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

Analog Line Level Preamplifiers , Passive Pre-amps, Crossovers, etc.

Laying out preamp pcb
Laying out preamp pcb
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 6th December 2017, 11:31 PM   #21
gfiandy is offline gfiandy  United Kingdom
diyAudio Member
 
gfiandy's Avatar
 
Join Date: Jul 2003
Location: Cambridge UK
As currently laid out your input static protection will be compromised by the inductance of the long thin tracks back to the power rails. As you want the ESD to return to is source via the ground plane on a two layer PCB the best way to achieve this would be to combine the diode with capacitors on the +/- rails by each one of the diodes that way there is a low impedance return path for the static event.

Depending on the level of protection you require you could simply eliminate them. The imput impedance offers quite high Static protection and the diodes were put in as comercial designs require a very high level of esd protection to avoid customer returns from dry environments.

Last edited by gfiandy; 6th December 2017 at 11:49 PM.
  Reply With Quote
Old 7th December 2017, 08:21 AM   #22
belyakove is offline belyakove
diyAudio Member
 
Join Date: Jan 2017
Quote:
Originally Posted by gfiandy View Post
I think this is the input stage from an ARCAM A85 amplifier. I used to be the design manager there and think I recognise it.
You're absolutely right. I took it from A32 service manual but I've checked and A85 has exactly the same input stage. Thank you very much for your input. It's very interesting to know how and why decisions were made.

Quote:
Originally Posted by gfiandy View Post
As currently laid out your input static protection will be compromised by the inductance of the long thin tracks back to the power rails. As you want the ESD to return to is source via the ground plane on a two layer PCB the best way to achieve this would be to combine the diode with capacitors on the +/- rails by each one of the diodes that way there is a low impedance return path for the static event.

Depending on the level of protection you require you could simply eliminate them. The imput impedance offers quite high Static protection and the diodes were put in as comercial designs require a very high level of esd protection to avoid customer returns from dry environments.

I've looked at the Arcam's preamp board layout in service manual (it doesn't show traces unfortunately, only the layout of components) and it seemed to me that esd protection diodes are located quite far from one another and that they are also quite long there.

Unfortunately I don't quite get the idea with the capacitors in combination with diodes. Do you mean to put them between power supply rail and the ground next to each diode?
  Reply With Quote
Old 7th December 2017, 08:28 AM   #23
belyakove is offline belyakove
diyAudio Member
 
Join Date: Jan 2017
Quote:
Originally Posted by Monte McGuire View Post
Yeah, large C0G caps cost a fortune and are huge, but they're still tiny compared to a film and a lot cleaner, unless you spend a lot of money. Still, you do not need anything above 0.1F for a servo - using an output attenuator to reduce the servo loop gain will lower the effective highpass frequency. In a servo I'm working on now, I'm using around 60K and 0.1F, and I get an overall high pass corner of 1Hz because the servo output is attenuated back into the amplifier it's correcting. That also solves a lot of other problems, such as minimizing the servo amp's LF noise, which is injected back into the controlled op amp.

It's best to use a simulator like LTspice to verify the response of these circuits, since the calculations can get complicated, and at the very least, it's nice to have confirmation that what you think is happening is actually happening.
Surprisingly I can understand almost everything that you've wrote. You're explaining it very good. Thank you!

Unfortunately I don't know the theory behind the dc servo circuit so I don't quite get how to make the attenuator and how it can affect circuit. I understand the basic principle of dc servo, that an integrator would make an average of the signal which will be the dc offset and will supply it back to the op amp and shifting the output to stay at 0 offset. But I don't know why the values of feedback capacitor and input and output resistors are chosen this way and how it is calculated.
  Reply With Quote
Old 7th December 2017, 08:34 AM   #24
belyakove is offline belyakove
diyAudio Member
 
Join Date: Jan 2017
A bit of off topic but related to dc servo circuits. My power amp that I'm going to use is also using dc servo circuit. It is basically LM3886 bridged-parallel amplifier so it uses dc servos at each chip to prevent amplifier chips from fighting each other. I've bought ready made PCBs for that and they also use 0.47uF capacitors in the feedback of the servo op amp but the component that should used to be there is 0805. So the only capacitor with that value and package size appeared to be X7R ceramic. Is it ok to use X7R there. How can it affect the circuit in this application compared to C0G? I don't know if it matters but amplifier chips and dc servos are in non-inverting configuration there.
  Reply With Quote
Old 7th December 2017, 12:03 PM   #25
gfiandy is offline gfiandy  United Kingdom
diyAudio Member
 
gfiandy's Avatar
 
Join Date: Jul 2003
Location: Cambridge UK
The A32 is a 4 layer PCB and the return path for the ESD diodes is enhanced by that. In a two layer design you need a way to ensure that the ESD strike becomes common mode as fast as possible. To do this you couple the power lines to the ground plane at high frequency with capacitors.

This way if you get an ESD strike the energy ends up on all the parts of the circuit together causing a short common mode lift in voltage. Rather than rushing through the electronics to get to the lower potential points causing damage.

As I said earlier if you are relatively careful about static you can get away without these parts. But for your interest I have shown a possiblle placement sharing caps beween diodes to reduce the number required.
Attached Images
File Type: jpg 98EB34B3-BFBD-436E-BAB6-CF3BBACB5E1B.jpg (217.2 KB, 112 views)
  Reply With Quote
Old 9th December 2017, 10:05 AM   #26
belyakove is offline belyakove
diyAudio Member
 
Join Date: Jan 2017
Quote:
Originally Posted by gfiandy View Post
The A32 is a 4 layer PCB and the return path for the ESD diodes is enhanced by that. In a two layer design you need a way to ensure that the ESD strike becomes common mode as fast as possible. To do this you couple the power lines to the ground plane at high frequency with capacitors.

This way if you get an ESD strike the energy ends up on all the parts of the circuit together causing a short common mode lift in voltage. Rather than rushing through the electronics to get to the lower potential points causing damage.

As I said earlier if you are relatively careful about static you can get away without these parts. But for your interest I have shown a possiblle placement sharing caps beween diodes to reduce the number required.
Thank you. Now I'm starting to understand how ESD protection works. Probably I'll remove this protection because as you said it was done primarily for dry countries and I live probably in one of the most wet places in the world
But I'm interested in how to choose values for these capacitors.
  Reply With Quote
Old 9th December 2017, 11:36 AM   #27
gfiandy is offline gfiandy  United Kingdom
diyAudio Member
 
gfiandy's Avatar
 
Join Date: Jul 2003
Location: Cambridge UK
Typically the performance of capacitors in this application is limited by the inductance of the capacitor and its pad and PCB layout. The situation is complicated by the conflicting requirements of the component. To withstand the inital strike voltage you want a very high breakdown voltage, however to have low inductance you want as small a part as possible and to have the minimum reduction in capacitance due to the voltage you want a stable dielectric like cog. In a situation like this I would guess 470pF in 0603 at as high a voltage as was reasonable in price would be a reasonable compromise. However to be sure I now simulate an ESD strike using LTSpice and optimise the protection that way, it can be quite counter intuative how the circuit will behave.
  Reply With Quote
Old 10th December 2017, 04:56 PM   #28
belyakove is offline belyakove
diyAudio Member
 
Join Date: Jan 2017
So I've rebuilt PCB a little following the recommendations. I got rid of ESD protection diodes, filters are now completely SMD with C0G capacitors instead of a film, replaced tantalum capacitors with aluminium electrolytics. Also I've laid out digital part so the entire PCB is kinda finished now.
Below I've attached complete proper schematics and PCB layout.
Attached Files
File Type: pdf New-Schematic-2-2.pdf (53.7 KB, 26 views)
File Type: pdf Preamp-PCB.pdf (63.7 KB, 38 views)
  Reply With Quote
Old 14th December 2017, 04:16 PM   #29
r_merola is offline r_merola  Brazil
diyAudio Member
 
Join Date: Apr 2009
belyakove

I would like to know if you already have the microcontroller control code for this design and also know if you will share it with us.

Your PCB is really nice now.

Regards
Ronaldo
  Reply With Quote
Old 14th December 2017, 04:38 PM   #30
gfiandy is offline gfiandy  United Kingdom
diyAudio Member
 
gfiandy's Avatar
 
Join Date: Jul 2003
Location: Cambridge UK
Improved design looks good,
I have identified a few things you might want to look at.

I dont know if you had a design rule checker on your PCB package but it looks like the diagonal tracks exiting r1 r31 r21 r22 are too close to the pad and you might get etching or solder wisker problems.

The digital and analogue grounds do not appear to be connected they need to be connected together somewhere or they can float from each other causing problems.

The digital control lines going to the mux can be a source of noise from the microcontroller, an in line resistor and capacitor helps to filter this off. It should be filtered to the analogue ground but preferable close to the ground plane split.
  Reply With Quote

Reply


Laying out preamp pcbHide 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
Help:Laying out inductors of crossover jocoman Multi-Way 12 19th April 2012 01:54 AM
anyone have any el86 circuits laying around? sousmielie Tubes / Valves 10 25th July 2009 02:30 PM
help laying out a pcb rockstudio Chip Amps 1 7th April 2006 03:55 PM
Dipolar sub laying down? eRiCdWoNg Subwoofers 3 13th November 2004 06:55 PM


New To Site? Need Help?

All times are GMT. The time now is 05:27 AM.


Search Engine Optimisation provided by DragonByte SEO (Pro) - vBulletin Mods & Addons Copyright © 2017 DragonByte Technologies Ltd.
Resources saved on this page: MySQL 15.00%
vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2017 DragonByte Technologies Ltd.
Copyright ©1999-2017 diyAudio
Wiki