AD8610, OPA134, OPA627, BUF634 SMD headphone amp - Page 2 - diyAudio
Go Back   Home > Forums > Amplifiers > Headphone Systems

Headphone Systems Everything to do with Headphones

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 17th April 2003, 10:12 PM   #11
PMA is offline PMA  Europe
diyAudio Member
 
PMA's Avatar
 
Join Date: Apr 2002
Location: Prague
peranders,

try AD825 (excellent) and OPA602. My schematic is at http://web.telecom.cz/macura/buffer_en.html
  Reply With Quote
Old 18th April 2003, 05:30 AM   #12
dimitri is offline dimitri  United States
diyAudio Member
 
dimitri's Avatar
 
Join Date: Oct 2002
Location: retired
Send a message via ICQ to dimitri
Here is Ben Duncan amp where buffers aren't in the loop
Attached Images
File Type: gif duncan.gif (10.5 KB, 3550 views)
  Reply With Quote
Old 18th April 2003, 06:58 AM   #13
Electrons are yellow and more is better!
diyAudio Member
 
peranders's Avatar
 
Join Date: Apr 2002
Location: Göteborg, Sweden
Blog Entries: 4
Quote:
Originally posted by PMA
Hi peranders,

this is my PCB for Audio Buffer (OA+BUF634T):
Nice pcb, but it's rather unusual to mount BUF634 in a straight line, never seen that before. I would prefer staggered pins so the distance between the pins get more. Have you tested making groundplanes, it's rather easy even if your program can't handle it.
__________________
/Per-Anders (my first name) or P-A as my friends call me
Super Regulator SSR03 Group buy
  Reply With Quote
Old 18th April 2003, 07:20 AM   #14
PMA is offline PMA  Europe
diyAudio Member
 
PMA's Avatar
 
Join Date: Apr 2002
Location: Prague
peranders,

all of the BUF634T's that I have bought or obtained as samples have had TO220-5 case with five in-line pins, that is why I use in-line mount.
I have not tried ground plane yet, but I did not get into trouble with this PCB, considerable amount of measurements was done and about 20 pcs of 2-channel circuits were assemlied and proved.

Pavel
  Reply With Quote
Old 18th April 2003, 09:02 AM   #15
trwh is offline trwh  United Kingdom
diyAudio Member
 
trwh's Avatar
 
Join Date: Apr 2002
Location: UK
Hi peranders,

I just finished designing a PCB for a BUF634 / OPA2134 based headphone amp - I sent it off to the board manufacturers last week. Here is the layout for my (single sided) PCB, if anyone's interested in seeing. I would be very interested to hear your opinion of my layout, although it is too late to change anything now

See ya,
Tim.

PS - Surely using the buffer outside a feedback loop is a bad idea? Someone posted on Headwize that this topology would lead to high distortion and DC offset.
Attached Images
File Type: gif cans.gif (32.6 KB, 3350 views)
  Reply With Quote
Old 18th April 2003, 09:44 AM   #16
PMA is offline PMA  Europe
diyAudio Member
 
PMA's Avatar
 
Join Date: Apr 2002
Location: Prague
BUF634 inside feedback loop really brings better results.
  Reply With Quote
Old 18th April 2003, 05:58 PM   #17
ALW is offline ALW  United Kingdom
diyAudio Member
 
Join Date: Jun 2001
Location: UK
Default Tim

Quote:
I would be very interested to hear your opinion of my layout, although it is too late to change anything now
The most obvious thing to me is that the PSU rails, as seen by U2, would seem to be modulated by the potentially significant currents drawn by the buffers.

It would have been better to star-wire the supplies, or considered a seperate low current supply for U2, IMVHO.

Some RC decoupling may be beneficial as a result of the above.

The grounding, via the large copper area is thinned by neccessity in many areas, and this is also likely to bring reference problems and potential error signals.

I'm sure it will work fine, but you may like to consider a double-sided artwork for a future variant, as this will simplify the artwork and allow you much more board area to play with and costs very little extra. I think if you were to consider all the potential error sources and address them, you will be surprised at the difference.

It's easy to forget the PCB is a critical part of your circuit diagram, that rarely shows in a SPICE model or simulation unless you put it there yourself.

Out of interest who is doing your PCB's and how much are they?

Hope that doesn't sound overly critical, it's not intended to be, PCB layout is very much a skill that get's better every time you do it. There's not a single PCB I've ever done that I would not change, if I ever re-visited it later on

Andy.
  Reply With Quote
Old 19th April 2003, 09:29 AM   #18
trwh is offline trwh  United Kingdom
diyAudio Member
 
trwh's Avatar
 
Join Date: Apr 2002
Location: UK
Thanks for your comments, ALW.

I'm sure you're right about the supply to the opamp U2. I decoupled it with a 10uF tantalum cap to ground on both supplies next to the device (C5 and C8), and I used 40 mil tracks for all the buffer's power rails. I assumed this would be sufficient, maybe not

I did think about thinning of the copper ground plane, and I took some steps to minimise it. Maybe I didn't do enough, although some of the thinning looks worse on the screen shot than I remember it being close up in my layout program.

"I'm sure it will work fine, but you may like to consider a double-sided artwork for a future variant, as this will simplify the artwork and allow you much more board area to play with and costs very little extra. I think if you were to consider all the potential error sources and address them, you will be surprised at the difference."

OK, double sided it is next time... for my board manufacturer it is significantly more expensive, though. I use PCB Pool, at: http://www.pcbpool.com/uk_index.htm - they have given me good service in the past. They charge about 40 euros for a 1 dm^2 single sided PCB on a 10WD lead time, including postage.

Thanks again,
Tim.
  Reply With Quote
Old 19th April 2003, 10:45 AM   #19
jcarr is offline jcarr  United States
diyAudio Member
 
Join Date: Jul 2002
Location: Tokyo, Japan
Tim: In addition to Andy's comments, which I agree with, in general conducted and radiated noise levels will be lower if you _make_ the ground network have as low an impedance as possible. And this usually suggests multi-layer pcbs with a solid copper pour applied to every millimeter of the board that isn't being used for traces. Certain circuit nodes may prefer not to have capacitive coupling to ground, in which case I would broach the ground layer in the immediate vicinity of the circuit node in question, and possibly add guard rings.

The ground behavior tends to be more stable if you install the power supply filter capacitors so that the return nodes to ground are all grouped in as small a loop as possible, preferably with no roundabout routes or thinned copper between. In your design, for example, I would flip C19/C20 by 180 degrees so that the ground return nodes are facing each other, and do the same for C21/C22. If you look over your design with this concept in mind, I am sure that you will see other areas which can be refined.

Regarding Per's layout, in my opinion here too not enough effort has been paid to reducing the ground network impedance. Now if you wanted to increase the track widths as much as possible, this could be a plausible reason not to install a solid poured copper ground, but as it is, this hasn't been done, either. Also, I suggest that via's are avoided as much as possible, unless there is absolutely no other way to connect the required traces and pads together.

My two cents.

regards, jonathan carr
__________________
http://www.lyraconnoisseur.com/, http://www.lyraaudio.com
  Reply With Quote
Old 19th April 2003, 11:57 AM   #20
ALW is offline ALW  United Kingdom
diyAudio Member
 
Join Date: Jun 2001
Location: UK
Default Tim

I looked at PCB-Pool for my boards, but they are, frankly, bloody expensive!

Talk (email!) Minnitron (www.minnitron.co.uk) a D/S board like yours will have a one-off NRE (tooling charge) in the order of 40ukp, but cost per board should be quite sensible (a few pounds), even for small quantities.

They offer excellent service but you'll need to send them Gerber files + NC drill data - not a problem with any of the major PCB packages.

Standard lead time is 15 working days, with modest premiums for faster service. I wouldn't use anyone else anymore, adn use them exclusively for my own, and work-related boards.

Ask for a quote for various numbers of boards, you'll be surprised how much the prices can drop for even modest quantities.

I had one batch of boards with faulty PTH holes, but these were replaced within a few days, FOC and I got to keep the faulty (but useable to me, boards.

Andy.
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
Anyone interested in PCB's for OPA627/BUF634 based headphone amp? Maxhawk Headphone Systems 39 21st February 2013 06:32 AM
OPA627 vs AD8610 Dr.H Solid State 58 8th April 2006 12:36 PM
YardBird OPA627/637 BUF634 preamp/headphone amp Russ White Headphone Systems 4 23rd November 2005 01:53 AM
OPA627/AD8610 comparison Bgt Chip Amps 5 1st June 2005 03:48 PM


New To Site? Need Help?

All times are GMT. The time now is 10:06 AM.


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