diyAudio

diyAudio (http://www.diyaudio.com/forums/)
-   Chip Amps (http://www.diyaudio.com/forums/chip-amps/)
-   -   My_Ref Fremen Edition - need help on PCB evaluation (http://www.diyaudio.com/forums/chip-amps/197120-my_ref-fremen-edition-need-help-pcb-evaluation.html)

ClaveFremen 22nd September 2011 09:34 PM

My_Ref Fremen Edition
 
2 Attachment(s)
This thread starts to discuss a variation of Mauro Penasa's My_Ref with this goals:
  • a more stable and performing amp using SMD parts
  • raise LM318's PS voltage thanks to a voltage limiter
  • Better PS for LM318
So I've designed (starting from Russ White's Eagle schematic) a brand new (and untested) PCB with these features:

  • bigger caps (16mm diameter with both 7 and 5 mm pads) for C1, C2, C9
  • large use of SMD components
  • all small caps and some critical resistors are still through-hole
  • the feedback resistor (R7) can be through hole or MELF
  • very small paths thanks to SMD
  • ground planes in star configuration
  • zener limiter based on schematic 5b from this link (which seems pretty similar to My_Evo one)
  • a double diode bridge like in most gainclones (tested by Suburra with great results)
Both PCB and schematic are untested and prone to errors so any comment, fix, suggestion on both is welcome and appreciated.

I've been authorized by Mauro Penasa to proceed with this My_Ref derivate amp.

Mauro also pointed out some minor glitches that should have been fixed in the attached schematic.

Also, we will discuss on a better performing LM318's PS (at the moment the schematic include the original zener shunt supply) and, maybe, on possible mods to the compensation scheme.

I've already tried a simple TL431 peer to peer regulator that works and in theory should measure much better than zeners but in practice sounds (much) worse.

On amp's name:

  • As part of my nickname the name is an homage to Frank Herbert's Dune novel.
  • The official abbreviation for My_Ref Fremen Edition is My_Ref_FE ;)

bcmbob 22nd September 2011 10:36 PM

Very happy that Mauro is willing to offer a bit of assistance. I was beginning to believe he was just a figment of someones imagination. Hopefully many will post here and enjoy working on the development level of this project.

Thanks again for your efforts - both Dario and Mauro!

ClaveFremen 22nd September 2011 10:48 PM

Quote:

Originally Posted by bcmbob (Post 2720743)
Very happy that Mauro is willing to offer a bit of assistance. I was beginning to believe he was just a figment of someones imagination.

Mauro exists, be sure... :D

But the fact he kindly asnwered my mail and gave permission doesn't mean he is willing to offer assistance.

Obviuosly if it will ever happen I'll be happy and honored. ;)

Quote:

Originally Posted by bcmbob (Post 2720743)
Hopefully many will post here and enjoy working on the development level of this project.

I hope so... :)

Quote:

Originally Posted by bcmbob (Post 2720743)
Thanks again for your efforts

You're welcome, Bob :)

soongsc 23rd September 2011 12:15 AM

I am going to try these on the original Rev C for LM3886 PS
?????? AD6-11242411B A6-11242411B ????? DC24V 1.1A x2 ???????
Do not think there will be a ground problem, but we shall see.
It will also be interesting to see if the EMI will effect the circuit or not. Local EMI radiation seemed to be within standards here.

linuxguru 23rd September 2011 08:04 AM

Quote:

Originally Posted by ClaveFremen (Post 2720683)
...
I've been authorized by Mauro Penasa to proceed with this My_Ref derivate amp.
...
  • As part of my nickname the name is an homage to Frank Herbert's Dune novel.
  • The official abbreviation for My_Ref Fremen Edition is My_Ref_FE ;)

Dario - great and way cool!

Good luck on the design and layout - I'll try to contribute my 2c from time to time.
I've started running simulations, but the NatSemi LM318 model is an incomplete behavioural model which doesn't model external compensation through the comp pin. I'm trying to find a component-level model which can be modified.

ClaveFremen 23rd September 2011 08:57 AM

Quote:

Originally Posted by linuxguru (Post 2721166)
Dario - great and way cool!

Good luck on the design and layout - I'll try to contribute my 2c from time to time.

Hi Siva,

thanks :)

Your contribution will be precious.

Quote:

Originally Posted by linuxguru (Post 2721166)
I've started running simulations, but the NatSemi LM318 model is an incomplete behavioural model which doesn't model external compensation through the comp pin. I'm trying to find a component-level model which can be modified.

It would be great!

Pixo 23rd September 2011 05:58 PM

1 Attachment(s)
That's a very nice layout. since you're now designing the PCB from the ground up, i thought i'd suggest another way of placing the components. I see you're good at copper pours, so this shouldn't be a problem. One benefit would be that the large capacitors won't be in the way of a screw driver when you try to mount the chip onto the heatsink.

madisonears 23rd September 2011 09:12 PM

Dario,

I'm new to this, so I don't know if I'm reading the color coding correctly. If a thin white border represents isolation from the ground plane, then look at the pads of R10 and R13. I think you have the wrong end isolated from ground. Is R12 isolated?

What are D7 and D8 connected to on the ground end? I see white borders around their pads, too. Am I interpreting this wrong?

I see you've eliminated the bypass cap from C9. There was a lot of discussion about that, so it might be nice to leave the option there if you can fit it in. Other than space, it doesn't hurt anything to have extra pads and a small trace.

You do not want to move the big PS caps, as they provide some physical blocking of AC section from the signal area. I don't know if that's really important for the low noise level this amp exhibits, but why mess with it? We know there are ways to mount the chip after the caps are in place.

Why does the signal input trace now cross underneath R10? Perhaps the input pads should be moved back to be next to C13. Can you put R10 at a 45 degree angle?

There is not much space around R3 if people want to use bulk metal foil resistor with a heatsink there. It's very tight on the old board, and this looks even tighter.

R7 is in the way if C9 is bigger. Is there an extra pad under R7? Hard to see what's going on there.

There is a single pad below R11. I think it says C11.

I'm trying to digest all the changes you made. Sorry I can't help much with the circuit itself.

Peace,
Tom E

ClaveFremen 23rd September 2011 10:45 PM

1 Attachment(s)
Quote:

Originally Posted by Pixo (Post 2721617)
That's a very nice layout.

Thanks :)

Quote:

Originally Posted by Pixo (Post 2721617)
i thought i'd suggest another way of placing the components.
...
One benefit would be that the large capacitors won't be in the way of a screw driver when you try to mount the chip onto the heatsink.

When I've first tried to arrange components on the PCB I've tried also that solution but it wasted too much space... and as Madisonears pointed out the possible screening offered by the big smothing caps from both the diode bridge and the relay coil is lost.

BTW I'll check again.

Quote:

Originally Posted by madisonears (Post 2721782)
I'm new to this, so I don't know if I'm reading the color coding correctly. If a thin white border represents isolation from the ground plane, then look at the pads of R10 and R13. I think you have the wrong end isolated from ground. Is R12 isolated?

What are D7 and D8 connected to on the ground end? I see white borders around their pads, too. Am I interpreting this wrong?

Hi Tom,

Take a look at the attached detail, the white borders are termal pads (easier to solder and, eventually, desolder)

Red represents the top layer, blue the bottom one.

Darker red are tracks overlapped by the other layer.

Quote:

Originally Posted by madisonears (Post 2721782)
I see you've eliminated the bypass cap from C9. There was a lot of discussion about that, so it might be nice to leave the option there if you can fit it in.

Right, I'll check if it's possible the use of a TH cap without disrupting current return paths.

A SMD position is possible and I've added it, as you can see in the attachment.

Quote:

Originally Posted by madisonears (Post 2721782)
IYou do not want to move the big PS caps, as they provide some physical blocking of AC section from the signal area. I don't know if that's really important for the low noise level this amp exhibits, but why mess with it? We know there are ways to mount the chip after the caps are in place.

As I wrote above I do agree but I'll do a rapid check, just to be sure.

Quote:

Originally Posted by madisonears (Post 2721782)
IWhy does the signal input trace now cross underneath R10? Perhaps the input pads should be moved back to be next to C13. Can you put R10 at a 45 degree angle?

Initially it was so but I've arranged things this way to gain more distance between output ground and R13 and C12.

Input signal cross R10 at 45 and this should minimize the influence.

Not sure on which solution is better (R10 not crossing input signal or R13 and C12 nearer to output ground?).

Quote:

Originally Posted by madisonears (Post 2721782)
IThere is not much space around R3 if people want to use bulk metal foil resistor with a heatsink there. It's very tight on the old board, and this looks even tighter.

Unfortunately gainining more space is problematic but I've verified that a small heatsink like the one I've used for RevC fits well and mine gets barely warm.

As you can see in the attachment such heatsink now is indicated in the silk-screen.

Quote:

Originally Posted by madisonears (Post 2721782)
R7 is in the way if C9 is bigger. Is there an extra pad under R7? Hard to see what's going on there.

See the pic.

There are two alternatives:

  • R7 can be monted on bottom side
  • there is a position for an alternate MELF R7 (between R7 and C32)
Carbon films are available in MELF packaging.

The use of the MELF R7 shortens a lot the feedback loop.

Quote:

Originally Posted by madisonears (Post 2721782)
There is a single pad below R11. I think it says C11.

The 'C11' label is wrongly placed, it refers to the elco below.

That pad is a via between layers.

Quote:

Originally Posted by madisonears (Post 2721782)
II'm trying to digest all the changes you made. Sorry I can't help much with the circuit itself.

Any feedback is useful and welcome. ;)

ClaveFremen 23rd September 2011 11:00 PM

1 Attachment(s)
Quote:

Originally Posted by ClaveFremen (Post 2721855)
When I've first tried to arrange components on the PCB I've tried also that solution but it wasted too much space... and as Madisonears pointed out the possible screening offered by the big smothing caps from both the diode bridge and the relay coil is lost.

BTW I'll check again.

Sorry but, as you can see in the attachment, the radiating tracks of the diode bridge are too near to the 0V zone....

And lack of space is greater...

If the PCB will grow in dimension (but I should buy Eagle Hobbyst Edition... 160€) this option will come back.


All times are GMT. The time now is 11:45 PM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio


Content Relevant URLs by vBSEO 3.3.2