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 Source Digital Players and Recorders: CD , SACD , Tape, Memory Card, etc.

AD1862 PCB layout
AD1862 PCB layout
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 9th April 2014, 07:06 AM   #21
Painkiller is offline Painkiller  Norway
diyAudio Member
 
Join Date: Sep 2006
Quote:
Originally Posted by nopants View Post
How are you planning to implement the digital filter (if any) for this DAC? I'm glad to see that this chip is getting some attention these days.
This dac is meant to be fed by the I2SoverUSB with software upsampling to 176.4Khz or higher, so I can omit the digital filter. Well, in my case I'll actually be using the ExaU2I and iancanadas PCM to I2S converter board. This combo only supports 88.2, 96 and 192 kHz.
  Reply With Quote
Old 9th April 2014, 07:37 AM   #22
vzs is offline vzs  Europe
diyAudio Member
 
Join Date: Dec 2005
Location: Cluj-Napoca, Romania
All 3 parts of this article are very informative about what you are asking: Successful PCB grounding with mixed-signal chips

Somewhere last year there was an initiative to implement multiple standardized format multibit DAC boards coupled with Ian's I2S to PCM board (Multibit DAC core boards coupled with I2S-PCM driver board).
Ian proposed to design/prototype some boards if enough information and interest is available.
If you feel like joining would be nice to restart this initiative.

Thanks,
Zsolt
  Reply With Quote
Old 9th April 2014, 07:49 AM   #23
marce is offline marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
You don't, you have one contiguous ground plane.
A quick example of how I would do the output, with as I said earlier pseudo diff pair routing. I could do with your full schematic including output filter to give a much better answer as their is a loop of high frequency noise that goes from the outputs and is shunted down to ground by the output filter.
As to splitting the digital and analogue sections, what software are you using?
Generaly most CAD software allows more than one connection code (route width), a basic starter is to have four separate codes:
GND, all ground connections
VCC, all power connections
DIG, all digital signal connections
ALG, all analogue signal connections
These can be displayed in different colours so when placing the components you can see by the rats nest and the different signal colours where the signals flow and change the layout to avoid digital and analogue signals crossing.
It will be easier to demonstrate this with an example layout hence a full schematic.
Grounding of Mixes Signal Systems
http://www.ti.com/lit/an/slyt499/slyt499.pdf
http://www.analog.com/static/importe...0Grounding.pdf
Attached Images
File Type: png DAC_Example1.png (4.3 KB, 457 views)
  Reply With Quote
Old 9th April 2014, 08:00 AM   #24
marce is offline marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
A list of some basic links I provide for PCB designer's just starting out that want some basic info....
All the usual subjects such as Henry Ott, Howard Johnson, Eric Bogatin are in there plus links to EMC guides. Now EMC is one area where a lot of DIYers get the wrong idea (comments such as EMC doesn't matter to DIY designs)...EMC and Signal Integrity are two sides of the same coin, and both are critical to a successful design...
Don't be put off by the quantity, just glance through a few, and use the rest as a reference. I do need to update this list when time permits...

Now if you want complex analogue digital grounding problems try a 50 channel phase array sonar
Attached Files
File Type: txt PCB related links.txt (5.1 KB, 39 views)

Last edited by marce; 9th April 2014 at 08:09 AM.
  Reply With Quote
Old 10th April 2014, 07:59 AM   #25
skouliki is offline skouliki  Greece
diyAudio Member
 
skouliki's Avatar
 
Join Date: Aug 2010
Location: Athens
Hi.
Im posting a dual layer pcb i designed some months ago for AD1862 with AD844 for i/v. Digital supplies have onboard regs (mic5207). I havent etched the boards mainly because i havent really studied how to implement logic ic's yet. Any comments are welcome
Attached Images
File Type: png ad1862.png (78.2 KB, 438 views)
  Reply With Quote
Old 10th April 2014, 08:38 AM   #26
skouliki is offline skouliki  Greece
diyAudio Member
 
skouliki's Avatar
 
Join Date: Aug 2010
Location: Athens
Realized i uploaded an image of the pcb with routing errors. New one should be ok
Attached Images
File Type: jpg ad1862.jpg (144.4 KB, 425 views)
  Reply With Quote
Old 10th April 2014, 08:50 AM   #27
marce is offline marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
My only comment would be some vias very close to pads which may cause solder thieving.
I presume those are very small SMD (0402) caps next to the pins, cool, again watch for solder thieving due to the proximity of the pth hole, though if you do the AS1862 first it shouldn't be much of a problem...But may make soldering the chip cap a bit more problematic.
Also some thermal relief on the GND pads would help.
So my only caveat would be to just give these components a bit more room for soldering and move the vias out from the pads a little bit.
Other than that the analogue and digital is separated, the layout is neat and simple, job well done
  Reply With Quote
Old 10th April 2014, 10:22 AM   #28
Painkiller is offline Painkiller  Norway
diyAudio Member
 
Join Date: Sep 2006
That looks really neat! I see how you have managed to separate the digital and analog sections. Did you ever consider making a stereo dac board?

As for the glue logic. We don't really need to think about flip flops and shift registers anymore, because the I2SoverUSB receiver can output a compatible 20-bit "PCM" signal directly. With separate DL and DR lines.

If you compare with my layout suggestion, you can see that the digital lines and the +-5V supply have switched places. I think you got it right. A question to marce; how would you place "several decoupling caps strategically around the board"? That is if one were to use two 100 nF SMD caps for filtering on each of the digital supply lines. Henry Ott suggests spreading them out across the board.
Attached Images
File Type: jpg AD8162 layout.jpg (177.5 KB, 415 views)
  Reply With Quote
Old 10th April 2014, 10:31 AM   #29
Painkiller is offline Painkiller  Norway
diyAudio Member
 
Join Date: Sep 2006
Quote:
Originally Posted by marce View Post
You don't, you have one contiguous ground plane.
A quick example of how I would do the output, with as I said earlier pseudo diff pair routing. I could do with your full schematic including output filter to give a much better answer as their is a loop of high frequency noise that goes from the outputs and is shunted down to ground by the output filter.
As to splitting the digital and analogue sections, what software are you using?
Generaly most CAD software allows more than one connection code (route width), a basic starter is to have four separate codes:
GND, all ground connections
VCC, all power connections
DIG, all digital signal connections
ALG, all analogue signal connections
These can be displayed in different colours so when placing the components you can see by the rats nest and the different signal colours where the signals flow and change the layout to avoid digital and analogue signals crossing.
It will be easier to demonstrate this with an example layout hence a full schematic.
I you use this pseudo diff pair routing, would you still connect it dac chip and the I/V stage to the same ground plane?

I use sPrint layout from Abacom. It doesn't support color coding of rubber bands unfortunately. Maybe I need to switch to Eagle.

I don't have a full schematic ready yet, but I will upload it when I do. I will probably be using Pedja Rogics discrete circuit. The only filtering will be a 330pF cap across the iv-resistor (1-2k). So the high frequency noise from this output stage will be looping back the dac ground?

Thanks for all the links! I have to admit that feels a bit overwhelming. I'll have a look at it. Seems there's a lot I need to learn.
  Reply With Quote
Old 10th April 2014, 12:06 PM   #30
marce is offline marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
Decoupling first, Henry Ott is talking more of boards with more components and pins, with BGA's etc, boards 100mm x 100mm can have a few hundred components and 5000+ pins, for this sort of design the caps you have will be adequate. Some boards with multiple gates switching can have instantaneous current demands in the 100A region, hence the importance of decoupling capacitors (if you want to fry your brain look up "simultaneous switching noise").

The pseudo balanced connections are used on some complex analogue digital boards where we want to avoid cross channel interference (think military headsets and communication) and probably a bit of overkill for this design, it also depends on the topology of the layout. if you are going direct into an op-amp as Skouliki has done above, both devices are on the same GND plane, you would join the AGND pin to this plane at the DAC, then run a signal from this pin to the op-amp - pin, as I have shown above, but do not connect this - pin to the GND plane (otherwise the current would travel through both). I will try and throw together an illustration as it is easier to follow. This is quite a specialised technique and I only use it on critical audio/analogue designs where ultimate signal fidelity and cross talk avoidance is required, generally just using the ground plane can suffice and people wont notice any difference.
The colour coding of the rubber bans isn't strictly necessary, but is a great help in visualising the rats nest, especially when you end up with a few thousand connections
Rather a lot of info, it is a generic list I give people who are going into professional PCB design, as on another forum one of the regular questions was "what do I need to know to do PCB design" and I got sick of giving the same answer so I just post that file, for hobby design probably overkill, for professional PCB design it is the basics.
  Reply With Quote

Reply


AD1862 PCB layoutHide 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
Eagle vs. Sprint-Layout for PCB design/layout hollowman Parts 11 12th January 2014 09:01 PM
Yet Another Cmoy - PCB layout with Eagle and making PCB B&W_arthur Headphone Systems 48 12th November 2013 01:07 PM
pcb layout for- carlsburg Software Tools 20 17th June 2011 08:42 PM
pcb layout jamesrnz Power Supplies 0 9th March 2008 12:42 AM
About PCB layout gaetan8888 Solid State 14 11th January 2008 04:11 AM


New To Site? Need Help?

All times are GMT. The time now is 08:14 PM.


Search Engine Optimisation provided by DragonByte SEO (Pro) - vBulletin Mods & Addons Copyright © 2019 DragonByte Technologies Ltd.
Resources saved on this page: MySQL 14.29%
vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2019 DragonByte Technologies Ltd.
Copyright ©1999-2019 diyAudio
Wiki