SA-9800 PCB Layout Info

[TalYWaun]

I hope this doesn’t fall foul with the mods as I started it in Solid State before realising it Should go here.

So here is layout info for the Protection and Power Supply boards (UK variants).

The transistors and caps are on order and will work through them as I’m replacing the parts (as there are probably a few mistakes).

 

[TalYWaun]

The story so far.

All the caps and transistors replaced on the Power Board. Put it back in the chassis but some reference voltages incorrect/intermittent. Every time a probe touched the board I could hear arcing. When I was replacing the transistors I noticed that sometimes desoldering one leg would be enough to lift the others. The trackwork was OK but many of the solder pads were lifting off the board. Even A good look through the microscope did didn’t show any obvious problems. So retouched all the solder joints. On powering it up again I had the same problem (I suspected a cracked track, but never found one). So retracked the board and as some of the wire wrap ends were getting short I replaced the posts with terminal blocks. Not ideal, I know, and if I can get the unit working again I will put the circuit into OrCAD/Altium and have a new board made and the terminal blocks will make it easy to swap between boards.

So the reference voltages are now all good but no activation of the protection relay. Found that one of the Power Amp boards is returning 50 Volts, so time to get intimate with another PCB.

Layout to follow.

 

[rcs16]

orcad and altuim are 2 different s/w packages. I can help you with orcad, what version?
Isolate the power supplies from the loads so you can get them working first and check loads for shorts before connecting them up.
check out the other NSA PA type amp threads. SA-8800

 

[QSilver]

A new board design for the 9800 would be a good idea as these boards are almost always badly damaged from all the heat being pushed through them from being mounted upside down. Some additional modifications to the power supply would also benefit the fluroscan drive (to help prevent the dimming and drive the fluroscan correctly, pioneer did a bad job on this one). It would be well worth incorporating those improvements.

Also mounting Q11 & Q12 elsewhere would be a big positive step, redesigning the power circuit for the pilot lamp to run with an LED would also be big helps.

 

[TalYWaun]

>rcs16
The Power Amp board is out and everything I have checked so far seems OK. Perhaps my component tester doesn’t have enough voltage to really test the components. So my next step is to extend the wires and run it on the bench where I can go through the circuit in its powered state.

Thanks for the offer of help but I should be OK as I do the layouts for a lighting controller manufacturer (architectural and theatrical systems). I have v16.6 (on two machines) and v17.2 (on another) but try not to use 17.2 as a layout opened in 17.2 can’t then be opened in 16.6 and I don’t want to replace the 32bit data sources on the v16.6 machines as it’s needed for some legacy programs.

I have started entering the schematic into Altium. I used Altium before my employer decided we had to use OrCAD, so have been using that for the last few years and could do with brushing up on my Altium skills. Altium’s all in one, seamless interface is such a joy after using OrCAD, it behaves like it was designed by engineers for engineers, OrCAD by a succession of unhappy programmers on work experience who couldn’t even spell integrated.

>QSilver
Pilot light to LED – LOL. Already thought of this. I wanted to fit a blue LED (I used to build AVI Lab Series amps) and always liked their blue indicator LEDs.

Putting a blue LED behind the orange cover doesn’t work so my plan b may be to drill a hole in it and poke the LED though it. But don’t think it will look ‘right’. A red or orange LED might work but I have my heart set on a blue one to match the display. Need to find a solution – maybe use a light pipe to replace the original cover?

Not so much a new design more a respin of the original using modern parts. Making it a two layer board with ground on one side will free up some real estate for moving some bits around/thicker tracks so will have a look at your suggestion. Will post the gerbers when I get them done.

 

[TalYWaun]

Hi All.
My contemporary interpretation of the Power Supply Board is on-going but have hit the common question.
Has the 2SK34 replacement problem ever been definitively solved?
From what I have read a suitable replacement is BF256B, which is available on Mouser and looks like it fulfils the specs. I will of course test it in my existing Power Supply board (assuming I get the Power Amp board working), but am wondering if there is anything else I should consider?
Thanks

 

[rcs16]

mouser has constant current sources, pick one that is around 2mA.

 

[QSilver]

I'd say yes, its permanently solved with a current regulator diode (CRD) I think the code on mouser is E-202. If you want to be sure, Pioneer moved over to the use of the CRD's in a later amplifier model, the Pioneer A-80. The phono pre-amp power regulator board can be seen to have CRD's in place of the CCR's.

As a further note, if you can, the 17V zener and 1W 330 Ohm resistor should be removed and replaced with an additional two regulators....

 

[markthefixer]

CRD for Q6 will work, but Q5 is NOT a CRD configuration.

We usually leave the 2sk34s alone in place. They're not a high failure item EXCEPT when they are in the SX-1980 power supply in a current regulator configuration. The function of these CRD's in the power supply is HUM REJECTION in the DC used to light up the regulator. more on that..

THOSE (SX-1980) CRD replacements use the EchoWars 2 transistor current source
which has a far higher voltage tolerance than the 30v spec and 50v special factory selected 2sk34 jfets.

In the older power supplies, that current is supplied by a huge RC filter. The CRD servos out the hum instead of the filter integrating it out.

 

[TalYWaun]

The story so far.

Initial schematic complete but quickly dropping the components on the PCB shows some with the wrong footprints so need to do some checks on those.

Have added an option for an LED Pilot Lamp taking the supply from the transformer feeding the Fluorescent display. Am hoping 5-10mA won’t give it any problems.

All suggestions welcome.

 

[rcs16]

Designing the supply exactly as Pioneer has done is not what i would call optimum. One BIG missing is over temp, current protection/shutdown.
Another thing that I suggest that you do is simulate the design in ltspice, that way you have a better idea of performance, power dissipation of devices.
Precision IC regulators were not available when this circuit was designed. You could look at a TL783,(replaces Q1,3,5,7 etc) it is a perfect HV regulator. you can track it as you are doing. possible to use LM317/337 as floating regulators for lower voltages.
Using above will allow for bigger heatsinks and make the layout much easier.

Beef up the heatsinks, that means making symbols/footprints for them, that way the Tj run lower and the devices are more reliable.

 

[TalYWaun]

OK, better fess up.
I can do digital and power but the subtleties of redesigning a low noise power supply is currently beyond me. For now I just want something that I can use to replace the mess of a board currently in my amp.
Using ground planes on the top of the PCB reduces the number and complexity of the tracks on the original board. I had to move J8 but as it’s a Ground that isn’t going to cause any major problems.
The TO-220’s are nearer the inside edge of the board and have bigger heatsinks plus I will connect them to some (isolated) copper fills that should help dissipate even more heat.
Now I can see where there’s space I can spread the components out a bit more and maybe get the TO-220’s even closer to the edge.

 

[rcs16]

I would not count on heat thru the leads conducting to pcb copper as a an effective heatsink, you are not using a smt packages such as Dtab.
A PS designer would usually figure out Pd of each device and calculate your target Tj (reliability) based on heatsinks and package specs.
Suggest to use terminal block(s) to connect your wires, as was done for the SX-1980 PS re-design. use ferrules over the wires to insert in the TB positions.

 

[TalYWaun]

Fair points, which is why I have put the tang of the heatsink on the same net as the collector (pin2). Pins 1&3 have their own fills with pin2&heatsink on another larger one. Although the tang on the heatsink I have found isn’t as large as I would like (but am currently limiting my choices to the mouser ‘catalogue’).

In work we use up to 60A devices (used on phase cut dimmers) and have IR camera data showing the leads do conduct significant amounts of heat to the copper, perhaps it’s just the heat of the transistor body but it’s still heat, so why not spread it out if you can?

Your suggestion on using terminal blocks surprises me. I don’t have any experience with wire wrapped connections but have read up on them. Their cold welding to the posts and resistance to oxidisation made me think that terminal blocks are a less than optimal solution. Yes, they make life simpler but a better solution? I wasn’t sure. Thanks, now I feel better using them and have used them on the schematic.

Ferrules? OK, using them on the few connections that use stranded wire makes sense but as most of the wires are solid I don’t see the advantage to use them on those, as hopefully any change of the PSU board is a once in a lifetime event.

The only major item remaining is the transformer. Does anyone have one that they can measure so that I can produce a footprint? I really don’t want to have to remove my amp’s PSU board again just to measure the distance between the pins.

I have attached the Altium files, as is, at the moment (well I would have if the file types were allowed, but they are not - Anyone know if I can link to files in my Google Drive?). When I get a finalised version I will post the project files (in text format so that the schematic can be read into OrCAD), Gerber, XY and BOM info I send to my local PCB manufacturer. That way anyone who wants to make a new Power Supply board can get them made (I deliberately didn’t use SMD devices so that the project is ‘easy’ to construct).

 

[rcs16]

You need large copper areas to cool devices, best is direct tab soldering, copper lands becomes diminishing returns unless you have airflow, more efficient using a proper HS if possible. Hot cooper could require higher Tg material due to de-lamination issues
If you do not like terminal blocks you can go back to direct soldering or w/w posts as original, but they are good for isolation in first time power up testing and isolation if you have shorted loads
axial ecaps limit your availability of lower esr, higher ripple current devices which are the preferred parts to use (radial) plus they save a lot of pcb space/area unless you have height restrictions, even then you can parallel smaller ecaps which is even better for specs but more $
Do I see pig tail fuses? why not use fuse clips as original. fuses blow, you do not want to have to un-solder a fuse if at all possible. you can still solder a pig tail if you do not trust fuse clips
I would think that you should have the original PS assembly in your hand to use as your template, measure mounting holes. You can print out your layout and over lay it to verify your placement of tooling/assembly holes for mounting. Most important is that the existing wires can mate correctly with your placement and do not require wire extensions if at all possible.
once in your hand you can measure the transformer size for a footprint. might want to accommodate an modern day sub using a dual footprint arrangement so that if the transformer blows you can source a new one.
I can look at your fab data files when done, i do not need Altium files as I do not use it.

 

[TalYWaun]

All the i’s dotted, now to finish crossing the t’s.

The fuse’s are 20mm fuse holders (10A rated), I would have liked some larger tangs but they will have to do.

Have measured up the transformer but that’s academic until I can find a modern equivalent, so it’s just a guide at the moment. Currently shifting everything to the left so there’s room for the transformer and the optional LED power supply components, the screw holes and anything else that needs to be added.

Red – top layer Blue – bottom layer (have checked with my PCB supplier and there is no difference in price between 1 and 2 layer. 4 layer (which could be handy) more than doubles the price, so not going there).

So the big question now is the colour of the resist and silk screen – Am thinking of black with yellow silk. It’s a labour of love so why not make it pretty?


The data so far – decode it for the raw data (if it gets past the sites filters, and you can):

https(colon)//drive(dot)google(dot)com/open?id=1X6If7Y8kpQZS6-seUAiS-6TgsLIzcXrd

 

[TalYWaun]

Final prototype info done (now to get back to working on my Power Amp Bd).

Altium project and Gerber data available on my Google Drive.

Gerber’s ready to send to PCB manufacturer but will hold off until the 24th in case anyone spots something that needs changing.

Altium schematic also saved in ASCII format if anyone wants to load it into OrCAD.

 

[QSilver]

I should be able to confirm the size of the fluroscan transformer for you sometime soon.

D10 looks to be wrong however... I checked the part and it came out at a 6V Zener. The Zener in this position should be 17V with a 330R 1W resistor in series before it connected to the regulated output of Q13/Q11. This feeds the drive circuitry for the VFD and a voltage to illuminate TAPE/TUNER/AUX etc IIRC

D10 would be best replaced with a simple emitter flower 18V regulator.

In addition to that, the off-board resistor R5 (2.2K) on some power boards, is actually two resistors. A 1K and a 1.2K resistor. A tap is taken from between the two and fed to the protection circuit. This a a factory modification by Pioneer and so an additional binding post between these two resistors for the wire to the protection circuit would be really helpful in tidying everything up.

Finally, if there is room, you could fit an adjustable regulator that is supplied by the J30 rail that feeds the fluroscan grid voltage. Pioneer should have included a voltage following regulator in order to better run the VFD however the circuit they implemented is flawed and is one reason the tube can be over driven and die. An emitter follwer with an adjustment pot is what I have see recommended here.

I hope this helps! Most of these modifications have already been mentioned by other members like MTF who have far more experience of these amps than I do.

 

[TalYWaun]

Thank you for taking the time to look over the schematic. Nice catch on my mistake on D10. On my board (AWR-196-) the 330R resistor (R3) is off the board, but note that on the US version (AWR-194-) it is on the board as R20. Will add that to the schematic and BOM with a warning to check which variant of board is being replaced.

Am looking into making it an emitter follower but the position of D10 has to be the worst possible place to try to make a change from both the space and heat perspectives. My thinking is Q11-14 need to stay where they are (near the edge of the board close to the central cooling ventilation). So D10, the transistor and resistors would need to move to the other side of them. The components below Q11-14 could be squashed down and right and then bring D10 down near J1-4. So that just leaves how to thread J6&7 between Q14 and Q11.

Will split R5 and add an extra terminal J33 (ah – a nice easy one).

“Finally, if there is room, you could fit an adjustable regulator that is supplied by the J30 rail”
OK, I’m not sure what is going on here. Why off J30? Why not off the original supply J18?
Space isn’t a problem above C2&3 so will try and find the posts you mention.

Not going to make any (serious) changes for a few days as I need to get the Power Amp board problem fixed and working out the layout on that board is a real headache.

 

[QSilver]

OK, I’m not sure what is going on here. Why off J30? Why not off the original supply J18?

The only reason being that at J30, the AC supply has been rectified already by D8 & D9. Another reason is that the J30 IIRC is mostly for control circuitry and not audio so putting the VFD grid on this keeps the supplies for the amplifier sections away from noise.

Just another thing worth mentioning. Q1 and Q2 in their TO-126 packages do still get noticeably hot when in operation so might be something to just keep an eye on during building/moving components as these need good airflow too.

I have in the past, used 3-Pin headers to connect Q11 & Q12 and attach these to bigger heatsinks elsewhere, then removed Q13 and Q14 as their main purpose is to spread out the load and heat. This would free up more board space, but require more time migrating the transistors to heatsinks. I'm not sure what your thoughts are on this but I thought it might be worth consideration.