I2S and digital signal path - in-line resistors? - Page 4 - diyAudio
Go Back   Home > Forums > Source & Line > Digital Line Level

Digital Line Level DACs, Digital Crossovers, Equalizers, 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 4th May 2012, 01:01 AM   #31
diyAudio Member
 
Join Date: Oct 2011
Quote:
Originally Posted by Ken Newton View Post
IMO, such series resistors mostly serve to damp the ringing of the series resonant parasitic circuit formed by the PCB trace inductance and the logic input termination capacitance. Undamped, such ringing is quite apparent on digital signals viewed via oscilloscope. I've before measured peak ringing voltages higher than the logic supply voltage! These resistors also reduce the peak current demand placed on the logic supply, and thereby, logic supply noise, which has jitter related implications.
Good contribution! Good to know it's also a Jitter mitigation



Quote:
Originally Posted by Ken Newton View Post
Also, an impedance matched termination of a simple digital signal connection will cut the logic voltage levels in half at the receiving end, right smack in the region of qualifying as an invalid logic level. If the point to point connection (source, path, termination, signal levels) was originally designed for impedance matched transmission - which most audio DAC digital logic components and paths seem not to be - then, no problems.
hehe, I guess you are correct there

Quote:
Originally Posted by DF96 View Post
Google transmission line reflection coefficient. I can never remember the formula so I just look it up.
thanks, will do
__________________
This is not reality...
  Reply With Quote
Old 4th May 2012, 01:18 AM   #32
diyAudio Member
 
Join Date: Oct 2011
Well here is the schematic for AMB design for Gamma2 DAC.

Copyrighted material removed by Moderation. You must have the permission of the copyright owner and must be clearly stated to post here.

They use R1 and R2 resistor networks, 68Ohm per individual resistor on the I2S line.

I couldn't tell very well from the layout on the PCB but the resistors are closer to the receivers.

That's probably the best reference I could find but of course I want to know the reasons behind them picking 68 Ohm or putting a resistor there at all and make an optimization for my own design
__________________
This is not reality...
  Reply With Quote
Old 4th May 2012, 11:23 AM   #33
DF96 is offline DF96  England
diyAudio Member
 
Join Date: May 2007
Those resistors appear to be in series with the lines. In that case they should be at the sending end. If they are at the receiving end, or in the middle, then that suggests that whoever designed the PCB did not know what he was doing. Or that the resistors are not actually necessary and are there for cosmetic reasons.
  Reply With Quote
Old 4th May 2012, 12:20 PM   #34
diyAudio Member
 
Join Date: May 2010
Quote:
Originally Posted by zxgravediggerxz View Post
So what are the reasons behind those in-line resistors on the digital lines? and how I can pick the optimal values/types of resistors and position?
This link may be useful. Trace Termination and Reflection Rules and Observations
  Reply With Quote
Old 4th May 2012, 12:44 PM   #35
diyAudio Member
 
s3tup's Avatar
 
Join Date: Dec 2004
Location: Israel
DF96, +1. There are many designs around, which you can't break down to pieces and investigate, but when you see such apparent mistakes, you can imply these mistakes to the whole circuit, rendering the design in a bad manner as well as designer himself with his other circuits. Unless there are side notes as "low cost", where you have to balance between proper design and costs involved.

Another example of wrong digital design is Twisted Pear products. They use single GND wire for I2S connectors on their boards. This mistake creates horrorous amount of EMC energy, which both kills analog TVs and radios around, and as well denies the whole SQ gain of external DAC thing. To overtake the issue you should use copper foil tape - solder it on both ends directly to PCB near the connector, and wrap the cable with it. Then you'll get both good EMI shield, good ground and good low semi-controlled impedance.
You can't use a short wire to connect the foil to circuit, you'll need to scratch the board to get to the GND layer directly near the connector, and connect the foil directly to it.

Last edited by s3tup; 4th May 2012 at 12:46 PM.
  Reply With Quote
Old 6th May 2012, 07:56 PM   #36
diyAudio Member
 
Join Date: Oct 2011
Quote:
Originally Posted by Tam Lin View Post
Tanks for that reference! Good read there

Quote:
Originally Posted by s3tup View Post
DF96, +1. There are many designs around, which you can't break down to pieces and investigate, but when you see such apparent mistakes, you can imply these mistakes to the whole circuit, rendering the design in a bad manner as well as designer himself with his other circuits. Unless there are side notes as "low cost", where you have to balance between proper design and costs involved.

Another example of wrong digital design is Twisted Pear products. They use single GND wire for I2S connectors on their boards. This mistake creates horrorous amount of EMC energy, which both kills analog TVs and radios around, and as well denies the whole SQ gain of external DAC thing. To overtake the issue you should use copper foil tape - solder it on both ends directly to PCB near the connector, and wrap the cable with it. Then you'll get both good EMI shield, good ground and good low semi-controlled impedance.
You can't use a short wire to connect the foil to circuit, you'll need to scratch the board to get to the GND layer directly near the connector, and connect the foil directly to it.
I am thinking of getting my IC's close together and having the I2S traces length be around 1-2", no layer jumping and minimum bends and omitting the termination series resistors and call it a day.

Orrrrrr I can use the same 22 Ohm resistors I use on the USB line and place them at the transmitter ICs on the I2S lines as per what I've see you and the others discuss here.

My I2S chain goes from PCM2707 to SRC4192 to PCM1794.

I am not done with the schematics yet but I am thinking of having all 3 IC's on the same board. 4 layer would suffice? I think 2 layer will be... impossible lol

If I do multiple boards I will use very short cable runs -3"? Good tip on EMI shielding. I could probably do some coax cable hack job lol, which has a copper braid for EMI
__________________
This is not reality...
  Reply With Quote
Old 6th May 2012, 08:11 PM   #37
diyAudio Member
 
s3tup's Avatar
 
Join Date: Dec 2004
Location: Israel
Keep the resistors, they won't harm

2-layer is doable, as long as you use thin board and don't need to swap I2S traces order. Otherwise, for your convenience and better layout - go for 4-layer. If it's price won't horrify you

PCM2707 to SRC4192 to PCM1794 - should nicely fit on a single board. keep the traces on top/bottom layers so you can reach 'em in case you miss something in PCB layout stage.
  Reply With Quote
Old 7th May 2012, 07:40 AM   #38
marce is offline marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
Route the I2S lines as daisy chain, source to 1st device, then to second device, all lines in the same sequence and if possible as a bus.
Signal integrity will be much better with a 4 layer board, it will allow an unbroken ground layer under the critical signal layer providing a good return path, this is as (if not more) critical than the signal trace, thing of every signal as a diff pair coupled to its return path, the return path wants to travel underneath the signal trace, and where it cant causes problems with digital layouts.
  Reply With Quote
Old 8th May 2012, 08:07 PM   #39
diyAudio Member
 
Join Date: Oct 2011
Quote:
Originally Posted by s3tup View Post
Keep the resistors, they won't harm

2-layer is doable, as long as you use thin board and don't need to swap I2S traces order. Otherwise, for your convenience and better layout - go for 4-layer. If it's price won't horrify you

PCM2707 to SRC4192 to PCM1794 - should nicely fit on a single board. keep the traces on top/bottom layers so you can reach 'em in case you miss something in PCB layout stage.
Quote:
Originally Posted by marce View Post
Route the I2S lines as daisy chain, source to 1st device, then to second device, all lines in the same sequence and if possible as a bus.
Signal integrity will be much better with a 4 layer board, it will allow an unbroken ground layer under the critical signal layer providing a good return path, this is as (if not more) critical than the signal trace, thing of every signal as a diff pair coupled to its return path, the return path wants to travel underneath the signal trace, and where it cant causes problems with digital layouts.
Good tips guys!

I will try both approaches actually and see how it works out on a 2 layer vs 4.
If my traces start looping around the board like crazy I'll go 4 layer and lay them out more properly.

Hopefully I'll be done with the schematic in the next month or so and post it up in this form... will see how many mistakes I have than

Right now I'm reading up some general guidelines for better Pcb design, hopefully that will help a bit and autoroutes won't do stupid crap.

I only have access to DIpTrace and NI multisim and ultiboard. I have started this design with DipTrace and there are limitations to it that I notice. In a simpler design that I did before I couldnt figure out how to use the copper pour/power plane correctly. Apparently you can't route after you put a copper plane?!? So route first that copper pour?!? When and for what others use the autorouter for?
__________________
This is not reality...
  Reply With Quote
Old 8th May 2012, 08:25 PM   #40
diyAudio Member
 
s3tup's Avatar
 
Join Date: Dec 2004
Location: Israel
Layout, route, pour, then stitch with vias. If your design software is able to "shelve" the polygon pours, then you could create these pours anytime, and shelve/restore them as you progress to see the layout better.

But... layout is the first thing If you did the layout properly, you won't have any work in routing - just simple straight connections between components.
  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
what resistors are in the aikido signal path jarthel Tubes / Valves 10 29th June 2006 07:33 AM
Relays in digital signal path Prune Digital Source 23 2nd July 2004 06:08 PM


New To Site? Need Help?

All times are GMT. The time now is 02:44 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