-
Vacuum tube amp PCB: Can ground planes be problematic?
Posted by
TimNJ
on 22 Dec, 2017 16:57
-
Hi everyone,
A month or two ago, I got some boards made for a layout I did for the '59 Fender Bassman guitar amp. I've come here hopefully to avoid getting told "you can't build a good tube amp on a PCB!".
The board uses a shared ground plane for the input stages (3x 12AX7 tubes in classic arrangement). The plane is tied back to a star ground point which the power supplies and output stage tie back to.
However, after assembling the board and turning it on, it was obvious I had a nasty parasitic oscillation problem. The oscillation was found even on the first stage, directly on the input connector, leading me to believe an oscillator was inadvertently formed on the first or second stage.
Here's what I've been hypothesizing as possible reasons. (These are based on my engineering insight and some guitar amp folklore.)
-Miller capacitance of the tubes, grid stopper resistors not close enough to grid pin
-Traces from subsequent stages too close to previous stage, capacitive coupling/positive feedback forming an oscillator
-Ground plane creating excessive trace-to-ground capacitance, potentially problematic on high impedance nodes
-Ground plane allows return currents from different stages to interact with each other
I'm about 75% done with a new layout that does not use a ground plane and is much more intentional about keeping the input stages far apart and laying components out in their functional blocks, as opposed to what fits/looks the best. That said, a ground plane can fairly easily be re-implemented. (How about a mini ground plane for each input tube tied back to star ground?)
For now, I've attached the old layout if anyone is interested.
What do you guys think about a ground plane causing a problem in this case?
Thank you!
-
#1 Reply
Posted by
duak
on 22 Dec, 2017 21:52
-
Unless the ground plane is on another layer, I see only a star ground with ground traces snaking outwards to the various sections. I'm not surprised that it has a few oscillation problems. The attached image shows a PCB with and without a ground plane.
Ideally, one surface, usually the top of a circuit board is a complete conductive plane or sheet with only holes for components punched thru it. This is like the metal chassis in point-to-point wiring.
There are at least three reasons to use a ground plane:
1.) reduce loop area of a circuit to minimize inductance, both self and mutual (with another circuit),
2.) reduce unwanted capacitive coupling between circuits by having an electric field terminate to ground instead,
3.) reduce DC resistance of ground return part of circuit by using wider traces or areas,
Hope this makes sense,
Best o' luck!
-
#2 Reply
Posted by
TimNJ
on 23 Dec, 2017 22:36
-
Unless the ground plane is on another layer, I see only a star ground with ground traces snaking outwards to the various sections. I'm not surprised that it has a few oscillation problems. The attached image shows a PCB with and without a ground plane.
Ideally, one surface, usually the top of a circuit board is a complete conductive plane or sheet with only holes for components punched thru it. This is like the metal chassis in point-to-point wiring.
There are at least three reasons to use a ground plane:
1.) reduce loop area of a circuit to minimize inductance, both self and mutual (with another circuit),
2.) reduce unwanted capacitive coupling between circuits by having an electric field terminate to ground instead,
3.) reduce DC resistance of ground return part of circuit by using wider traces or areas,
Hope this makes sense,
Best o' luck!
Thanks for your reply. When I said there was a ground plane, I was talking about the section of ground pour near the front of the board. That said, it's probably not a very effective one. I was a bit nervous to use a full ground plane near all the high voltage traces, although I do have design rules set on all of the high voltage nets that would make sure the ground pour is pulled back sufficiently. So maybe that was dumb...
My concern with a full ground plane is (and may very well be baseless) is: Shared return path for high currents (push-pull power amp) and low-level pre-amp return currents. Am I overthinking it? How about a full ground plane, but with slots that meet at a "star" point to isolate some of the high currents from the lower levels.
Otherwise, I guess it is unlikely that a ground plane can contribute to parasitic oscillation? I guess I was thinking a capacitor from a node to ground (in the wrong place) might cause a problem.
Thank you again. Really appreciate it!
-
#3 Reply
Posted by
duak
on 24 Dec, 2017 00:38
-
I don't think there will be any trouble with a single continuous ground plane properly connected to all necessary points and properly clearanced for the voltage. The only currents really high enough to couple to low level circuits by way of a ground plane are the 6.3 VAC heater circuit and the speaker output circuits. The plate and screen circuit currents are far less because their voltages and impedances are about 100X greater.
As a quick check to see if a ground plane or shield might help, do you have access to a piece of board material with copper on one side a bit smaller than the furthest extents of the GND net? It's OK to have holes in it as long as they are quite small. Lay the shield with the copper side away from the traces and solder short wires to various points on the GND net, particularly the locus near the power supply. Make sure there aren't any spurious connections to other circuits and see if anything changes.
If I were respinning the board I would rip up the existing GND traces and try to move as many of the traces as I could from the top layer to the bottom and then fill the top layer with a ground plane connected to GND net. If you're not happy with the idea of a single continuous ground plane, I'd consider cutting a gap in it from the mounting hole just above the 'Pine' logo all the way to the right side to make a 'C' out of it. I'd also consider putting in a couple of axial resistor footprints connected to the ground plane across the gap to stitch it back together again; one near the two coupling caps to the output stage and one on the right side. I can't quite figure out where all the inputs are and so the gap may have to be finnessed to go around them.
If respinning I'd add some 4-5 mm dia holes for cooling air around the output tubes and near any power resistors. These things get hot and even FR-4 will be affected.
I'd check to see how much of a voltage drop there is in the traces to the heaters. I'm assuming the output tubes are something like 6L6s which draw something like an amp each. I see there are single vias in the heater circuit and these could be a point of failure because of current concentration. Have you calculated the voltage drop for the given copper thickness? ie. 1 oz or 2 oz or ?
Cheers,
-
#4 Reply
Posted by
TimNJ
on 24 Dec, 2017 01:12
-
Thanks once again.
I don't have any blank copper board or foil, unfortunately, though my boss at work just introduced me to that idea on Friday, interestingly. (I'm a junior engineer.)
I was working on the board earlier today and I think I did something pretty similar to what you suggested (I think.) I've attached the progress I've made so far. One of screenshots is just the bottom signal layer, and the other is both layers. Notice the heater traces leading to the output tubes creates a big discontinuity in the low-level ground plane, so I may use jumper wires there to allow the ground plane to be continuous back to the "star" point. I might also do that up near the output tubes. Thanks for the tip about adding a few jumper footprints.
I don't plan on soldering tube sockets directly to the board, but rather ~0.75" short wires to the top of the enclosure. The board will "hang" from the top of the enclosure using 0.5" hex standoffs. But still a good idea to add a little thermal relief there, you are right. Are you suggesting those holes to allow air to rise through them?
I calculated ~0.1V drop in heater voltage at the farther output tube (5881s) based on ~16" total path with 100mil traces and 2oz copper. I think that should be okay. Perhaps I will double up on the vias, though most online resources I've seem to suggest 75mil vias would be more than adequate, but probably not a bad idea anyway.
Thank you for your awesome input.
-
#5 Reply
Posted by
T3sl4co1l
on 24 Dec, 2017 12:04
-
Star grounding typically makes worse oscillators than ground plane does. One can build an amplifier that oscillates, and vice versa, with either method.
There is no quick rule that can encompass all the considerations of a well designed circuit.
There are kernels of truth here and there: ground planes shield traces and star grounds maintain consistent DC potentials without creating loops. Most people -- the people who need "quick" rules to live their lives by -- take one or the other, and stretch it all the way to the absurd limit.
The key is to use each when appropriate, and to understand the equivalent circuit that one is creating in the layout. One must understand that the schematic is an idealized abstraction, not a description of the real layout. Conversely, one can model a real layout with an equivalent schematic, but it is likely to look very different from what one might be expecting.
Ground planes (at the PCB level) are generally not used for tube circuits, because the impedances are much too high. It is not possible to fabricate microstrip over about 150 ohms, while the circuit impedances are kohms at the lowest. It hardly matters anyway, as very few tube circuits need significant shielding, nor characteristic impedances. In any case, the low impedance of microstrip implies that stray capacitance is utterly dominant, and one should not exacerbate that by increasing it further (decreasing the PCB impedance).
Ground plane is still valuable, at the enclosure and cable level, to prevent crosstalk and interference. This, by the way, is where the myth of "terminate shield on one end only" came from: back in the toob days, electrostatic shielding is needed, again because the impedances are high enough that magnetic induction can be ignored.
Make no mistake: there is absolutely, positively nothing objectively good about leaving a shield open at one end, at radio frequency or with respect to controlled impedance conditions. You're literally introducing 100% noise to your signal, at RF!
The only reason it was done at all, was because the offending interference was electrostatic in nature, and the shield simply provides a path to shunt that field away. Likewise, not double-grounding the shield prevented ground loop currents from passing, typically a consequence of the only intense magnetic field source in a tube amplifier: the power transformer, and the currents flowing around the rectifier.
Instead, one should seek to extend the one truth (as it is at RF) down to DC, or as low as is possible. Avoid crossing current flow paths -- don't route the input around the rectifier, you'll pick up induced (electric and magnetic) hum or buzz. Do not ground coax signals to the chassis in one location, and ground the amplifier elsewhere; return the input stage to the same reference. Amplifier inputs and outputs are differential, just like everything else, by definition, because voltage is a difference. If there is a voltage drop along a ground return path, it is better for that voltage to appear on the output side than the input side, because the signal is larger on the output side. (So, if you are going to star-ground, return it to the input connection.)
It's easy to forget about AC and RF conditions. Star grounding is an invitation to oscillation. It's a series of resonant stubs just waiting to be excited; all it takes is an unlucky feedback path, probably some grids lacking adequate losses, or accidentally loaded with capacitance, and there you go. If each amplifier stage is referenced to its inputs, then one should obviously chain the grounds, from input, to stage 1, to stage 2, to output, to filter, to rectifier. That keeps all the loops precisely where they are needed (the loop between stage 1 output and stage 2 input is joined by a minimal length ground, and no currents cross it, such as rectifier-to-filter current, which is safely on the other end).
As ground plane increases capacitances, it can also be an invitation to oscillation, because of the increased capacitances. Maybe less likely? I don't know. The key, whatever the gross layout method used, is to prevent gain at radio frequencies, most importantly by adding grid stoppers. (Don't forget heater bypass if cascodes are used, too.)
Tim
-
#6 Reply
Posted by
TimNJ
on 24 Dec, 2017 17:18
-
Tim, thanks for your revealing and comprehensive response.
As always, there's no one-size fits-all solution. It seems that regardless of the approach, there's a trap to fall into, if you are ignorant to it. To that extent, I'm still not sure the direction to take on this. Since boards are so cheap, I might send a design with and without a ground plane.
While duak (above), seems confident that a ground plane will be unlikely to cause problems, I am still a bit scared of sprinkling in some capacitance throughout the board. Of course, there is probably a right and wrong way to do it, but I don't have that level of intuition yet.
I think I may consider a "bus grounding" approach, as you (seem) to suggest by chaining together the grounds of subsequent stages. Correct me if I'm wrong, but I see bus grounding as pretty similar to star grounding (in terms of the concept, not sharing return paths, etc.) but without needing to run a spider web of wires back to some location. Ground planes very openly invite shared return paths. That said, I suppose you could limit interaction of return currents but putting slots in the plane, as I have done above. Still, you have much less control of where ground currents flow, especially over top of other traces.
Very interesting about the whole floating shield thing. Thanks again.
-
#7 Reply
Posted by
floobydust
on 24 Dec, 2017 20:12
-
Books have been written on PC board layout, grounding alone. There is a lot to know and even more with high voltage/high impedance circuits. A few observations here:
If the output transformer is connected backwards, so the NFB becomes positive feedback, an oscillator results. Maybe check this (phasing) before blaming the layout.
Oscillations can result from power supply interactions.
You are supplying the O/P stages screens after the filter choke and that can make a motorboat oscillator. Try move the screens (VCC) takeoff to (VAA). It kind of depends on R9/C7 and R10/C8 values, but screen currents can modulate the preamp's power rails enough to upset it. You can try upsize C7 or C8 and see what happens.
A ground-pour is generally avoided with tube gear because the capacitive loading causes HF rolloff and instability. People also forget about the HV clearances and don't back off the pour enough, it is always avoided with mains sections.
The high-current traces such as main filter caps, output tube cathodes are dedicated short runs to the central (PSU) ground, to keep these currents out of the preamp circuit ground.
Remember my mantra "the fuse comes first" for safety; Repeat this throughout your career. Never route stuff before the fuse. IEC outlet L must go to the fuse (deep end) first.
I don't think the CM filter on the mains input is useful, you'll get lots of EMI internally from the HV rectifier diode switching transients. There is no HF suitable capacitor (disk/film) on B+ so it will be noisy for the output stage and those associated (VAA) PCB traces. After the filter choke it's much better.
I dislike a single via on the filament traces, these are maybe plated to 1/2-1oz. Not 2oz as your base PCB laminate is always less than finished copper.
MOV's on the O/P transformer add a lot of capacitance and are not really used. Marshall et al uses a HV 1.6kV diode across each tube to prevent over 2XVCC being generated by the output stage in heavy overload.
I'm not sure if you want to troubleshoot the board you built or just review and redo?
The KSL-M77 phono preamp is a tube PCB layout to look at. There are many chinese knockoffs of this kit.
It's using the multiple-ground pour (island) approach popular in Asian boutique audio, with the power supply at one side, and is one way to go which I think you are moving towards.
-
#8 Reply
Posted by
TimNJ
on 24 Dec, 2017 21:13
-
Books have been written on PC board layout, grounding alone. There is a lot to know and even more with high voltage/high impedance circuits. A few observations here:
If the output transformer is connected backwards, so the NFB becomes positive feedback, an oscillator results. Maybe check this (phasing) before blaming the layout.
I had the output transformer hooked up wrong the first time I powered it up, and sure enough, it howled like a banshee. Swapped the OT connection and that problem was resolved. Good thought, though.
Oscillations can result from power supply interactions.
You are supplying the O/P stages screens after the filter choke and that can make a motorboat oscillator. Try move the screens (VCC) takeoff to (VAA). It kind of depends on R9/C7 and R10/C8 values, but screen currents can modulate the preamp's power rails enough to upset it. You can try upsize C7 or C8 and see what happens.
Now that's a theory I've never heard of before. Doesn't the screen need to be operated at a voltage less than VAA, the plate voltage? I assume you mean, creating VCC from VAA, instead of taking it from the node following the choke. I can tack on some extra capacitance to see if that helps at all. I'd be pretty surprised if this was the problem because this is exactly how Fender did it on the 5F6A (this amp) and many of their others (to my knowledge). Not to say that Fender was perfect, as they definitely were not.
A ground-pour is generally avoided with tube gear because the capacitive loading causes HF rolloff and instability. People also forget about the HV clearances and don't back off the pour enough, it is always avoided with mains sections.
These are my biggest fears/concerns of using a ground pour. A little capacitance and high impedance nodes can spell disaster, it seems. That said, then why do some tube PCBs do it, if it's such a legitimate concern? With regard to HF rolloff, I figured the attenuated frequencies would likely be higher than the audible range? Maybe not?
Remember my mantra "the fuse comes first" for safety; Repeat this throughout your career. Never route stuff before the fuse. IEC outlet L must go to the fuse (deep end) first.
I don't think the CM filter on the mains input is useful, you'll get lots of EMI internally from the HV rectifier diode switching transients. There is no HF suitable capacitor (disk/film) on B+ so it will be noisy for the output stage and those associated (VAA) PCB traces. After the filter choke it's much better.
Thanks. With the layouts I've shown above, I've done switch -> fuse -> EMI filter. I suppose I could swap the switch and fuse though I've seen it done both ways.
I guess I kind of just threw that filter in there are "good practice" but probably not necessary as you say. I might just leave a MOV or two there.
MOV's on the O/P transformer add a lot of capacitance and are not really used. Marshall et al uses a HV 1.6kV diode across each tube to prevent over 2XVCC being generated by the output stage in heavy overload.
The MOVs are there to protect the OT and push-pull amp if someone inadvertently tries to run the amp without a load attached. The MOVs I used are 75pF at 1kHz, which I thought wasn't too crazy. What would be the problem with that? HF rolloff?
I'm not sure if you want to troubleshoot the board you built or just review and redo?
I'm not sure either. I figure there is probably more to be learned on the board I built, but I also have a lot of good ideas to implement on the new board, so it might not be worth playing around with the old one too much.
Thanks for all of your suggestions and advice!
-
#9 Reply
Posted by
TimNJ
on 24 Dec, 2017 22:06
-
Regarding split/segmented ground planes, here's what I was thinking. Still contemplating a buss ground solution with actual traces.
-
#10 Reply
Posted by
floobydust
on 26 Dec, 2017 21:38
-
The MOVs capacitance in parallel with the O/P transformer's leakage inductance makes (another) parasitic resonance. This is to be avoided. So I believe the two diode solution is preferred there. DiyAudio discussion
here. Seen in JCM800 Model 2000. I use
Vishay BY269. You must have grid-stoppers on the O/P tube's grids.
Feedback is from the O/P tranny secondary, so no load on the amplifier is not catastrophic but many manufacturers place a dummy load like 47-100R 2W on the secondary so a little load is always present.
I wonder if you are using skimpy magnetics, such as for the power transformer and filter choke.
To cut'n paste a 1950's design but with cheaper magnetics does not always work. Remember Einstein's theorem E=mc^2 so the heavier the amplifier, the more power it has
5881 screen current is 5-15mA ea. and the added load (post choke) can modulate the preamp B+. The choke and its filter cap value is important and note if you are using less (filter choke) inductance or higher DC resistance or smaller capacitance there.
This also plays a big part in how the amp sounds, the "grunt" and overload sound, as the power supply sag plays a part in that.
On the PCB layout, the HV rectifier to filter cap traces have high peak currents, so I'd use the cap's (-) as the central GND point, with dedicated traces from the rectifiers. I think your pic shows this. Also, the O/P tubes cathode return line needs a dedicated trace back the cap (-). Doing that prevents the high currents from polluting the pre-amp's GND. Then everything else is mA current levels.
I do not suggest using a GND pour around mains components and traces. A transient or flux contamination can breakdown, or a component's body or underside to the GND pour arc can happen. I would not use Y-caps as they dump all mains HF EMI to your board's GND. Many people assume GND is perfect and quiet at the IEC connector but in reality many 10's ohms impedance to earth-ground, so the Y-caps just make the guitar and cable really noisy.
I think the 5881's look too close together? They make significant heat, and no convection air holes on the PCB. Changing tubes flexes a PCB so chassis mounting holes are needed for the torque. Is this in a metal enclosure? You may get GND loops with the mounting hardware, defeating your segments if all 4 corners of the PCB are connected together through the spacers to a metal chassis.
The only tradeoff with the big GND pour approach is it maximizes PCB capacitive loading. A few pF is audible and I'm not sure how bright you want this to sound.
If the stray PCB capacitance is not symmetrical (after phase-inverter), it can make an oscillator.
-
#11 Reply
Posted by
TimNJ
on 27 Dec, 2017 06:11
-
Floobydust,
Thank you for taking time out of your day to carefully analyze and critique my work. Really humbled by that.
I see what you mean about the MOVs. I've made the switch to the diode solution. Also, I did not have grid stoppers on my original layout and it motorboated under certain conditions. I cut some traces and installed grid-stoppers and seemed to be resolved.
For magnetics, I'm using a 100VA 250V toroidal transformer (from Antek). I also have a 300V transformer that I haven't yet experimented with. I'm using a Hammond 194B choke. I believe it is intended to be a drop in replacement for the 4H choke used on the original 5F6A.
I haven't bothered routing the AC section yet so that's why I left the ground pour there. But yes, absolutely would pull back the plane there, as it is completley unnecessary.
The 5881s are a tad close. Looks like I can probably pull them apart another 0.5" or so. This will be in a metal enclosure, indeed. The board will "hang" from the top of the enclosure (on the inside) using 0.5" aluminum standoffs. Holes will be drilled in the top of the enclosure that perfectly line up with the tube footprints. Tube sockets will be soldered to the board using wires to decouple mechanical stress from the board. The tube sockets will be fastened to the chassis. There are holes in the board near the tube sockets to allow for a screw driver to hold a screw in place while tightening a nut on top side of the enclosure.
Regarding the metal standoffs, if a groundplane is used, I will pull back the plane such that an electrical connection is not made via the standoffs.
---
I did some work on the layout today, and went back to a non ground-plane design to see what that might look like. (I'm still feeling a bit queasy about using a ground plane since the parasitic effects are tough to predict and tube circuits seem particularly sensitive.)
Not changing much about the existing layout, this is a preliminary attempt at a hybrid bus/star ground layout. I've used a bus ground for the pre-amp section and then connected that bus to the negatives of the first (two) filter caps which supply the plate voltage. I feel that it may be a good approach. The high current return paths are isolated from the low-level returns using a star approach, but without the mess of a "pure star" system.
The layout is far from perfect right now, and there are many things I already want/need to change. For example, I think the return path for the left most cap, Vcc,should be reworked.. A few technicalities aside, I think this is the direction I'm going to take.
Thanks again for your help. If you are willing/up to it, I'd love to hear your feedback
-
#12 Reply
Posted by
floobydust
on 28 Dec, 2017 18:05
-
The star grounding is good for DC to low frequencies, where you need precise control of voltage drops say for uV circuits.
But it's terrible for higher (RF) frequencies as a long, thin ground trace has high impedance.
Follow the long drive from C22/C1 over to your central ground point. It's almost a loop (antenna) at RF frequencies, almost a 10" run I estimate.
Thought about it and I would say the best compromise is to have the segmented ground pours and live with the capacitive loading affecting the design. A thicker PCB laminate helps lower it too.
Mesa Boogie amp (Mark II?) I worked on has a lone mystery wire stapled to the cabinet, one end not connected to anything and the other connected to one output-tube's plate. It's called a "radiator wire" and adds intentional (stray or "gimmick") capacitive coupling from output to pre-amp stage. It helps the amp go into feedback oscillation, you have 500 volts of signal on the wire at high volumes and she starts to wail. It's kind of a secret, part of the art, not on the schematics or service manuals. Took me a while to figure it out.
My point is a few pF is a lot for these impedances and signal voltages, and on a PCB it's always higher capacitance than good old point-point wiring.
Running a PCB (signal) trace over filament traces, which have a few volts AC on it, I just don't like and again another compromise for hum and noise.
Other notes, have a grid-stopper resistor on the input tube also, as the guitar+cable etc. pick up a lot of RF like AM radio and the best amps have that and/or a small cap to GND.
P3, P6 pin spacing might not be enough for high voltages.
Your transformers and filter choke and wiring will also generate a noisy magnetic field, so watch they are not too close to the pre-amp section. Or have the metal chassis shield it with a lip bent up.
I had problems with musicians when the gig was over, unplugging their amps, tossing the power cord inside and hitting the tubes. So bent sockets and broken tubes.
You should have some metal screen to protect them.
-
#13 Reply
Posted by
TimNJ
on 29 Dec, 2017 02:03
-
Thanks again.
Good point at the unintentional antenna. That's probably asking for trouble.
I guess I'm still a little confused because dedicated traces = high inductance, and ground plane = high capacitance. Neither seem particularly great if we're talking about parasitic oscillation. I guess the idea is to make both as small as possible such that if an oscillation "wants" to occur, it's so high in frequency that's it's completely swamped out by the circuit resistance. Or at least that's how I see it. Additionally, maybe signal-trace to ground capacitance is not as big of a deal as signal-trace-to-signal-trace capacitance?
Also, I've always considered the audio band "low frequency". Maybe not?
After re-reading some of the above suggestions by you and others, I think I may have misunderstood some of the comments made about ground planes and the (possible) consequences of using one. My indecisiveness is killing me, but am feeling more confident about the ground plane this time. (I really liked how it looked too, not that that's a good reason for a layout.)
Regarding grid-stoppers on the input tube: There are grid-stoppers on the first tube, one for each channel (R4-R7). I've moved them closer in the latest layouts. Not sure if 0.5" closer will really help, but maybe.
Regarding the connectors (P3, P6): They are rated for 400V (Molex Ultra-Fit) and I used isolation slots on the board I got made, but I definitely agree, they are a little close for comfort. I am switching to Molex Mini-Fit Jr (600V) on the next revision.
I've also considered bypassing the plates with a small capacitor to ground (100nF?) to provide a high frequency return path. Just a thought.
Yes! Definitely going to be using a cage. I'm designing around a Hammond 1431 chassis which has a optional perforated top cover available. See below.
Thanks again. It's been quite a challenge thus far and it's
really nice to have some unbiased external input.
-
#14 Reply
Posted by
b_force
on 29 Dec, 2017 13:18
-
I find it a little strange to have that much oscillation.
Can you share the schematic?
If you use proper (grid) resistors on the right places, that normally would fix most of your issues.
Also, try to remove sections, so you can pin point the problem.
-
#15 Reply
Posted by
TimNJ
on 29 Dec, 2017 18:37
-
I find it a little strange to have that much oscillation.
Can you share the schematic?
If you use proper (grid) resistors on the right places, that normally would fix most of your issues.
Also, try to remove sections, so you can pin point the problem.
It's a little tricky for me to say whether it was
a lot of oscillation or not. It definitely makes it unusable.
The amplifier worked fine at low volumes and with the treble pot turned all the way down (essentially attenuating HF oscillation). I applied a sine wave to the input. As I increased the amplitude, a small oscillation (maybe 10kHz, tough to tell on my analog scope) formed on the positive slope of the wave. With a low amplitude input, the oscillation damps out once the sine wave slope goes negative. With higher amplitudes, the oscillation stays around for longer and eventually dominates. Playing a guitar through it, striking a string particularly hard, would lead to a nasty frizzy sound (oscillation) instead of the note.
So, it
kind of works but not really.
The original schematic for the board is attached. I've since cleaned it up so it's a little more logical, but does not reflect the rev 01 build. The schematic is almost identical to the original 5F6A schematic.
Thanks!
-
#16 Reply
Posted by
b_force
on 29 Dec, 2017 21:34
-
First of all, some grid resistors/stopper on the output tubes?
Something like 1k5 or 2k2.
I also would be careful with those MOVs at those places.
Varistors can act basically as capacitors, so you form a very nice little oscillation group
I have repaired quite some guitar amps, even hardwired, and I never came across such heavy oscillations.
-
#17 Reply
Posted by
floobydust
on 29 Dec, 2017 22:23
-
Experiment to see what is making it oscillate. First assume it's not the PCB layout, although that may be improved but assume it's good for now.
For troubleshooting, split it in two. The power amp and preamp section. I start with getting it to stop oscillating and check DC voltages are reasonable.
If you leave the input jacks floating, it should oscillate actually. With no 1/4" plugs, (Fender) input jacks short the preamp (or you can remove V1) and things should be quiet.
RV2, RV3 should do nothing. This tells you if the input section is getting positive feedback from somewhere and is affected.
See if the power amp section is being unstable.
I'd inject audio (from CD player etc.) at the treble control wiper and listen to the power amp. It would be tinny due to the (guitar) 0.02uF coupling cap there, but at least you can see if that amp section behaves itself. It should not motorboat or fwump fwump fwump, lol. Upsizing C20 to 100-220pF can verify it's not high freq. stuff going on assuming the MOV's are not part of the problem.
The other path for oscillation is the power supply, but it looks OK assuming the bias supply is smooth.
Using a different O/P transformer or the Presence pot RV7 value 5k is critical, so differences there can make things unstable. Most pots are all over the place for end-end resistance. Otherwise, the 27k loop feedback resistor would be changed (increased as a last resort, or small cap across it) to stabilize the power amp.
-
#18 Reply
Posted by
TimNJ
on 30 Dec, 2017 15:55
-
Well I'll be darned. It appears the oscillation was a power amp problem in disguise as a pre-amp problem. Based off the '59 Reissue schematic (1990s-present), I used a much smaller value for the power tube grid stoppers (220ohm, schematic used 47ohm). Bumped up the grid stoppers to 2.2K and wallah...stable as heck, and sounds really nice too. I also removed the MOVs for good measure, though I haven't had the chance to check with an oscilloscope to see if there was an appreciable effect. I've read somewhere that newer pentodes are more likely to have oscillation problems compared to their 50 year old brethren. I don't know if that's true or just someone trying to justify their $100 NOS GE 6L6s.
I guess I didn't think it was likely the power amp oscillation would able to get all the way back to the input jacks, but perhaps it was extreme enough to modulate the power supply rails or something(?)
There is a little radio frequency interference picked up when the presence pot is turned all the way. I suppose a simple remedy would be to reduce the maximum feedback voltage, by changing the 27K to 36K (or something).
And here I was cutting traces and tearing up the input section...
Thank you so so much to everyone who has helped thus far. I'm still going to go forward with the PCB respin, mainly for mechanical reasons, fixing incorrect footprints, changing part types, etc. I will keep you all updated. Thanks again.
-
#19 Reply
Posted by
b_force
on 30 Dec, 2017 16:06
-
NEVER forget grid stoppers. Very important for the pre-amp tubes as well!
Especially for guitar amps because you can get pretty nasty distortion.
more information;
http://valvewizard.co.uk/gridstopper.htmlFor guitar amps it's even better to use a slightly higher value.
I actually really recommended reading Merlin Blencows books; "Designing Tube Preamps for Guitar and Bass, 2nd edition".
A must read, very easy to follow.