putting rectifier on the same PCB close to the small signal area is a very bad idea too.
I started thinking about that too, but is there a way to calculate how much coupling there is from one trace to another? I downloaded PCB toolkit to see if it had a tool to calculate such trace to trace coupling, but I'm not sure what to look for. I've haven't cared about what traces goes where or next to what, thinking that the frequencies on this board are way too low to make an issue, perhaps I was fooling myself? :P
You can try to insert something like 22-33 ohm resistors in series with opamp power pins and put 47-100uF electrolytic capacitors from power pins to GND. But IMO it is not a good idea to power such a circuit from unregulated power supply in the first place.
I added 30Ohm resistor in series with the supply and 220uF caps to ground. It effectively smoothed out the supply voltage to the op-amp completely (can't see any ripple at all on my scope), but the output hum is still the same.
What if I were to measure the voltage on the input to see if there actually is a small 100hz signal present? Would that help any?
-
It would be interesting to see the waveform on pin 6 of the op-amp, better still if it could be compared to the output node.
-
Connect the input to the ground through 1k resistor. Does that affect the hum?
Cut the power traces that go to the power transistors and cut the op amp output feeding the power transistors. Does that affect the hum signal amplitude seen by the oscilloscope?
-
It would be interesting to see the waveform on pin 6 of the op-amp, better still if it could be compared to the output node.
Pin 6 is the output node, the output stage is not connected to the op-amp.
Connect the input to the ground through 1k resistor. Does that affect the hum?
Cut the power traces that go to the power transistors and cut the op amp output feeding the power transistors. Does that affect the hum signal amplitude seen by the oscilloscope?
Replacing the 100kOhm with a 1kOhm reduces the hum to a level where I can't really measure it.
If I cut the power traces to the transistors there will be very little current draw from the supply which again will almost remove any ripple on the supply.
We are on to something! I was too quick to say that the filtering of the op-amp supply didn't have an effect, look at this (taken with 100kOhm input resistor):
(http://i.imgur.com/rUNS6i7.png)
That's measured through a small battery powered amp with a gain of 100 that I made so the ripple is now down from 4mVpp to 600uVpp, but the ripple waveform is now the same as the waveform of the supply (triangle wave).
-
Remove the 1k and put the 100k back, but remove the capacitor C1 at the input. Does that accect the hum?
-
Remove the 1k and put the 100k back, but remove the capacitor C1 at the input. Does that accect the hum?
C1 has never been connected. Look at the schematic in post #33.
-
Remove the 1k and put the 100k back, but remove the capacitor C1 at the input. Does that accect the hum?
C1 has never been connected. Look at the schematic in post #33.
Sorry, I missed that. Obviously the hum is being coupled to the op amp input as the hum dissapeared when you replaced the 100k resistor with the 1k resistor. So, if any of the power supply lines are near the input, the hum gets coupled either capacitively or inductively to the input, and the op amp will be amplifying the hum. Check your PCB layout and how you have routed the power supply traces. Keep the power supply traces as far as possible from the input.
-
Do you have some kind of silk screen applied to the PCB? Could that conduct the hum from the power trace to the input trace?
-
I did something wrong when I tried measuring the hum after replacing the 100kOhm input resistor with a 1k one, here's the result:
(http://i.imgur.com/dVbj67R.png)
Down from 600uVpp to almost 300uVpp. A lot of difference, but the humming didn't go away, it's still audible, but it's getting pretty faint at this point.
Do you have some kind of silk screen applied to the PCB? Could that conduct the hum from the power trace to the input trace?
Nothing like that. I did at one point begin to think that solder flux residue could perhaps cause some issues, but I've cleaned the whole board with acetone without it making any difference (except making it more shiny and good looking).
Sorry, I missed that. Obviously the hum is being coupled to the op amp input as the hum dissapeared when you replaced the 100k resistor with the 1k resistor. So, if any of the power supply lines are near the input, the hum gets coupled either capacitively or inductively to the input, and the op amp will be amplifying the hum. Check your PCB layout and how you have routed the power supply traces. Keep the power supply traces as far as possible from the input.
I'll try to have separate wires going to and from the supply pins to see what that does.
Update: I cut the power traces by removing the 30Ohm series resistors that I installed earlier. I attached jumper wires going directly from the op-amp pins to the rectifier and even removed the 470nF caps just to be sure that the supply current was flowing nowhere but in the wires, but the hum is still the same. Now that it's without the filtering that was previously added, the humming is back to where I started, about 2mVpp. Perhaps the input is coupled to one of the supplies in the op-amp internally? Perhaps I've got two faulty op-amps :( Since the waveform with and without the supply filtering looks different, is it possible that the source of the hum can be different as well? I was thinking at what point PSRR steps in, but with a PSRR at 100hz of 90dB and a ripple of now 400mVpp, PSRR should cause 0.4*10^(-90/20)*22=278uVpp which is dangerously close to the 300uVpp I get with filtered supplies + 1kOhm of input resistance.
Update: Output waveform with input shorted to ground (with supply filtering removed):
(http://i.imgur.com/nOxzRpS.png)
-
The humming varies with the input resistor value, but only to a certain point. The last screenshot shows the output when the input is grounded so whatever is causing those 2mVpp of hum is not picked up from the input. Looking at the PSRR of the OPA551:
(http://i.imgur.com/XXHENna.jpg)
I'm a little unsure of how to do these calculations as the datasheet speaks of +PSRR and -PSRR. Currenly my circuit has 400mVpp of ripple referenced to ground, but then 800mVpp referenced to -V, which of the numbers to I use to calculate the effects of PSRR on the output? That graph also shows the +PSRR declining rapidly with frequency so even though the PSRR at 100hz is a decent -90dB, it's way less for it's upper harmonics.
-
Update: I cut the power traces by removing the 30Ohm series resistors that I installed earlier. I attached jumper wires going directly from the op-amp pins to the rectifier and even removed the 470nF caps just to be sure that the supply current was flowing nowhere but in the wires, but the hum is still the same. Now that it's without the filtering that was previously added, the humming is back to where I started, about 2mVpp. Perhaps the input is coupled to one of the supplies in the op-amp internally? Perhaps I've got two faulty op-amps :( Since the waveform with and without the supply filtering looks different, is it possible that the source of the hum can be different as well? I was thinking at what point PSRR steps in, but with a PSRR at 100hz of 90dB and a ripple of now 400mVpp, PSRR should cause 0.4*10^(-90/20)*22=278uVpp which is dangerously close to the 300uVpp I get with filtered supplies + 1kOhm of input resistance.
Update: Output waveform with input shorted to ground (with supply filtering removed):
How about cutting the power traces to the transistors and wiring the transistors to directly to the rectifier and capacitors. Would this make any difference?
Well, one more thing comes to my mind: Capacitor multiplier for the op amp power supplies.
-
How about cutting the power traces to the transistors and wiring the transistors to directly to the rectifier and capacitors. Would this make any difference?
Well, one more thing comes to my mind: Capacitor multiplier for the op amp power supplies.
No, that didn't make a difference.
If PSRR is a big part of the problem then perhaps it's an idea to replace the 30Ohm resistors with diodes? That would really improve the supply ripple for the op-amp and I don't mind the 0.7V diode drop.
-
Did you ever try to change the bridge rectifier with a different one? If you don't have another bridge rectifier you might want to connect 22 nF capacitors in parallel with each diode in the bridge. See what happens.
-
Did you ever try to change the bridge rectifier with a different one? If you don't have another bridge rectifier you might want to connect 22 nF capacitors in parallel with each diode in the bridge. See what happens.
No I haven't, but what good will it do to replace the rectifier? Adding nF caps in parallel with the diodes is to filter out RF, isn't it? Is that really necessary in a circuit like this?
-
Each diode in the bridge has its own internal capacitance, which, in the case of bridge rectifiers is in the range of nF. Adding larger capacitors in parallel balances the bridge and lowers the AC component that results. Try and see if it helps. It used to be a method to minimize hum in older equipment.
-
Rather than the DSO filtering you've been using, try averaging for the scope displays. It will clean up the waveform of all the signal artifacts that AREN'T of interest to this analysis. some might be from the scope internal processing. Use BW limit too.
I notice from recent screenshots that sometimes you have the trigger set to Ch2 while showing us a Ch1 waveform. Why?
-
Each diode in the bridge has its own internal capacitance, which, in the case of bridge rectifiers is in the range of nF. Adding larger capacitors in parallel balances the bridge and lowers the AC component that results. Try and see if it helps. It used to be a method to minimize hum in older equipment.
I have a SMD rectifying chip so I guess adding capacitors won't be possible?
Rather than the DSO filtering you've been using, try averaging for the scope displays. It will clean up the waveform of all the signal artifacts that AREN'T of interest to this analysis. some might be from the scope internal processing. Use BW limit too.
I notice from recent screenshots that sometimes you have the trigger set to Ch2 while showing us a Ch1 waveform. Why?
What does DSO stand for? :P I don't know if my scope has an average function, but I am using BW limit to filter out the upper frequencies though (most of the times at least). Why I'm triggering from ch2 when showing ch1 waveforms? I find triggering on ch2 way more soothing for the soul regardless of what channel is used to display the waveform, truth be told I really didn't notice that it was triggering from ch2 :(
-
Averaging should be in the Acquire menu.
If using only 1 channel, you MUST trigger from that channel, OR at least tell us what the trigger is referenced to. (reference signal)
-
The humming varies with the input resistor value, but only to a certain point. The last screenshot shows the output when the input is grounded so whatever is causing those 2mVpp of hum is not picked up from the input.
Don't forget that opamp have 2 inputs. Therefore even if you short the non-inverting input to GND, inverting input will still pick up and amplify the noise. You can try to reduce the resistance of feedback resistors while maintaining their ratio to keep the same gain. This will reduce picking up the noise by inverting input to some extent.
-
Also I see that you put some switch in the feedback loop (guess to change the gain) supplemented by long tracks. Not smart idea.
-
Averaging should be in the Acquire menu.
If using only 1 channel, you MUST trigger from that channel, OR at least tell us what the trigger is referenced to. (reference signal)
Averaging makes the waveform smoother, but it seems to morph continuously with ever changing amplitude and waveform, perhaps it's not too helpful on odd looking waveforms? Why is it important where it triggers from? It doesn't change the look or amplitude of the waveform, does it?
I did something interesting. I did a FFT of the supply ripple voltage and noted the values for the different harmonics. It shows that the amplitude of the fundamental harmonic is about 110mVrms, adding up all the harmonics gave me a trangle wave with a peak of about 144mV, not sure why it's not even close to the actual peak of my ripple which is about 225mVp, anyway, I then multiplied each harmonic with the correct PSRR of that frequency and then added them all up, this is what I got:
(http://i.imgur.com/pjKZw9t.jpg)
The peak of the waveform that's PSRR adjusted shows about 9Vp which would amount to 20*log(144/(18*10-3))=-84dB of PSRR for such triangle waveforms with the OPA551.
Don't forget that opamp have 2 inputs. Therefore even if you short the non-inverting input to GND, inverting input will still pick up and amplify the noise. You can try to reduce the resistance of feedback resistors while maintaining their ratio to keep the same gain. This will reduce picking up the noise by inverting input to some extent.
Also I see that you put some switch in the feedback loop (guess to change the gain) supplemented by long tracks. Not smart idea.
I replaced my 100k and 4.7k resistors with 10k and 470Ohm, it made absolutely no difference to the output hum. With the input still shorted and the op-amp supply filtering removed, the hum is still about 2mVpp. I know that having the feedback path go all over the place is not a good idea, but I need a gain control and now that using ten times the lower resistor value without it making any difference I hope that I can keep my feedback path without any issues? The reason for trying to avoid a long feedback path is to prevent excessive noise and the possibility of oscillation, right? But having lower resistor values directly counters this, doesn't it? What if I needed to have my gain switch at the back of the enclosure?
So with the input shorted to ground and feedback resistor values reduced I now know that the remaining 2mVpp of humming isn't picked up on the input or in the feedback path, right? The humming is being reduced when the ripple on the supply to the op-amp is reduced, doesn't that prove that this is caused by crappy PSRR? Is there any other aspects of this op-amp that I've payed too poor attention to perhaps?
-
What does DSO stand for?
Digital Storage Oscilloscope
Averaging should be in the Acquire menu.
If using only 1 channel, you MUST trigger from that channel, OR at least tell us what the trigger is referenced to. (reference signal)
Averaging makes the waveform smoother, but it seems to morph continuously with ever changing amplitude and waveform, perhaps it's not too helpful on odd looking waveforms? Why is it important where it triggers from? It doesn't change the look or amplitude of the waveform, does it?
This is an ABC basic requirement of any scope use, Triggering correctly.
Spend some time with the Triggering set to "Normal", not Auto and get a feel for why it is important.
And put 2 signals of differing frequencies on screen and see why triggering on the signal of interest is important. ;)
Averaging helps omit the non-repeditive artifacts from the waveform displayed and is best suited for repeditive waveforms only.
The fundamental waveform is not affected by averaging.
actual peak of my ripple which is about 225mVp, anyway
I always use averaging to measure P-P ripple for the above reasons. A DSO will grab any erroneous pulse and add it to the calculations of P-P. Your 225 mV seems an awful lot of ripple for a linear PSU.
I'd want to see less than 10 mV.
-
How do you achieve 10mV of ripple? :P Even if I had nothing but my op-amps connected, the quiescent current alone would require 16000uF to get a ripple of less than 10mV.
-
How do you achieve 10mV of ripple? :P Even if I had nothing but my op-amps connected, the quiescent current alone would require 16000uF to get a ripple of less than 10mV.
SO?
PSU redesign required.
-
How about cutting the power traces to the transistors and wiring the transistors to directly to the rectifier and capacitors. Would this make any difference?
Well, one more thing comes to my mind: Capacitor multiplier for the op amp power supplies.
No, that didn't make a difference.
If PSRR is a big part of the problem then perhaps it's an idea to replace the 30Ohm resistors with diodes? That would really improve the supply ripple for the op-amp and I don't mind the 0.7V diode drop.
Capacitance multiplier migh be a better solution. See fig. 2.
http://sound.westhost.com/project15.htm (http://sound.westhost.com/project15.htm)
-
How do you achieve 10mV of ripple? :P Even if I had nothing but my op-amps connected, the quiescent current alone would require 16000uF to get a ripple of less than 10mV.
By using regulators? A 78xx has typically 50-100 µV (mainly depending on manufacturer) noise and at least 60 dB PSRR (/1000) at line frequencies, so you should get less than 1 mV noise and ripple combined even with the cheapest regulators.
I wouldn't recommend a capacitance multiplier, they are - in my experience - worse than regulators and don't have all the fancy protection built-in.
-
Ok this is likely the blind leading the blind here (as I am pretty much a newbie at this) but I had a very similar issue while working on this lab PSU I have going (am trying to design from scratch).
In my case it was because I was grounding from a point near the first of two bulk caps and the current was causing my 'ground' to jump as the voltage deviated from the ground wire resistance. When I say the first I mean the one nearer the bridge recrifier.
I found the signal traces changed a lot depending on where I put my scope ground lead. I don't know if you are finding that but it might help track down the problem. I only grounded one lead at a time to figure it out.
Also, I used LT Spice to model the circuit and inserted resistors to model the resistance of the ground path. I managed to replicate the behaviour and find a way to fix the problem.
Anyway I hope this helps.
Tom
-
glad to see that waveform, i simulated your circuit, and that is what i saw on the push-pull output stage with the input node tied to ground, its because of the output stage being effected by supply ripple,
-
Averaging should be in the Acquire menu.
If using only 1 channel, you MUST trigger from that channel, OR at least tell us what the trigger is referenced to. (reference signal)
Averaging makes the waveform smoother, but it seems to morph continuously with ever changing amplitude and waveform, perhaps it's not too helpful on odd looking waveforms? Why is it important where it triggers from? It doesn't change the look or amplitude of the waveform, does it?
When you have a 100% repeatable signal like power line AC input (unless local power sucks), setting up the trigger properly should produce 100% repeatable display with no waveform wandering.
If you enable averaging but cannot keep the waveforms locked in place by using proper triggering, you get garbage - the waveform "morphing."
Since your 100Hz is almost certainly line-related, choosing AC-trigger should stop your ripples from wandering.
-
Did you ever try to change the bridge rectifier with a different one? If you don't have another bridge rectifier you might want to connect 22 nF capacitors in parallel with each diode in the bridge. See what happens.
No I haven't, but what good will it do to replace the rectifier? Adding nF caps in parallel with the diodes is to filter out RF, isn't it? Is that really necessary in a circuit like this?
Yup. It's absolutely necessary and certainly a big difference. The key is transient behavior of diodes! Please give it a try , put a 10 - 22 nF capacitor in parallel with each diode in the bridge. You can solder even on the rectifier pads.
-
Your pcb traces are forming many loops which could have caused coupling between the rectifier part and opamp circuitry causing the hum.
Also i observed some of your traces connecting ics and other components come very close to the supply part. it is a good design practise to separate power supply part from the sensitive analog circuitry by providing some spacing between them on same pcb.