Hi all,
I have been working on a USB DAC (that I will post up as I get my schematic finalized) and I have finally arrived at the DAC section.
I am using a PCM2707 to asynchronous up-sampling converter SRC4192 to the PCM1794 DAC.
I have been reading numerous threads on the IV stage and have seen many solutions involving discrete, passive and op-amp solutions but I don't want to blatantly just copy some one else's design and slap it onto my schematic (ZEN converther hehe). I have been trying to understand how the IV and amp/filter stage work, and I have taken a liking to the OPAMP solution.
So in my attempt no to copy other people and to understand how this works.... I have copied the design on page 20 of the PCM1794 datasheet 😀. I have read up on finding an alternate opamp solution to the one proposed by the TI/BB designers. I have been looking into the ADA4627 and the ADA4637
Those opamps are pretty expensive at just under $10 on digikey/mouser and are supposed to be a rival to the OPA627 and OPA637 from TI/BB, therefore I need to know that this wont be a waste of money to performance that I can get.
ADA4637 has a higher Gain Bandwidth, Slew Rate, and Settling Time than the ADA4627 and I decided to run some simulations to see if it makes sense.... the results are below 🙂
Simulation done with LTSpice IV
Transient response at 1kHz and 10k load shows the highest harmonic at around 5kHz at 81.2106dB separation from the 1k (3kHz harmonic is has slightly larger dB separation around 82dB).
Frequency response shows a small roll-off at 10k to 20k at about -219.924mdB which should be good i guess, and a -3dB rolloff at around 79kHz
This the bare bones circuit from TI's datasheet and I hope to get some feedback from you guys and get a better THD than 81dB. Ideally I want to eliminate the IV/filter/gain stage being noise dominant over the DAC.
Also, all the components are ideal 🙁 except for the ADA4637 models, so this might be a challenge.
All help will be appreciated.
Thanks 🙂
I have been working on a USB DAC (that I will post up as I get my schematic finalized) and I have finally arrived at the DAC section.
I am using a PCM2707 to asynchronous up-sampling converter SRC4192 to the PCM1794 DAC.
I have been reading numerous threads on the IV stage and have seen many solutions involving discrete, passive and op-amp solutions but I don't want to blatantly just copy some one else's design and slap it onto my schematic (ZEN converther hehe). I have been trying to understand how the IV and amp/filter stage work, and I have taken a liking to the OPAMP solution.
So in my attempt no to copy other people and to understand how this works.... I have copied the design on page 20 of the PCM1794 datasheet 😀. I have read up on finding an alternate opamp solution to the one proposed by the TI/BB designers. I have been looking into the ADA4627 and the ADA4637
Those opamps are pretty expensive at just under $10 on digikey/mouser and are supposed to be a rival to the OPA627 and OPA637 from TI/BB, therefore I need to know that this wont be a waste of money to performance that I can get.
ADA4637 has a higher Gain Bandwidth, Slew Rate, and Settling Time than the ADA4627 and I decided to run some simulations to see if it makes sense.... the results are below 🙂
Simulation done with LTSpice IV
Transient response at 1kHz and 10k load shows the highest harmonic at around 5kHz at 81.2106dB separation from the 1k (3kHz harmonic is has slightly larger dB separation around 82dB).
Frequency response shows a small roll-off at 10k to 20k at about -219.924mdB which should be good i guess, and a -3dB rolloff at around 79kHz
This the bare bones circuit from TI's datasheet and I hope to get some feedback from you guys and get a better THD than 81dB. Ideally I want to eliminate the IV/filter/gain stage being noise dominant over the DAC.
Also, all the components are ideal 🙁 except for the ADA4637 models, so this might be a challenge.
All help will be appreciated.
Thanks 🙂
Last edited:
As a decompensated op amp the ADA4637 requires cirucit modifications for use in DAC I/V which are "unity gain" from a stability standpoint
also the Vnoise isn't great - to max S/N you would need much higher than standard consumer audio 2.0 Vrms fs output
my guess is that the ADA4897 is "the best" candidate today for DAC I/V at the "high" ref current levels of the PCM1794, consumer output levels
but with 10 V max supply limit on the chip I would want to use it in a composite amp with a higher Vswing output op amp for the improved performance and because I have an applciation where higher, pro level output would be useful - but I've never seen a published, practical "multiloop" DAC I/V circuit - even though I've simmed some possibilities
also the Vnoise isn't great - to max S/N you would need much higher than standard consumer audio 2.0 Vrms fs output
my guess is that the ADA4897 is "the best" candidate today for DAC I/V at the "high" ref current levels of the PCM1794, consumer output levels
but with 10 V max supply limit on the chip I would want to use it in a composite amp with a higher Vswing output op amp for the improved performance and because I have an applciation where higher, pro level output would be useful - but I've never seen a published, practical "multiloop" DAC I/V circuit - even though I've simmed some possibilities
Last edited:
I like the idea: http://www.diyaudio.com/forums/digi...sford-iv-nested-loop-op-amps.html#post2218591
but Hawsford didn't disclose what"s in the "input filter" box - my sims show there are a few stability issues not explained to the point others could confidently design/scale the multiloop I/V
even my "working" sims are still suspect due to the unrealistic op amp output Z models - I wouldn't say the circuits are "proved" without at least seeing working hardware looked over with 'scope much faster than the op amp GBW
but Hawsford didn't disclose what"s in the "input filter" box - my sims show there are a few stability issues not explained to the point others could confidently design/scale the multiloop I/V
even my "working" sims are still suspect due to the unrealistic op amp output Z models - I wouldn't say the circuits are "proved" without at least seeing working hardware looked over with 'scope much faster than the op amp GBW
Thanks for the catch! I overlooked the non unity gain of the ADA4637. I have found a paper by TI (Using a decompensated op amp for
improved performance) that describes how to compensate the op amp for gains lower than what is specced. Aparently you can get better THD by externaly compensating a decompensated op amp but I couldnt get my head around it yet. Perhaps I will draft up a ADA4627 IV stage with ADA4637 as the gain op amp with filter.
I was able to improve the circuit I presented by shuntig a 0.7uF capacitor at the output before the 100Ohm resistor. The noise level went down several dB and cleaned up the FFT a bit!!! I will post later
I read jcx's thread extensivelly and went over the Hawksford paper but my expertiese limits my understanding of the circuit and how to adjust it to my application. Also the amout of op amps is undesirable :/ (3x per Iout.... 2x3x2 = 12 opamps for the DAC?!?)
I will simulate a ADA4627 IV stage with ADA4637 differential gain/filter and see what comes out 🙂 (i susspect the same thing but we will see)
Also the ADA4637 being decompensated and actually simulating somewhat reasonably good does not give me a lot of confidence in the simulation. It might show me that the ADA4637 PSpice model is stable at unity (might be using the ADA4627 model, slightly modified).
I am also looking at the LME49713 current feedback op amp for the IV 🙂
We will see how it simulates and if I can make the current feedback work.
I found this in the ADA4627/37 models
Will that significantly affect my simulation?
Is that a spice directive command that I have to copy and paste?
Will that significantly affect my simulation?
Is that a spice directive command that I have to copy and paste?
I am not sure your simulation is giving you accurate results. If TI achieved ~120 dB DNR and -110 dB THD measured with this circuit with NE5534, I would not expect numbers so much worse with what is basically an OPA627 clone. Voltage noise is worse, however, at 6.1 nV / rtHz vs 3.5 for NE5534.
Is there some reason you are only considering 627/637?
Is there some reason you are only considering 627/637?
Last edited:
Yeah I am not sure either but it looks a good start but my other simulations are not doing so well as this one.
I tried using the ADA4627...... but there is something funky in the model and I get a "Time step is too small" type of error when trying to do a simple low pass filter... and it takes a million years to simulate in the IV circuit... aka it wont simulate and it looks like it can take days to finish.
I would like to simulate the TI cicuit BUT I cant even do that! I downloaded the Spice model for the NE5534 and put it in the circuit as per the datasheet and it is taking a million years to simulate. It has been an hour and it is at "Damped Pseudo-Transient Analysis: 18.41.. time constants done with no end in sight 🙁
I have also modeled and used the LME49713 in the IV portion and it simulates fast but the Harmonics and noise are ever present and I cant get rid of them :/. I used some app note by AD from 1988 to get the Current Feedback Amp to "work" but it's not looking good. Seems the IV stage is giving all the distortion once again.
Attachments show:
-ADA4637 updated circuit and freq response
-LME49713 IV and ADA4637 amp stage circuit and it's freq response
I want to use the 627/637 due to their better performance specs compared to some other audio op amps. Also the AD versions of the 627/637 are cheaper and you can get samples compared to the TI ones, and I don't see a lot of people using the AD ones so it's worth a try I guess.
The 627/637 gain bandwidth and slew rates are better than most of the other well known audio op amps and the opamps listed on the PCM1794 datasheet. I am open to suggestions tho 🙂, I do want it to sound good.
I would like to sim the TI reference circuit if i can but this LT spice is taking forever... and it will probably give an error at the end or some crappy output
I would say the biggest advantage of the TI OPA627/37 in Audio is the unusually high input Z, especially the dynamic, nonlinear common mode part - which only makes a big difference with large input common mode swing and high, unbalanced source&feedback Z
so the best feature of these op amps is not that important in a DAC I/V with 0 common mode V inverting input and for the PCM1794 currents giving < 1 kOhm feedback Z
I would rate GBW, input noise referred to the circuit conditions, low open loop output Z as more important in DAC I/V
"input linearity" should also be on the 1st order importance list, has some subtleties
slew rate is not 1st order important per se with feedback C, it has in the past been a proxy for good input linearity with higher Vdif, I think the new "highly linear" input stages that AD is doing such a poor job advertising are a "game changer" in the use of bjt input op amps for DAC I/V - I think these change the presumption of fet input being "more linear"
“noise gain compensation” of a decompensated op amp is good with resistive feedback, plenty of design guides, explanations out there
but for DAC I/V with feedback C the “noise gain” feedback becomes a C divider - I worry that a C divider feedback will have additional interactions with the op amp output Z – can still be dealt with if you have some practical info on op amp output Z near the gain intercept, possibly way beyond if local output Q oscillations are possible
Unfortunately maxing out GBW with today’s fast processes put us way beyond the spice macromodel output Z usefulness – sim can’t help us much here if the device designers don’t give use useful output models
We do have the example of Wurcer’s AD797 datasheet app with the input shunt C in a DAV I/V, he adds series R to the feedback C which partially defeats one of the advantages of having the feedback C, and the AD797 stability is known to be a compromise so this may not be a general answer
so the best feature of these op amps is not that important in a DAC I/V with 0 common mode V inverting input and for the PCM1794 currents giving < 1 kOhm feedback Z
I would rate GBW, input noise referred to the circuit conditions, low open loop output Z as more important in DAC I/V
"input linearity" should also be on the 1st order importance list, has some subtleties
slew rate is not 1st order important per se with feedback C, it has in the past been a proxy for good input linearity with higher Vdif, I think the new "highly linear" input stages that AD is doing such a poor job advertising are a "game changer" in the use of bjt input op amps for DAC I/V - I think these change the presumption of fet input being "more linear"
“noise gain compensation” of a decompensated op amp is good with resistive feedback, plenty of design guides, explanations out there
but for DAC I/V with feedback C the “noise gain” feedback becomes a C divider - I worry that a C divider feedback will have additional interactions with the op amp output Z – can still be dealt with if you have some practical info on op amp output Z near the gain intercept, possibly way beyond if local output Q oscillations are possible
Unfortunately maxing out GBW with today’s fast processes put us way beyond the spice macromodel output Z usefulness – sim can’t help us much here if the device designers don’t give use useful output models
We do have the example of Wurcer’s AD797 datasheet app with the input shunt C in a DAV I/V, he adds series R to the feedback C which partially defeats one of the advantages of having the feedback C, and the AD797 stability is known to be a compromise so this may not be a general answer
Attachments
Last edited:
Simulation will tell you very little about whether some I/V circuit will sound good. I've spent hours and hours trying to correlate listening results with the output of LTSpice, to no avail 🙂 As you say your aim is good sound then the most effective route to that goal is breadboarding - listen as you tweak.
A week ago I'd have said abandon the 1794 if you really want good sound, but earlier this week I read a good review on Head-Fi of the Nuforce DAC9 which uses a sister part, the 1798. So decent results are indeed possible. Ultimately though the limitations of their digital noise-shaping loops will be the bottleneck I believe.
A week ago I'd have said abandon the 1794 if you really want good sound, but earlier this week I read a good review on Head-Fi of the Nuforce DAC9 which uses a sister part, the 1798. So decent results are indeed possible. Ultimately though the limitations of their digital noise-shaping loops will be the bottleneck I believe.
Agree and correct! Simulation does not relate to sound quality, but it tells you about the predicted result of design. Since simulation relies on mathematical formula to calculate, it still exists error. The actual result depends on the prototype and the sound quality depends on topology of circuit design.
The advantage of simulation is to shorten your development leadtime, particularly benefit to you if multiple scenario of designs are selected. Since the predicted data or measured value of low distortion, high skew rate, etc.. do not gurantee good sound quality, the final judgement must be done by practical listening test.
Simulation is only as good as the models we use correspond to real components. A recent example:
I had an idea for a discrete MOSFET design for I/V. I planned to use small signal FETs - and I discovered one of those (BSS84) was already included amongst LTSpice's list. So, having been bitten before, I tried the model out by itself to see if the sub-threshold behaviour was modelled correctly. Nope - so I gave up this route. In this case, I either develop my own FET model, or cannibalize someone elses or do it by breadboarding. Seeing as I'm interested more in sound than figures (though I do love getting decent figures!) I'll do this one by breadboarding if I do it at all. Sometimes I turn to LTSpice out of laziness 😉
I had an idea for a discrete MOSFET design for I/V. I planned to use small signal FETs - and I discovered one of those (BSS84) was already included amongst LTSpice's list. So, having been bitten before, I tried the model out by itself to see if the sub-threshold behaviour was modelled correctly. Nope - so I gave up this route. In this case, I either develop my own FET model, or cannibalize someone elses or do it by breadboarding. Seeing as I'm interested more in sound than figures (though I do love getting decent figures!) I'll do this one by breadboarding if I do it at all. Sometimes I turn to LTSpice out of laziness 😉
Well, it was on Head-Fi, where some people are in love with an expensive headphone amp that is based on OPA541 in a bridged configuration 😉.
But, to the OP in all seriousness, you could try ADA4898 which has a similar input stage to the ADA4897 JCX suggested but may work better for you because of it's higher max supply V. If you don't mind a standard BJT input LME49990 or OPA1611 might be ok. The AD1955 and ES9018 (Sabre) both use AD797 in their eval boards and measure extremely well, but as mentioned you must be careful and don't forget the resistor in series with the cap.
Good point - I saw that and had a good chuckle too 😛 One does have to pick carefully the relatively 'credible' reviewers over there....
True that!
I am thinking that I need to look at a couple of other op amps and try a few more simulations to see if I get any good results.
I looked at the ESS white paper on DAC quality improvement and I like some of their opamp suggestions. I am also considering some of the opamps stated in this thread.
I think I will get a couple of op amps that i see the benefit of using. They might be a straight replacement of each other and try to sim them (some will and some wont). after the sim I will probably proceed with a universal PCB IV board that will have +-15V and sufficent footprints that I can swap out different types of op amps and test out how it sounds.
There are a couple of sims that I will try to run first and see if I can get any close to the TI and ESS reference design THD measurements first and post them up here.
I also downloaded Tina TI in order to simulate NE5534 opamp IV stage but at first attempt I am unsucessful... some errors come up and the software is not as intuative as LT spice.
I am thinking that I need to look at a couple of other op amps and try a few more simulations to see if I get any good results.
I looked at the ESS white paper on DAC quality improvement and I like some of their opamp suggestions. I am also considering some of the opamps stated in this thread.
I think I will get a couple of op amps that i see the benefit of using. They might be a straight replacement of each other and try to sim them (some will and some wont). after the sim I will probably proceed with a universal PCB IV board that will have +-15V and sufficent footprints that I can swap out different types of op amps and test out how it sounds.
There are a couple of sims that I will try to run first and see if I can get any close to the TI and ESS reference design THD measurements first and post them up here.
I also downloaded Tina TI in order to simulate NE5534 opamp IV stage but at first attempt I am unsucessful... some errors come up and the software is not as intuative as LT spice.
I found the following paper absolutely invaluable in developing my own (chipamp) model in LTSpice - http://www.analog.com/static/imported-files/application_notes/AN-138.pdf
Thanks! Those are all very good suggestions! I will see which ones I can sim in LTSpice and what comes out.
Yes I have looked at that ESS White paper on DAC quality improvement and the AD797 seems to give them the best figures but it only has 2db advantage over the #2 spot on their chart and the AD797 is at least twice the price of the #2. Also the ADA4627/4637 have better specs than the AD797 and I think there are a couple of more options out there.
Also about the cap and resistor in series in the feedback loop.
What does it do? It looks like something you would see in a current feedback op amp? I'm sure it's filtering something or? What does it exactly do? Will it filter some high frequencies and dissipate them into that resistor in series so it wont affect the output of the opamp?
explanation would be appreciated 🙂
HAHA i looked at that OPA541... and it looks like crap on the datasheet! That thing was not ment for audio and than the price! 😕 oh well, i'll stick to the performance specs and some testing before I start randomly picking opamps hehe
The only reason why I want to use Tina TI is to model the IV stage in the PCM1794A datasheet with the NE5534 opamps..... the spice models of the NE5534 are not working well in LTSpice and it cant simulate :/
So I figure that TI's own program can simulate it's own Spice models but I have to learn Tina to do this one thing 🙁
Thanks for that paper! It's funny how a paper from 20+ years ago is still quite relevant hehe. I will admit tho that I am not as advanced yet as to make my own models but I am sure I will get into it once I learn a lot more about Spice and it's shortcomings.
When I get home I'll try to make a list of opamp choises for sim.
I can also post some fo the LTSpice schematics/sims if you want to take a look at them, maybe something you can figure out in seconds lol
I also get an error that says some of the sort "Node is floating U:99" or something. But every pin is connected 😡
I don't have a problem with TI's NE5534 - did you add the comp pins, add the 22 pF comp C?
.asy symbol with comp pins has to be added where you can find it - edit off the .txt extension
also had extra character at end of TI's model file that I deleted when pasting the text into Ltspice' "Spice directive" box (far right tool bar button)
the AN138 PMI op amp modeling paper is great - too bad AD doesn't actually use it now - some AD project engineers/spice model authors don't understand it
.asy symbol with comp pins has to be added where you can find it - edit off the .txt extension
also had extra character at end of TI's model file that I deleted when pasting the text into Ltspice' "Spice directive" box (far right tool bar button)
the AN138 PMI op amp modeling paper is great - too bad AD doesn't actually use it now - some AD project engineers/spice model authors don't understand it
Attachments
Last edited:
How about doing the i/v conversion on single chip sharing positive and negative supplies plus steering the current from + and - iout of the DAC? Seems to be a perfect job for fully-balanced opamps as OPA1632. Let the harmonics/glitches cancel out not in the summation circuit, but in the i/v opamp itself...
Here - DAC ????????????? ?????? v1.2 - ????????? ??????? - PCM1794A Picardian chord S/PDIF WM8804 - Overture audio
Proper filtering is essential as no opamp circuit could deal nicely with all the noise of DS DACs.
Here - DAC ????????????? ?????? v1.2 - ????????? ??????? - PCM1794A Picardian chord S/PDIF WM8804 - Overture audio
Proper filtering is essential as no opamp circuit could deal nicely with all the noise of DS DACs.
- Status
- Not open for further replies.