• These commercial threads are for private transactions. diyAudio.com provides these forums for the convenience of our members, but makes no warranty nor assumes any responsibility. We do not vet any members, use of this facility is at your own risk. Customers can post any issues in those threads as long as it is done in a civil manner. All diyAudio rules about conduct apply and will be enforced.

GB for DC coupled B1 buffer with shunt PSUs

Disabled Account
Joined 2002
Very nice ! As it seems a heatsink is not really needed unless people want to use the power supply PCB for purposes other than B1. So if you change this the PCB will be more versatile. If changing the design will compromise performance please do not even bother to change it !

Some comments:

The clearance between the right FETs and the 68 Ohm resistors is not enough for a heatsink to fit I think. Also clearence between the left FETs and the mounting hole is tight. When the PCB is mounted the screw will touch the heatsink. Maybe Salas can comment on the gate stoppers as the FETs have been turned around ? I think it looks better and it makes mounting more easy with no negative side effects but i could be wrong. Maybe the gate stopper at the lower left side near the IRFP240 could be placed more optimal when the small transistors are turned 180 degrees CCW.

Please move the outputs of the buffer to the right side and add decoupling caps on the power lines. IMO the buffer board should be separate from the supply board in this particular case for optimal results. If the buffer PCB could be somewhat larger the routing of input- and output pads could be more optimal. I would design the PCB for using Phoenix connectors for power supply lines but this a personal choice. However, my own design is far from ready and severe lack of time makes matters worse. Even in this current design stage I would like to use your design.

I will not mention adding a volume potentiometer, I promise ;)
 
diyAudio Chief Moderator
Joined 2002
Paid Member
xaudiox said:
How about this guys?
please check if theres any errors.. thanks

Hello, thanks for your effort. The resistor pairs which are designated 34R, must change to 68R. We don't need the 3rd hole between them. Any current can be set with one or two resistors.

Is there a silkscreen layer too? Should mention DC Coupled Pass B1 with symmetrical shunts by Salas. PCB by XaudioX. It is good to mention on the copper side too. There are Ebay vendors out there...

The shunt must stay physically in contact with the buffer in the tightest way possible for lowest output impedance. Same board and no connectors and wiring is optimum.

As for the Mosfets having their backs facing outside, you arranged them well enough, maybe the lower left 470R isn't that tightly coupled but I don't think that it will lead to oscillation either. A secure step is to use carbon resistors for the 470Rs. Now with the Mosfets having a natural distance in leg height from the PCB, light off board sinks can be used, but not for heavy current.
 
thanks guys.. this is what i've done so far,.. i'll continue to work on it tomorrow...thanks

b1-2.png
 
Member
Joined 2003
Paid Member
That pcb design is a fine job indeed.

I would like to suggest to separate the common ground trace into two parallel ground traces. They would connect at the bridge (see below) and at the buffer side. This might require to expand the width of the pcb from 1,75 to say 1.8 inch (Edit: in the version of post 124 this might even fit as is).
This has advantages:
- lower inductance of the ground connection
- option to split the pcb and mount them for instance above each other where space is limited (if you would first separate the buffer from the supply, of course)
- enable those who prefer to use a separate bridge for plus and for minus (you only would have to hard wire the two bridges separately ( it might be possible to fit this also on the pcb but it will complicate unnecessarily. I do not propose that). You then may separate the connection of the ground traces at the current bridge side (it can even be layed out as a wire connection), and the positive and negative regulator would only meet at the buffer so there is a maximum of separation in regulation.

Thanks again for the patience, Arjen.
 
Disabled Account
Joined 2002
The PCB got better. Thanks for moving outputs to the right and adding 2 decoupling caps on the power lines. You could omit the upper and lower connections to the inputs as they are double now. The further they are separated from the outputs the better it is. I only have one remark concerning the stopper resistors for input and output. They are very close together. Omitting the upper and lower pads for inputs will make room for separating the 4 resistors a bit from eachother.

I wouldn't change the power supply part again as it looks quite optimal as it is now. Maybe there is a slight advantage by moving the 3 LEDs and the K170 a little more to the 4700 uF cap/100 nF cap. The 10 Ohm resistors could also move a little which leaves space for a 100 nf parallel to the 100 uF caps.

Salas wrote:"The shunt must stay physically in contact with the buffer in the tightest way possible for lowest output impedance. Same board and no connectors and wiring is optimum."

Which can be explained as:"make it just one PCB" so scoring is not really necessary. So 2 mounting holes can be omitted and power supply and ground jumpers can be omitted too. The power supply lines can be routed somewhat closer to eachother as well in that case. In the end you will have more board space to the right so larger pads can be used for the inputs...

Thank you for your effort !
 
diyAudio Chief Moderator
Joined 2002
Paid Member
If the mosfets can go further up n' down right along the pcb's edges it will help the shunt only fans for big common sinking. Also it would be very easy to bend and mount on the chassis floor. Very good sinking for up to 200mA per rail, no sinks. Only silicon pads. TO-247 gets metal screws without insulation. Since this is double sided, I think it can be arranged. Thanks.
 
I cannot check out from the monitor, but I would like to point out:

> the two 4700uF/25V caps in the raw ps should be 18 mm diam. 7.5 mm pitch to accomodate Panasonic FC

> the two 68 R in // on each side must have 12.5 mm (.5 ') pitch to easily accomodate 1/2 W resistors (the space between pads seems to be 10 mm, but I might be wrong)

> the two 100uF25 V output caps must have 10 mm diam. 5 mm pitch to accomodate Elna Silmic II (they looks much smaller than that) Yes, you can use 16 V caps, but 25 V are much easier to find (digikey has 25 V and 35 V only). Try to put them closer to the buffer stage.

> try to connect the gate stopper of the lower left mosfet in a different way, as already poited out.

P.S. A double sided pcb will cost more than a single sided one ;)
 
Ex-Moderator R.I.P.
Joined 2005
massimo said:

P.S. A double sided pcb will cost more than a single sided one ;)


I thought about that issue too
I found only a few connections with a need for double sided
With some care they could easily be jumpers, on a single sided board

Though with this many boards, I wouldnt expect cost to be much
But some have ordered more boards, and they would be hurt by it


But nice work, trying to make it the best possible, thanks :)
 
good morning guys..

thanks for all your replies.. i tried to accommodate all request/suggestions..

100uf > 5mm pitch 10mm dia
4700uf > 7.5mm pitch 18mm dia
68R > 0.5in (500mils) pitch

i also move the mosfets abit closer to the edge of the pcb as suggested by salas..

i added copper slot in the supply line.. you can just solder them (bridged).

additional 100nf caps for the 100uf..

red color > top layer
blue color > bottom layer

b1-3.png

b1-silk.png


thanks
 
diyAudio Chief Moderator
Joined 2002
Paid Member
So, input goes from RCA via a coaxial to a chassis mounted 22k log pot's leg 1 and pot's leg 3 (gnd), and from pot's leg 2 and 3 a coaxial goes to in, gnd. Ditto for channel 2. On first look does not seem to have errors, but I will look at it again with clearer head. I suggest a few more hawk eyes to double check. Link to circuits. I see enough clear space between the 100nF caps and 4700uF ones for some lettering. ''Pass B1 DC & Shunts by Salas. PCB XaudioX''. Does it take it?
 
Just a suggestion,

If you were to move the main central 0volt track to the bottom layer (blue) and add a link for the ac diode, would avoid relying on print thru connections for the electro caps at 4700uF, the terminal block and especially at the o/p 100uF - could then use top layer for other 0volt connections via resistor leads (not transistors legs) - many of us will change componenets quite a bit and the first" casualties" are the print thru sleeves and much agro!

On the -ve CCS (at the IRFP), can reroute the bottom layer and avoid the top track and also, by standing up the neg shunt IRFP's gate resistor avoid the whole top layer altogether apart from the +ve CCS (you could run the main rail along the outside of the shunt IRFP's pins, rather than thru the middle.

Not as neat, but would make it a easier to fit up and perhaps be more reliable in practice. Might need to increase the boards width a bit, too (just a few mm)

The legs on the IRFP's are quite long and it's easy to just bend the big fet outwards clear of the pcb's edge for heatsink mounting, or flat down "on their backs" - they're pretty tough things.

On the buffer, it's generally considered good practice to physically tie the 2sk170 fets together (left and right) as they stay warmer (good for sound) and track better (better balance, image, etc).
However, this isn't easy with the current layout, but with a bit of a fiddle, can adjust the 2 fets of each channel "face - face" and gain some benefit of the mutual heating ("tie wrap" together with a bit of "white goo" or Arctic Silver)

Xaudiox, hope this may be useful ...
 
diyAudio Chief Moderator
Joined 2002
Paid Member
In direct coupled B1 I have not seen any output dc offset drift even without tight face to face physical coupling of the JFETs, don't worry about it. This helps in differential amplifier couples with large gain. Here the auto feedback is 100% and gain just a tad less than 1. Keeps things calm.