DAC Schematic Review and Layout Suggestions - WM8804 and PCM5102A

Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
Disabled Account
Joined 2014
February 2021

I stumbled upon this project after looking through my archives and clearing out my old accounts. Obviously this project is dead, though I did learn a lot in the process and I hope this thread will help out others with similar designs.

I'm sharing the final schematic and gerbers here (final_design.zip) for future reference - my blog and social media accounts don't exist anymore. I couldn't find the BOM, but if someone really wants to build this do send me a PM and I'll look harder :).

Thanks again to everyone who helped out with this design.

--------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
November 2014

The information on this first post is outdated (I've made changes)! The final details are as follows:

  • Built-in linear power supply with external transformer and pre-reg (no USB!)
  • PCM5102A DAC, WM8804 with transformer-coupled SPDIF input (coaxial)
  • Four LP5907 regulators to feed the AVDD/DVDD supplies of the chips
  • 3.5mm and RCA outputs
I already have a working prototype available, but there is a potential clipping problem which I have yet to iron out.

The latest schematic is avaliable here, and the latest Gerber files are avaliable here. I'm sharing everything under the Creative Commons Attribution-NonCommercial 4.0 International license.

--------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
Original Post (July 2014)

Ok, so here's my first DAC project! I've got the schematic here, but I would prefer to hear your suggestions first before actually laying it out on a PCB. The circuit is a simple one, using a Wolfson WM8804 (coaxial SPDIF input, isolated) to send I2S signals to a TI PCM5102 DAC. Regulation is provided by 2 TI LP5907s (low noise and PSRR) connected to a USB 5V supply. Most of the actual circuitry is simply from the datasheet (I don't have the skill to come up with my own;).

Currently, I've separated the digital and analog supplies using 2 regulators (it looks like the right way to go), but there have been mixed reviews on the internet about whether or not I should have seperate analog and digital grounds, or just a single flat ground plane. SMD looks like the way to go, and most likely I'll be using thru-hole for the large caps and the connectors. Everything else seems fine - but I'm concerned with the high frequency I2S signals (and special considerations) needed to avoid interference.

I'm also a bit unsure about my power supply, as there's no detailed information on the ripple and noise on a USB input. The 100uF cap there is just a guess and may not be optimal. I've also heard mixed reviews on ferrites - some people love them and stick them everywhere, others avoid them altogether. Maybe someone here can help sort this out?

While I won't name names, I've seen several posts here where some of the members have extensively revised a beginner's board to fix all their "problems". After looking at those posts, I think I have a resonable idea of what a 2-layer DAC board should look like - but before I start I think it would be best to get some ideas first...:)

I'm calling it the df audio DAC1, for lack of a better name.

Schematic:
PA1rNBJ.png

Download link
 

Attachments

  • Schematic 1.pdf
    40.8 KB · Views: 341
Last edited:
Disabled Account
Joined 2002
Hi some tips:

- Your design needs beads/coils in the supply lines. People avoid parts that they don't know well and that cost extra money. Trust me, you need them.
- Use termination resistors at the right side of I2S.
- A larger electrolytic cap after the regs close to the DAC chip may be a good idea.
- Since PCM5102A has no free running external clock source possibility you could experiment with a low jitter XO for the 12 MHz (no crystal). It should not make a difference with a PLL but you could try and compare.
- You should remove the power on switch to the AC side of things as switching DC is a bad habit.
- While you are at it you could include a rectifier and large filter cap so the design will be ready for use when using a small power transformer.
- In that case make C19 a 2200 µF 16V.
- The USB connector indicates the use of a switching power supply (which are good, disclaimer etc) but a linear supply will make your design better sound wise. Just test and compare.
- Be prepared for ground loop issues if you just just a computer USB port for supplying power to this DAC.
- After having made the same decision like you on our Subbu V3 I would now include a PCB mount BNC connector straight on the PCB. No wiring !
- Same counts for RCA jacks, soldered straight to the board leaving only the power supply AC wiring to be necessary. There are some very nice quality versions available for that purpose !
- Least possible wiring as wiring does not make things better.
 
Last edited:
The problem with a high C19 is high inrush current via USB - I'm already exceeding the 100uF limit already.
A current limitting resistor (1.5 to 10 Ohms) could solve the issue. Although i believe that 100uF is more than enough.
What do you mean by "remove the power on switch to the AC side of things as switching DC is a bad habit"? I don't have AC at all on my board...
Connecting or disconnecting the USB plug is the same like the function of a DC switch. I think the switch option is OK.
 
- Your design needs beads/coils in the supply lines. People avoid parts that they don't know well and that cost extra money. Trust me, you need them.
Yes, that is correct. Put two ferrite beads in series with the USB Vbus and the USB gnd (ground is a return path for noise etc.) From memory, the ferrite bead should present a resistance of 50 Ohms - at least - at the frequency of interest. Here a type for the beginning: 2512066017Y1 - FAIR-RITE 2512066017Y1 - FERRITE BEAD, 0.08OHM, 1A, 1206, FULL REEL | Newark element14 Canada
 
Disabled Account
Joined 2002
Two things:

The problem with a high C19 is high inrush current via USB - I'm already exceeding the 100uF limit already.

What do you mean by "remove the power on switch to the AC side of things as switching DC is a bad habit"? I don't have AC at all on my board...

Thanks.

Hi, just design a proper mains fed linear power supply instead of feeding this DAC poisoned Volts via USB. Switch can then be at the AC side of things....Reread my post another time please. Try to make your design as good as possible as it will be more expensive than ready made Ebay stuff anyway. Quality is all in the details !

*Please also use CLC filtering to the power supply pins of chips. L may be a coil or a bead.*
 
Last edited:
A very nice thread regarding I2S bus "termination" resistors with excellent documentation here: http://www.diyaudio.com/forums/digital-line-level/212002-i2s-digital-signal-path-line-resistors.html
Top posts written from real scientists - experts on digital circuits and digital audio.
One of the best threads i've ever read on diyAudio.
Take a look and in schematics of WM8741 DAC evaluation board: http://www.wolfsonmicro.com/media/77432/WM8741_6060_DS28_EV2_REV1_Schematic_layout.pdf where a WM8804 spdif transceiver - configured in hardware mode like in your circuit - is used.
 
Last edited:
You should insert an small value A.C. coupling capacitor in series with the S/PDIF transformer T1's primary winding if the S/PDIF transmitter side is not already A.C. coupled. An cap. identical to C14 is probably okay, but a value closer to 10nF is probably preferred. This cap. is to block any D.C. current from flowing through the primary, which would otherwise greatly degrade the core inductance.
 
Last edited:
Oh! I forgot to refer the lack of a POR (Power On Reset) circuit which i think is of major importance regarding all other suggestions as it ensures a safe initialization of all registers of WM8804 during power up. Hardly suggested! See the attached picture.
 

Attachments

  • wm8804_reset.png
    wm8804_reset.png
    26.2 KB · Views: 810
Disabled Account
Joined 2002
You should insert an small value A.C. coupling capacitor in series with the S/PDIF transformer T1's primary winding if the S/PDIF transmitter side is not already A.C. coupled. An cap. identical to C14 is probably okay, but a value closer to 10nF is probably preferred. This cap. is to block any D.C. current from flowing through the primary, which would otherwise greatly degrade the core inductance.

Many sources have caps in series with their outputs or they have output transformers ...

BTW we experienced better results with somewhat larger caps for C14 (220 nF to 1 µF).
 
Disabled Account
Joined 2014
Ok, so here's my updated schematic. In fact, I've started on the layout and should be able to post it online soon.

After listening to your suggestions, I've made some changes:

  • Ferrite beads (this one) are added to the input
  • Cap (C24) added in series to the SPIDF input - it costs almost nothing and should do more harm than good:)
  • 22 ohm damping resistors added to the I2S lines (actually, I have no idea how to calculate the actual values since I don't have a scope and the datasheets don't say the input/output impedances)
  • Point for 5V input is added to the layout (not on the schematic though) so that I can use an external power supply if so desired...
The reset circuit looks interesting, maybe someone can explain why it's better than just connecting the RESET pin to the supply? For the suggestions regarding cap values and stuff, the best thing to do I think is to just order extras and switch them during testing to see which one sounds or measures the best.

4PfutVe.png

PDF avaliable here.

That's it! Layout coming soon, and remember that suggestions are always welcome.
 

Attachments

  • Schematic 1.2.pdf
    72.5 KB · Views: 170
Last edited:
Disabled Account
Joined 2002
Hi you will regret not having used CLC filtering to the supply pins of both chips. The device will be as good as its power supplies, don't skimp on parts in that area. "Low part count" is only a feature in the industry, you don't have to count pennies when DIYing as it will be more expensive than ready made anyway in 99% of cases. Both chips optimally should have their own separate voltage regulators. See our Subbu V3 for inspiration if you like. That one clearly shows the benefits of good decoupling, CLC filtering, separate regs and using beads all over IMHO. In fact I toyed with the idea to adjust our layout to PCM5102A (a 10 minute job) but the ES9023 is a slightly better chip with the external low jitter XO as a bonus so I did not pursue. Since I have the idea I am talking to myself I am out of here. Good luck with the design.

The way you made the reset circuit is OK.

BTW it is called SPDIF....
 
Last edited:
  • Like
Reactions: 1 user
Can you explain how it works?
I quote the section of WM8804 datasheet where is explained what exactly happens during power on reset.
E.g. when the internal processor of WM8804 is powered up, if the pin "RESETB" is in Hi state, won't read the state of "SDIN" pin to decide in which mode will configure the chip before enabling it. So it could decide to select the "software mode operation" without loading all factory preset binary values for "hardware mode" to the 31 registers of device. The same applies if a momentary power failure occurs. Especially in this case, the diode helps discharge the 10uF capacitor quickly. Why 10uF and not 0.1uF as is suggested in datasheet? From... habit due to my previous experience with microcontrollers! A bigger capacitor ensures a longer time lag during reset and so a more secure initialization of chip registers while, at the same time, does not cause any side effect. It also offers more room for unimportant power supply level variations. In either case, 0.1uF or 10uF, both reset and initialization process are instantaneous. A luxury version of course, is the use of a power supply supervisor IC like the DS1818R10 which continuously monitors the power supply level and accordingly decides if there is need for a device reset.
 

Attachments

  • wm8804_reset.png
    wm8804_reset.png
    35.5 KB · Views: 759
Last edited:
[*]Ferrite beads (this one) are added to the input[*]
The ferrite bead i proposed you is of 1206 case style = 3216 metric (or 3.2 X 1.6mm) and i did it simply for its size, for your convenience during soldering. This one you selected is OK as for resistance but of 0805 case style = 2012 metric (or 2.0 X 1.2 mm) which is very small. These "little devils" are magnetized and their handling with metal tweezers is very enervating during soldering, believe me!
22 ohm damping resistors added to the I2S lines (actually, I have no idea how to calculate the actual values since I don't have a scope and the datasheets don't say the input/output impedances)
In the thread i proposed you is clearly refered that the I2S bus lines impedance depends only in the shape, the width and the length of the physical tracks of PCB that connect the audio interface of spdif receiver with this of DAC. It does matter only in PCB layout drawing and for high sampling rate digital audio signals, i.e. 192Ks/s. For lower rates there is not any problem.
 
Last edited:
Disabled Account
Joined 2014
The ferrite bead i proposed you is of 1206 case style = 3216 metric (or 3.2 X 1.6mm) and i did it simply for its size, for your convenience during soldering. This one you selected is OK as for resistance but of 0805 case style = 2012 metric (or 2.0 X 1.2 mm) which is very small. These "little devils" are magnetized and their handling with metal tweezers is very enervating during soldering, believe me!

I've soldered 0805 ferrites before and with my tweezers they're fine.

Hi you will regret not having used CLC filtering to the supply pins of both chips. The device will be as good as its power supplies, don't skimp on parts in that area. "Low part count" is only a feature in the industry, you don't have to count pennies when DIYing as it will be more expensive than ready made anyway in 99% of cases. Both chips optimally should have their own separate voltage regulators. See our Subbu V3 for inspiration if you like. That one clearly shows the benefits of good decoupling, CLC filtering, separate regs and using beads all over IMHO. In fact I toyed with the idea to adjust our layout to PCM5102A (a 10 minute job) but the ES9023 is a slightly better chip with the external low jitter XO as a bonus so I did not pursue. Since I have the idea I am talking to myself I am out of here. Good luck with the design.

I'm looking at the Subbu design right now; it looks quite interesting. Maybe I'll make some changes... :D
 
Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.