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

Digital Line Level DACs, Digital Crossovers, Equalizers, etc.

General DAC design rules, layout techniques, etc.
General DAC design rules, layout techniques, etc.
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 7th December 2017, 01:50 PM   #11
dmills is offline dmills  United Kingdom
diyAudio Member
 
Join Date: Aug 2008
Location: High Wycombe
Series termination close to the receiver does not usually buy you much, you want the series termination to be close to the transmitter!

If you are going to split the ground plane, you need to make sure that nothing crosses the split on the top side of the board, difficult to tell without a view showing both layers.

You have the analog pairs on your analog out headers, but where are the high frequency grounds? The stuff coming straight out of the chip will likely have significant common mode RF on it (Which is never documented for some reason), and you want to be able to shunt that to ground, before it hits a slew rate limited opamp. I would be building the first pole on the board rather externally to make this more doable.
I really wish the DAC vendors would give an output spectrum extending well into the HF bands and not use a 20-20k filtered number. I should do some work with my SA and see what really comes out of these things up above the audio band.

DACs are to a first order approximation, mixers (in the RF sense of multiplier) and should be treated as such.


Regards, Dan.
  Reply With Quote
Old 7th December 2017, 08:28 PM   #12
MarcelvdG is offline MarcelvdG  Netherlands
diyAudio Member
 
Join Date: Mar 2003
Location: Haarlem, the Netherlands
Quote:
Originally Posted by zarandok View Post
Ok, calculated without guarding on the top side. And what now...?
Now you can compare it to the "koplanarer Wellenleiter mit Masseflaeche" to get an idea about how far your top layer ground fill must stay from the trace if you want the bottom to be the main return path. Above a certain ground fill spacing the characteristic impedance will stay nearly constant because almost all trace capacitance is to the bottom ground plane and not to the top layer ground fill.

With 125 ohm characteristic impedance, guesstimating 25 ohm source resistance and neglecting the input capacitance of the DAC inputs compared to the traces, you would need a 100 ohm series termination resistor at the source. As the input capacitance of the DAC is not zero, you could round that down a bit to 82 ohm or so.
  Reply With Quote
Old 7th December 2017, 08:51 PM   #13
MarcelvdG is offline MarcelvdG  Netherlands
diyAudio Member
 
Join Date: Mar 2003
Location: Haarlem, the Netherlands
Quote:
Originally Posted by zarandok View Post
Thanks MarcelvdG!
I didn't know KiCAD, but I will see this calculator tool... (I use DipTrace). Thanks for the tip!

I know that reference voltage is extreme important. I'll use low-noise shunt regs near to the DAC chip to supply them, possibly will try LT3042 too sometime...

The reason why I asked this question is that I have the small bypass caps on the bottom layer, and then connected the Vref line through vias to the DAC pins (see picture). This is of course not the best solution, because of vias have some inductance which could decreace the effect of the bypass caps -> IF the Vref pins need HF currents! And this is the point what I do not know, where the HF currents are flowing into the DAC. At the Vref pins or at the AVDD pin (by AK4458 for example)??
Whether there are significant HF currents flowing through the Vref pins depends on the internal circuitry; do they directly feed the actual DACs or only buffers that feed the DACs? The impression I get from the datasheet, but that's only an educated guess, is that the AK4458 probably contains switched capacitor DACs that are directly charged from the external bypass capacitors, resulting in large current spikes. Having too much trace and via inductance then messes up the settling of the voltage across the DAC capacitors, which could seriously affect the noise floor and the distortion. So I'd do whatever keeps the inductance in the VREFH-decoupling-VREFL loops as low as possible. Vias are inductive, but so are traces. Is there any way you can put the caps right next to each VREFH/VREFL pair on the same layer as the IC?
  Reply With Quote
Old 8th December 2017, 01:58 PM   #14
dmills is offline dmills  United Kingdom
diyAudio Member
 
Join Date: Aug 2008
Location: High Wycombe
Yep, rule of thumb with delta sigma parts is to assume they are charge transfer devices until proved wrong, and treat them as RF components not audio ones (obviously they are both, but the RF side is usually trickier about layout then the bit down in the wobbly DC region). 0402 and 0603 C0G are very much your friends.

The real gotcha is in ADCs actually, especially fast ADCs where source termination really needs to give good return loss up into the low microwave bands for maximum SFDR.

Regards, Dan.
  Reply With Quote
Old 11th December 2017, 09:59 AM   #15
zarandok is offline zarandok  Austria
diyAudio Member
 
Join Date: Feb 2015
Quote:
Originally Posted by MarcelvdG View Post
Vias are inductive, but so are traces. Is there any way you can put the caps right next to each VREFH/VREFL pair on the same layer as the IC?
It is not so easy, because of the analog signal pin headers. I'd like to place the voltage regulator circuits as near to the DAC as possible. This means that I have not a lot of space for 2x8=16 audio traces to run across the regulators (don't forget I have only 2 layers), so I've decided to lead them to the filter PCB direct from the DAC pins (see pics before). In that case there are only very small "islands" between them (on the top layer). Probably I can try with 0603 or smaller caps, but I did not find a good solution so far...

It would be advantageuos to know the inseide operation of the DAC but this is unfortunately not the case...

Last edited by zarandok; 11th December 2017 at 10:02 AM.
  Reply With Quote
Old 11th December 2017, 10:11 AM   #16
zarandok is offline zarandok  Austria
diyAudio Member
 
Join Date: Feb 2015
Quote:
Originally Posted by dmills View Post
If you are going to split the ground plane, you need to make sure that nothing crosses the split on the top side of the board, difficult to tell without a view showing both layers.

You have the analog pairs on your analog out headers, but where are the high frequency grounds? The stuff coming straight out of the chip will likely have significant common mode RF on it (Which is never documented for some reason), and you want to be able to shunt that to ground, before it hits a slew rate limited opamp. I would be building the first pole on the board rather externally to make this more doable.
Splitting the digital and analog ground layers is a recommendation from the manufacturer. There are no crosses, but I can upload my design files if you wish...

It is a good question. You mean that the HF components of the analog signal (that must be actually filtered out) want go back to DAC ground? If it is so, the loop must be really small to assure effectivity... But the question is the same: how can I make it with 2 layers and separate filter PCB in all 8 channels? I think I must make serious compromisses somewhere...
  Reply With Quote
Old 11th December 2017, 10:28 AM   #17
JPS64 is offline JPS64  Germany
diyAudio Member
 
Join Date: May 2011
General DAC design rules, layout techniques, etc.
4 layers for simplicity and fewer compromisses.

My 2 cents.

Good luck with 2 layers only.

JP
  Reply With Quote
Old 11th December 2017, 10:45 AM   #18
dmills is offline dmills  United Kingdom
diyAudio Member
 
Join Date: Aug 2008
Location: High Wycombe
Yep, my default for more or less anything these days is to start at 4 layers and if I need to go to 6 it does not take that much thought.

Multilayer boards do not have the cost for prototypes that they once did, and being able to bury power and (especially) a real ground plane is all to the good.

I would pick a much denser connector then that .1 inch thing, if you go to a 1 or even 0.5mm pitch board stacking connector from Molex or the like you can shoe horn a lot of ground onto it as well as the audio.

Regards, Dan.
  Reply With Quote
Old 11th December 2017, 10:53 AM   #19
JPS64 is offline JPS64  Germany
diyAudio Member
 
Join Date: May 2011
General DAC design rules, layout techniques, etc.
Multi-cb also offerings via filling (so nice to place vias in SMD pads), this helps a lot; I donīt know the costs.

Iīm using Samtec connectors (differential or not), but Molex ones not bad.

JP
  Reply With Quote
Old 11th December 2017, 11:40 AM   #20
zarandok is offline zarandok  Austria
diyAudio Member
 
Join Date: Feb 2015
Quote:
Originally Posted by dmills View Post
... or the like you can shoe horn a lot of ground onto it as well as the audio.
Sorry, but I can't understand that...
Which type would you recommend from e.g. Molex?

I'am considering 4-layers but it is not so easy. Nr.1: never done before. Nr.2: I must buy a layout software. Nr.3: manufacturing costs more, if I'd like to order 1-2 pieces (only for me).
  Reply With Quote

Reply


General DAC design rules, layout techniques, etc.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

Forum Jump

Similar Threads
Thread Thread Starter Forum Replies Last Post
Enclosure building specific techniques for general cabinetmaker? Barrettn Construction Tips 26 28th November 2017 12:51 AM
Audio Pcb Layout Techniques aspringv Construction Tips 98 10th June 2014 11:46 PM
Rules of thumb when designing a TMM 2.5 way Dave Bullet Multi-Way 2 16th March 2007 08:31 PM
layout rules Stefanoo Solid State 6 5th March 2007 06:01 PM
Opamp layout rules Onvinyl Chip Amps 15 27th March 2006 11:04 AM


New To Site? Need Help?

All times are GMT. The time now is 05:16 PM.


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