Go Back   Home > Forums > >
Home Forums Rules Articles diyAudio Store Blogs Gallery Wiki Register Donations FAQ Calendar Search Today's Posts Mark Forums Read

Headphone Systems Everything to do with Headphones

Critique my PCB! Headphone amplifier
Critique my PCB! Headphone amplifier
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 26th November 2017, 07:48 AM   #1
abza is offline abza  South Africa
diyAudio Member
 
abza's Avatar
 
Join Date: May 2014
Default Critique my PCB! Headphone amplifier

Right, as this is my first first PCB, my first time using Eagle and my first (production) headphone amplifier...

...your brutal honesty and constructive feedback will be welcome

Notes:
  • The schematic shows only the left channel (the right is identical)
  • The design uses one dual opamp for the amplification stage (OPA2227 or 1611), and a single BUF634 buffer for each channel.
  • There are three IC decoupling capacitors for each power rail - an electrolytic 100uF and two X7R SMD caps (2.2uF and 22uF). The X7Rs are placed directly under the DIP8 sockets of each IC to get nice and close to the pins.
  • The PCB - red is the top layer, blue on the bottom
  • The entire bottom layer is a ground plane, split into seperate signal ground (SGND) and power ground (GND) planes. These will merge off-board, at the power supply.
  • Most traces are 0.7mm in width, while the power traces are 1.5mm.

Apart from a general critique / trouble spotting, I've got a couple of questions:
  1. I understand the output resistors - R3 and R5 - need to dissipate a fair amount of power. Would 1/2W resistors be sufficient for this application?
  2. In an attempt to keep the ground planes unbroken, I resisted the temptation to create vias, which meant some of the traces are slightly longer than I would have liked - particularly the V+ and V- traces right at the bottom of the board. Will this present an issue? All signal traces were given priority (as short as possible).

Again, any feedback welcome.

Thanks!
Attached Images
File Type: jpg Schematic.jpg (177.6 KB, 409 views)
File Type: jpg Render Front.jpg (167.9 KB, 407 views)
File Type: jpg Render Back.jpg (90.6 KB, 379 views)
File Type: jpg PCB.jpg (211.7 KB, 384 views)
  Reply With Quote
Old 26th November 2017, 08:27 AM   #2
OlegSh is offline OlegSh
diyAudio Member
 
Join Date: Dec 2010
Location: Germany
Critique my PCB! Headphone amplifier
Let's start from the schematic first.

1. You do not need R3 at all. If you examine the reference headphone amplifier schematic in LME49600 datasheet (same IC as BUF634 inside) and similar reference schematic in the BUF634 datasheet you will notice that R3 is not there. And there is no big current flowing between the op-amp output and the buffer input to worry about.
2. RF filter at the input does not require such a huge physical size capacitor. I am sure there much smaller size parts for this.
3. I would recommend using just one ceramic decoupling capacitor instead of two per rail per IC. Also in your mostly through-hole design SMD parts look out of place. You can get small size leaded ceramic capacitors instead.

PCB:
1. Your GND plane has so many cuts and so many traces crossing those cuts that it makes the entire idea of having the GND plane useless. I recommend following the current flow along the traces to get an idea of how return current would flow. This will give you better idea how to lay out the GND plane.
2. There is no electrical connection between the power GND and signal GND which should be there for correct functioning of the amplifier.
3. When you route the supply traces keep in mind that they first go through the decoupling capacitors from big to small and only then hit the IC's pins. In your layout the supply traces first go to the IC pins and then continue to the decoupling capacitors.
4. Your schematic allows for nearly symmetric layout, which makes routing power traces more convenient along the middle of the PCB while left and right channel's signal can go along either side of the PCB. Note that the inputs are usually separate due to the use of RCA sockets, so you can use two separate input connectors and one common ground output connector.

Good luck with your project and don't give up! We all do mistakes at the beginning and have to learn to perfect our skilles.

Regards,
Oleg
  Reply With Quote
Old 26th November 2017, 09:21 AM   #3
Idiosyncrasy is offline Idiosyncrasy  Netherlands
Megahurtz
diyAudio Member
 
Join Date: Jan 2015
Critique my PCB! Headphone amplifier
Hey Abza, I agree with Oleg that the 680pF input cap can be a much smaller type, for example a surface mount C0G multilayer ceramic capacitor.

Also, if you're comfortable using SMT parts for the decoupling caps, why not do the same for the other components? That will reduce the PCB size, making it cheaper to produce and easier to fit in whatever case suits your fancy. For example, R3, R5 and the gain and feedback resistors can be replaced with high-quality thin-film (not thick-film!) SMD types. For example, the Susumu (RG series) and Panasonic thin film resistors in an SMD 1206 package are good parts and much smaller.

If you want to drive sensitive headphones or in-ears, you might want to go with a smaller isolation resistor at the output; for example, see this article. Edit: smaller values will also reduce their need to dissipate power.

I would also drop the 100μF electrolytic capacitors for the OPA2227; it won't be loaded heavily. You could use a small resistor (like 100Ω for the OPA2227, 10Ω for the BUF634) to create a low-pass filter with the decoupling capacitors. See this article from Bruce Carter, p.47, second paragraph.

Finally, put your feedback resistors as close as possible to the high-impedance inverting input pins. This helps to reduce noise, EMC pickup other nastiness.

Last edited by Idiosyncrasy; 26th November 2017 at 09:24 AM.
  Reply With Quote
Old 27th November 2017, 07:36 AM   #4
abza is offline abza  South Africa
diyAudio Member
 
abza's Avatar
 
Join Date: May 2014
@OlegSh, @Idiosyncrasy - thanks so much! All extremely valuable feedback.

Quote:
@OlegSh: Your GND plane has so many cuts and so many traces crossing those cuts that it makes the entire idea of having the GND plane useless. I recommend following the current flow along the traces to get an idea of how return current would flow. This will give you better idea how to lay out the GND plane.
Right, clearly I need to do a little more reading about how to lay traces over ground planes. Any suggestions as to example PCBs that do this well, or a tutorial that covers this?
  Reply With Quote
Old 27th November 2017, 03:26 PM   #5
abza is offline abza  South Africa
diyAudio Member
 
abza's Avatar
 
Join Date: May 2014
Next bash! Changes as per the above:
  1. Removed the resistor between the opamp and the buffer (previously R3)
  2. Removed the 2.2uF decoupling capacitors (the 22uF ones remain under each IC).
  3. Removed the 100uF decoupling caps for the OPA2227
  4. Ensured the power rails run mostly through the centre, and massively reduced the number of times traces intersect the ground planes
  5. Power now runs through the caps before entering the ICs
  6. Feedback resistors moved close to the -IN terminals of the opamp

Things that have stayed the same:
  1. I've kept the SMD IC decoupling capacitors, the enormous 680pF input capacitor and my resistor choices... purely because I have them already I also don't mind a mix of SMD/through hole components.
  2. I still haven't connected the ground planes - again, these will be merged by cable on the power supply side.

Let me know if I'm heading in the right direction - particularly when it comes to the new layout of the ground planes. But all suggestions welcome!
Attached Images
File Type: jpg Schematic-2.jpg (180.9 KB, 285 views)
File Type: jpg PCB-2.jpg (280.4 KB, 114 views)
  Reply With Quote
Old 27th November 2017, 08:42 PM   #6
OlegSh is offline OlegSh
diyAudio Member
 
Join Date: Dec 2010
Location: Germany
Critique my PCB! Headphone amplifier
This one is not much better. The reason is that power traces do not have GND plane underneath them and you still have traces crossing the cuts in the GND plane. I think moving power entry connector to the space between two BUF634 and reducing to only two electrolytic caps (one per rail) can simplify the routing of power supply network and separate it entirely from the signal network. Just make both channel's signals flow around the BUF634's. Then make one continuous GND plane under the entire board, no cuts.

Regards,
Oleg
  Reply With Quote
Old 27th November 2017, 11:07 PM   #7
Mark Whitney is online now Mark Whitney  Netherlands
diyAudio Member
 
Mark Whitney's Avatar
 
Join Date: Feb 2013
Location: Netherlands
SGND must connect to GND for the amp to work.

Try to minimize the area of the current loops and don't mix the currents in the ground plane. I have drawn some of the input, output and power loops.
Attached Images
File Type: jpg PCB-2.jpg (395.3 KB, 98 views)
__________________
Regards Mark.
  Reply With Quote
Old 28th November 2017, 01:25 AM   #8
abraxalito is online now abraxalito  United Kingdom
diyAudio Member
 
abraxalito's Avatar
 
Join Date: Sep 2007
Location: Hangzhou - Marco Polo's 'most beautiful city'. 700yrs is a long time though...
Send a message via Yahoo to abraxalito
You might find this thread, which is also about a composite headphone amp PCB useful - DIY Headphone Amp - Comments and advice appreciated

In particular I'd highlight the separation of the supplies to the opamp and output buffer through filtering. If you omit this you'll lose one of the primary advantages of going to a composite architecture IMO.
__________________
I know you think you understand what you thought I said but I'm not sure you realize that what you heard is not what I meant - Alan Greenspan
  Reply With Quote
Old 28th November 2017, 06:53 AM   #9
abza is offline abza  South Africa
diyAudio Member
 
abza's Avatar
 
Join Date: May 2014
Thank you so much, fellas!

Quote:
OlegSh: The reason is that power traces do not have GND plane underneath them...
^ Aha, okay! So basic noob question: why is it beneficial to have the power traces run directly above the GND plane?

Quote:
OlegSh: Then make one continuous GND plane under the entire board, no cuts.
^ So if I flood the entire bottom with a single GND plane, would I just dump the idea of a separate signal ground and just use the GND plane for everything instead? Or keep the signal ground traces separate by routing them on top?

Quote:
Mark Whitney: ...don't mix the currents in the ground plane...
^ Hi Mark! Could you elaborate on this a little please, or send me a link where I can find out more?

Quote:
abraxalito: ...separation of the supplies to the opamp and output buffer through filtering...
^Hi abraxalito! Unfortunately the schematic/PCB images in that thread are no longer working. Do you have any other information regarding the filtering and separation of the supply?

Thanks all
  Reply With Quote
Old 28th November 2017, 07:18 AM   #10
abraxalito is online now abraxalito  United Kingdom
diyAudio Member
 
abraxalito's Avatar
 
Join Date: Sep 2007
Location: Hangzhou - Marco Polo's 'most beautiful city'. 700yrs is a long time though...
Send a message via Yahoo to abraxalito
From reading the posts again I notice that the OP went for some polymer caps (560uF). I reckon those aren't the best bang for the buck now as Nichicon HZ caps offer similarly low ESRs but for cheaper. So my suggestion is to decouple your opamp with 1000uF/16V Nichicon HZ and feed those caps from the BUF634 rails via SLF7045-102 (1mH TDK inductors).
__________________
I know you think you understand what you thought I said but I'm not sure you realize that what you heard is not what I meant - Alan Greenspan
  Reply With Quote

Reply


Critique my PCB! Headphone amplifierHide 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

Forum Jump

Similar Threads
Thread Thread Starter Forum Replies Last Post
AB amplifier is oscillating. seeking critique jlny Solid State 56 13th February 2016 02:06 PM
Critique this noninverting opamp buffer/amplifier please? Almost time to build... audiovisceral Analog Line Level 87 2nd March 2015 05:25 PM
Headphone Impedance and headphone amplifier TheGimp Tubes / Valves 89 3rd May 2014 01:46 PM
Headphone amplifier audiofan Headphone Systems 5 3rd March 2006 03:43 PM
Please critique my Class A amplifier!! AudioGeek Solid State 2 28th July 2004 08:02 PM


New To Site? Need Help?

All times are GMT. The time now is 11:00 AM.


Search Engine Optimisation provided by DragonByte SEO (Pro) - vBulletin Mods & Addons Copyright © 2018 DragonByte Technologies Ltd.
Resources saved on this page: MySQL 15.00%
vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2018 DragonByte Technologies Ltd.
Copyright ©1999-2018 diyAudio
Wiki