Hi,
I'm about to start building this, and I've seen people show some interest so I thought I'd start a build thread.
I've put the information on my blog for anyone who's interested :
http://myl8test.wordpress.com/audio/ak4399-dac/
cheers,
Tom
I'm about to start building this, and I've seen people show some interest so I thought I'd start a build thread.
I've put the information on my blog for anyone who's interested :
http://myl8test.wordpress.com/audio/ak4399-dac/
cheers,
Tom
Last edited:
Thanks - I think it could be quite easily hacked for serial control, but I'm gonna stick with parallel.
Just a quick look and you can probably see a few routing issues - hopefully I can fix them - an op amp power line runs between the pads for 470R on both channels. It's okay that they cross perpendicular, so there's little chance of any induced problems, but I'd like to improve that. Maybe it'll be as simple as using a through hole resistor mounted on the other side. And the power rails for the DAC run perpendicular across the DAC's analogue output - between the C1-C4 mounting points. On the plus side, a continuous ground plane on the other side is very welcome.
Did I miss anything else that needs to be improved ?
I'll need to work out the Q of the lpf filter too.
cheers
Just a quick look and you can probably see a few routing issues - hopefully I can fix them - an op amp power line runs between the pads for 470R on both channels. It's okay that they cross perpendicular, so there's little chance of any induced problems, but I'd like to improve that. Maybe it'll be as simple as using a through hole resistor mounted on the other side. And the power rails for the DAC run perpendicular across the DAC's analogue output - between the C1-C4 mounting points. On the plus side, a continuous ground plane on the other side is very welcome.
Did I miss anything else that needs to be improved ?
I'll need to work out the Q of the lpf filter too.
cheers
Last edited:
The terms "ground pour" and "via" spring to mind.
I have some ideas about how to mitigate the C1-C4 and 470R routing. Is there anything else to address ?
It is just for fun - I'll try to build it for very little money. The parts I ordered were just US$8. Are there any other AK4399 diy projects out there ?
cheers
I have some ideas about how to mitigate the C1-C4 and 470R routing. Is there anything else to address ?
It is just for fun - I'll try to build it for very little money. The parts I ordered were just US$8. Are there any other AK4399 diy projects out there ?
cheers
Thanks. I'll try to do just that.
I think the seller is probably willing to make changes and try to improve the design because he has done this with his other kits, and a better PCB might increase sales. I don't doubt he'll read this thread so if you think it's worth your time, do feel free to give some specific comments. Then again, he could just read all those links you've posted !
http://www.diyaudio.com/forums/digi...signal-path-line-resistors-5.html#post3017750
I think the seller is probably willing to make changes and try to improve the design because he has done this with his other kits, and a better PCB might increase sales. I don't doubt he'll read this thread so if you think it's worth your time, do feel free to give some specific comments. Then again, he could just read all those links you've posted !
http://www.diyaudio.com/forums/digi...signal-path-line-resistors-5.html#post3017750
Cheers for the link, I was trying to find it the otherday as I have lost my source of a lot of those links.
As they are already populating the DAC it would be nice to add the decoupling and possibly a local LDo to supply the DAC, wouldn't add much to the overall cost but would make it a much better option for DIYers especially those with limited experience.
Cheers Marc
As they are already populating the DAC it would be nice to add the decoupling and possibly a local LDo to supply the DAC, wouldn't add much to the overall cost but would make it a much better option for DIYers especially those with limited experience.
Cheers Marc
I agree - a little bit more smd done already so the rest of the design can be through-hole stuff.
I found a really good online lpf calculator here : (Sample)Sallen-Key Low-pass Filter Design Tool - Result -
The AKM result is clearly better. However, for the board's values, changing the shunt cap on the op amp input to 7.5nF or 8nF is an improvement, although the cut off frequency is still quite low ~98Khz.
Here's some of the numbers. The site also gives graphs for transient response etc.
AKM Values :
Cut-off frequency
fc = 18202776.4579[Hz]
Quality factor
Q = 0.439589907374
The system does not oscillate.
And the circuit values on the board have this result :
Cut-off frequency
* * fc = 106386.994045[Hz]
Quality factor
* * Q = 0.5
Oscillation frequency
* * f = 0.00124339799291[Hz]
I found a really good online lpf calculator here : (Sample)Sallen-Key Low-pass Filter Design Tool - Result -
The AKM result is clearly better. However, for the board's values, changing the shunt cap on the op amp input to 7.5nF or 8nF is an improvement, although the cut off frequency is still quite low ~98Khz.
Here's some of the numbers. The site also gives graphs for transient response etc.
AKM Values :
Cut-off frequency
fc = 18202776.4579[Hz]
Quality factor
Q = 0.439589907374
The system does not oscillate.
And the circuit values on the board have this result :
Cut-off frequency
* * fc = 106386.994045[Hz]
Quality factor
* * Q = 0.5
Oscillation frequency
* * f = 0.00124339799291[Hz]
Last edited:
zero distance decoupling capacitor is done like this
the limitation is always on the diyer happy diying to allAn externally hosted image should be here but it was not working when we last tested it.
NiceWhen I do boards with these devices on, I place the decouplers there only on the other side of the board, your solution is better still, but impracticle for comercial production.
If it is a 0.8mm pitch device i would say they will be 0402 capacitors, having played with those I am impressed by your patience and dexterity. Not for the faint hearted or impatienced diyer.
Marc, have you seen the new 10000pf thin film (GX) caps from AVX? $7 a pop for an 0201 speck lol. for those that dont know thin film usually tops out around 10-22pf except for some rather impractical bare dies for wire-bonding... per kg these could be the most expensive capacitors on earth!!
re placement, between pins seems the best (most frustrating) way forward, wouldnt being soldered on top side as close as possible always be closer than even directly under the pins if its on the other side of the substrate?
re placement, between pins seems the best (most frustrating) way forward, wouldnt being soldered on top side as close as possible always be closer than even directly under the pins if its on the other side of the substrate?
Last edited:
Quite often put 0201 and 0105 on PCB's these days, but not at those prices, a single one costs more than some whole assemblies! Good to 40GHz.
The area directly under the pins is dead space, ie you cant get a via in there so for double sided placement PCB's its the best place to put the decouplers, not all chips have nice power pins next to each other as conviently as this device, and most devices of this type we see have a pin to pin spacing of 0.5mm quite often (and sometimes 0.4mm). Even with 0.65mm devices you have to get the routes out away from the device to be able to get some via fan outs, so the most efficient place is under the pins, with shared vias to the power planes with the relevant pins. You also have to consider the round trip to the plane through the board, vias arn't as inductive as a short trace length, and the capacitors have to be charged from the power planes.
A compramise like most PCB design, quite often you cant see any PCB because of components, so every bit of space is often needed.
Now the best option is using HDI PCB layout with microvias in the component pads, the top layer as a ground plane and the next plane down the most critical supply, this minimises both the loop area for the supplies (0.05 to 0.1 dialectric between layers) and stray parasitic inductance caused by a trace from the capacitor to a via (this can double the inductance for a 0402, 0201 cap). This is quite common these days especially in AISA (mobile phones etc)
and becoming more popular in the West as component size is often the deceiding factor to go to HDI.
http://www.google.co.uk/url?sa=t&rc...noGQBw&usg=AFQjCNHFVBbngoQa1g_EWvypzn3Woj1pUw
The area directly under the pins is dead space, ie you cant get a via in there so for double sided placement PCB's its the best place to put the decouplers, not all chips have nice power pins next to each other as conviently as this device, and most devices of this type we see have a pin to pin spacing of 0.5mm quite often (and sometimes 0.4mm). Even with 0.65mm devices you have to get the routes out away from the device to be able to get some via fan outs, so the most efficient place is under the pins, with shared vias to the power planes with the relevant pins. You also have to consider the round trip to the plane through the board, vias arn't as inductive as a short trace length, and the capacitors have to be charged from the power planes.
A compramise like most PCB design, quite often you cant see any PCB because of components, so every bit of space is often needed.
Now the best option is using HDI PCB layout with microvias in the component pads, the top layer as a ground plane and the next plane down the most critical supply, this minimises both the loop area for the supplies (0.05 to 0.1 dialectric between layers) and stray parasitic inductance caused by a trace from the capacitor to a via (this can double the inductance for a 0402, 0201 cap). This is quite common these days especially in AISA (mobile phones etc)
and becoming more popular in the West as component size is often the deceiding factor to go to HDI.
http://www.google.co.uk/url?sa=t&rc...noGQBw&usg=AFQjCNHFVBbngoQa1g_EWvypzn3Woj1pUw
Last edited:
Wah, very cool - great skills ! What size are they ? Only those four pins ? Any tips for me about building this ? Thanks.
and Kung Hei Fat Choi !
When I do boards with these devices on, I place the decouplers there only on the other side of the board, your solution is better still, but impracticle for comercial production.
If it is a 0.8mm pitch device i would say they will be 0402 capacitors, having played with those I am impressed by your patience and dexterity. Not for the faint hearted or impatienced diyer.
the cap in the pic is 0402 size
I also need magnifying glass to solder it.It's open secret that decouple cap directly solder on the pin is the best, but impractical for commercial production, diyer have no limitation
Last edited:
A magnifying glass, no coffee, plenty of time, good tools... and skills. I won't be trying !
What values are you using in the lpf ? The values printed on the board don't seem that good. The 220R is fine but the cap values need to be a little different from each other and a little smaller ?
cheers
What values are you using in the lpf ? The values printed on the board don't seem that good. The 220R is fine but the cap values need to be a little different from each other and a little smaller ?
cheers
The value on the pcb follows the AK4399 EVM pdf
http://www.asahi-kasei.co.jp/akm/en/product/ak4399/akd4399-sb4-03e.pdf
Thanks. I'll try either a slightly larger cap on the shunt or a slightly smaller cap in the feedback. It gives better impulse response etc.
Here's the EVM circuit for anyone interested :
Here's the EVM circuit for anyone interested :
An externally hosted image should be here but it was not working when we last tested it.
3rd routing issue. Bottom left corner, FB1, goes to a via, and on the other side there is a power trace that runs at 30 degrees across the MCLK line.
- Status
- Not open for further replies.