Jensen as017 preamp Adaptation

[Icegoldnixon]

You should really check the pitch of the parts you are using.

What makes you say that? I believe I've matched all of the footprints to the actual parts I plan to use. Does something look suspect to you?

 

[Icegoldnixon]

Here's a 'final' PCB unless people have thoughts on the zobel network issue. Maybe I should make a version with a footprint to accommodate the actual Jensen transformer to make it useful to other folks. What do you all think of that? Happy 4th!

 

[moamps]

What makes you say that? I believe I've matched all of the footprints to the actual parts I plan to use. Does something look suspect to you?

small power resistors pitch is usually 10mm
cog/npo, small MKT caps pitch is usually 2,5 or 5mm
elco pitch for 25V is usually 2,5 or 5mm
C7 is backward!!!!!
power connector's pitch is too small, move it to right
L1, R8, R9 should go to SGND
feedback track from pin 6 of IC is too long and too close to pin 3
lot of space on board is empty

 

[Icegoldnixon]

small power resistors pitch is usually 10mm
cog/npo, small MKT caps pitch is usually 2,5 or 5mm
elco pitch for 25V is usually 2,5 or 5mm
C7 is backward!!!!!
power connector's pitch is too small, move it to right
L1, R8, R9 should go to SGND
feedback track from pin 6 of IC is too long and too close to pin 3
lot of space on board is empty

Well the pitches are all matched to parts, so maybe I used atypical components for those.
Except for the power connector, I don't have a part picked out. Do you have a recommendation?
C7 is backward? I suppose you're right, when I laid this out I was using nonpolar caps.
I'm still confused about the gnd thing! The schematic definitely has R8, R9 not on SGND. Why do you say that?

I'm thinking of redoing a lot of this to make a 2-layer board, which might help reduce the length of some runs. would that be a better idea? Thanks all!

 

[ijzerpro]

If you go to do some mod's on your PCB .
Red is the top layer ( component side ) , green is the bottom layer in kicad.
It is very simple in Kicad to swop the layers.

 

[Icegoldnixon]

I've done a modest 2-layer version that shortens the routing in some spots I think. It's smaller too, and certainly could get smaller.
I'm mostly preoccupied with the zobel network issue, though if this layout would work with the Jensen transformer I might just order those to get this built.
I haven't done the back copper fill yet, but I think it would be one solid plane connected to DGND with a via.  Thoughts on that are welcome. Thanks!

 

[abbey road d enfer]

I'm mostly preoccupied with the zobel network issue, though if this layout would work with the Jensen transformer I might just order those to get this built.

I believe I already wrote several posts back that the Zobel network has to be tailored to the actual transformer, and that the best way is to do it while actually measuring the finished circuit, operating in its normal use conditions, particularly regarding the source impedance. Nobody can do that for you, particularly at a distance. Anyway, the Zobel network is always composed of a resistor and a capacitor in series, the typical value of the cap being between a few hundred picofarad and a few nanofarad, so you can guesstimate its actual size.
I would implement a multi-footpring capacitor capable of receiving 5mm, 7.5mm and 10mm sizes.

 

[Icegoldnixon]

I believe I already wrote several posts back that the Zobel network has to be tailored to the actual transformer, and that the best way is to do it while actually measuring the finished circuit, operating in its normal use conditions, particularly regarding the source impedance.

Ah yes, looking back you mentioned it would need to be "adjusted" but I wasn't sure if that meant calculating new values before putting it in the circuit or tuning it once built. I'll try the procedure described here?
https://groupdiy.com/index.php?topic=32441.0

 

[moamps]

I'm still confused about the gnd thing! The schematic definitely has R8, R9 not on SGND. Why do you say that?

I did a mistake. L2, R8 and R9 should be connected to SGND instead to PGND.
Here is an idea how I would do that board. It's the first, not the final version.