Forums

simulating a digital control loop

Started by John Larkin March 29, 2010
I'm designing a gadget that uses an ARM uP, with 12-bit mux'd ADC and
a 10-bit DAC, to essentially make a current and voltage regulated
power supply. The ADC will measure voltage and current and the DAC
will control a fairly soft source-follower series-pass mosfet. The
customer load could be most anything.

I think it would be time-effective to simulate the control loop while
the PC board is being fabbed, so we don't have to play with dynamics
as much in the critical delivery path. 

I can simulate it as an analog loop using LT Spice, as I'm familiar
with that and could get it done quickly. It would be handy if I could
also use the same model in digital mode, which would add sampling
delays and maybe even quantization.

Any thoughts on how to do this?

I note here that more and more formerly-analog control loops, things
like switching power supplies, motor drivers, power amps, will be
going digital in the future. Some of the ARM chips are selling for
under a dollar. Analog parts will, I think, increasingly be used for
things like amplification, and less for computation.

John


John Larkin wrote:

> I'm designing a gadget that uses an ARM uP, with 12-bit mux'd ADC and > a 10-bit DAC, to essentially make a current and voltage regulated > power supply. The ADC will measure voltage and current and the DAC > will control a fairly soft source-follower series-pass mosfet. The > customer load could be most anything. > > I think it would be time-effective to simulate the control loop while > the PC board is being fabbed, so we don't have to play with dynamics > as much in the critical delivery path. > > I can simulate it as an analog loop using LT Spice, as I'm familiar > with that and could get it done quickly. It would be handy if I could > also use the same model in digital mode, which would add sampling > delays and maybe even quantization. > > Any thoughts on how to do this? > > I note here that more and more formerly-analog control loops, things > like switching power supplies, motor drivers, power amps, will be > going digital in the future. Some of the ARM chips are selling for > under a dollar. Analog parts will, I think, increasingly be used for > things like amplification, and less for computation.
You can simulate digital loops in the analog simulator quite accurately. The main problem is how to do delay by one sample. In the simple cases, this can be simulated as 1-st order phase shifter; you may need better approximation as you get closer to Nyquist. Another way to simulate digital circuit is by switched capacitor sircuit (beware of convergence problems). I've done it both ways; it is possible to get reasonably accurate results if you know and understand the properties and limitations of both analog and digital methods. Vladimir Vassilevsky DSP and Mixed Signal Design Consultant http://www.abvolt.com
On Mon, 29 Mar 2010 09:11:48 -0700, John Larkin
<jjlarkin@highNOTlandTHIStechnologyPART.com> wrote:

>I'm designing a gadget that uses an ARM uP, with 12-bit mux'd ADC and >a 10-bit DAC, to essentially make a current and voltage regulated >power supply. The ADC will measure voltage and current and the DAC >will control a fairly soft source-follower series-pass mosfet. The >customer load could be most anything. > >I think it would be time-effective to simulate the control loop while >the PC board is being fabbed, so we don't have to play with dynamics >as much in the critical delivery path. > >I can simulate it as an analog loop using LT Spice, as I'm familiar >with that and could get it done quickly. It would be handy if I could >also use the same model in digital mode, which would add sampling >delays and maybe even quantization. > >Any thoughts on how to do this? > >I note here that more and more formerly-analog control loops, things >like switching power supplies, motor drivers, power amps, will be >going digital in the future. Some of the ARM chips are selling for >under a dollar. Analog parts will, I think, increasingly be used for >things like amplification, and less for computation. > >John
You can use ptolemy or matlab. Either can do the job you're trying pretty well. -- Muzaffer Kal DSPIA INC. ASIC/FPGA Design Services http://www.dspia.com
John Larkin wrote:
> I'm designing a gadget that uses an ARM uP, with 12-bit mux'd ADC and > a 10-bit DAC, to essentially make a current and voltage regulated > power supply. The ADC will measure voltage and current and the DAC > will control a fairly soft source-follower series-pass mosfet. The > customer load could be most anything. > > I think it would be time-effective to simulate the control loop while > the PC board is being fabbed, so we don't have to play with dynamics > as much in the critical delivery path. > > I can simulate it as an analog loop using LT Spice, as I'm familiar > with that and could get it done quickly. It would be handy if I could > also use the same model in digital mode, which would add sampling > delays and maybe even quantization. > > Any thoughts on how to do this? > > I note here that more and more formerly-analog control loops, things > like switching power supplies, motor drivers, power amps, will be > going digital in the future. Some of the ARM chips are selling for > under a dollar. Analog parts will, I think, increasingly be used for > things like amplification, and less for computation.
For analysis with a linearized plant see chapter 7 of my book: http://www.wescottdesign.com/actfes/actfes.html. If you're trying to simulate the loop with all of it's nonlinearities then Vladimir's suggestion of a one-cycle delay sounds smart. I don't know if there's a reasonable way to add quantization, though. You may want to consider a sample-and-hold circuit to simulate the action of the DAC and of any internal integrators instead of the delay; in theory it'd be more accurate. I wish that someone made an easy integration between some C-like scripting language and a circuit simulator (BTW: if it costs more than a new car it's not easy). Then you could implement your control algorithm in something resembling its native form, and still get a "real" circuit simulation. -- Tim Wescott Control system and signal processing consulting www.wescottdesign.com
On Mon, 29 Mar 2010 11:26:39 -0500, Vladimir Vassilevsky
<nospam@nowhere.com> wrote:

> > >John Larkin wrote: > >> I'm designing a gadget that uses an ARM uP, with 12-bit mux'd ADC and >> a 10-bit DAC, to essentially make a current and voltage regulated >> power supply. The ADC will measure voltage and current and the DAC >> will control a fairly soft source-follower series-pass mosfet. The >> customer load could be most anything. >> >> I think it would be time-effective to simulate the control loop while >> the PC board is being fabbed, so we don't have to play with dynamics >> as much in the critical delivery path. >> >> I can simulate it as an analog loop using LT Spice, as I'm familiar >> with that and could get it done quickly. It would be handy if I could >> also use the same model in digital mode, which would add sampling >> delays and maybe even quantization. >> >> Any thoughts on how to do this? >> >> I note here that more and more formerly-analog control loops, things >> like switching power supplies, motor drivers, power amps, will be >> going digital in the future. Some of the ARM chips are selling for >> under a dollar. Analog parts will, I think, increasingly be used for >> things like amplification, and less for computation. > >You can simulate digital loops in the analog simulator quite accurately. > The main problem is how to do delay by one sample. In the simple >cases, this can be simulated as 1-st order phase shifter; you may need >better approximation as you get closer to Nyquist. Another way to >simulate digital circuit is by switched capacitor sircuit (beware of >convergence problems). >I've done it both ways; it is possible to get reasonably accurate >results if you know and understand the properties and limitations of >both analog and digital methods.
I'd be happy with a 1 millisecond risetime, and can run the loop iteration ballpark 50 KHz, so my integration constants will be small. Given that, I can probably ignore sampling issues or, as you suggest, just throw in something like RC delays to approximate the effects of sampling. Simulating quantization would be interesting. I'll effectively (maybe even on purpose) be dithering the ADC and especially the DAC to more bits than they actually have. Hmmm... if I put an analog lowpass between the ADC and the mosfet (it's there already to deglitch, and I can play with the tau) the PID loop sort of dithers the DAC all by itself. And that dithers the ADC. All for free. John
John Larkin a &#2013265929;crit :
> I'm designing a gadget that uses an ARM uP, with 12-bit mux'd ADC and > a 10-bit DAC, to essentially make a current and voltage regulated > power supply. The ADC will measure voltage and current and the DAC > will control a fairly soft source-follower series-pass mosfet. The > customer load could be most anything. > > I think it would be time-effective to simulate the control loop while > the PC board is being fabbed, so we don't have to play with dynamics > as much in the critical delivery path. > > I can simulate it as an analog loop using LT Spice, as I'm familiar > with that and could get it done quickly. It would be handy if I could > also use the same model in digital mode, which would add sampling > delays and maybe even quantization. > > Any thoughts on how to do this? > > I note here that more and more formerly-analog control loops, things > like switching power supplies, motor drivers, power amps, will be > going digital in the future. Some of the ARM chips are selling for > under a dollar. Analog parts will, I think, increasingly be used for > things like amplification, and less for computation. > > John >
It can easily done with spice. The software delay can be modeled as a TLINE provided it is constant in your system. For switchers you model the switch as an averaged one (continuous model). The sampling action is modeled by a 2 poles TF (look at Ridley's paper "Accurate and practical small signal model for current mode control", or I can try to dig in one of my previous HDs). With good modeling you can have average transient and AC (loop gain,...) simulations which are real close to the actual circuit. That won't give you quantization though, and I guess this can't be modeled as with sigma delta since you have a first order loop and probably an almost constant signal. Maybe, but I never tried this, you can discretize the loop (only for transient analysis) with use of B "arbitrary sources" within which you use some integer part function. I don't know whether LTspice support B sources, but you should find something equivalent... -- Thanks, Fred.
Fred Bartoli wrote:
> John Larkin a &#2013265929;crit : >> I'm designing a gadget that uses an ARM uP, with 12-bit mux'd ADC and >> a 10-bit DAC, to essentially make a current and voltage regulated >> power supply. The ADC will measure voltage and current and the DAC >> will control a fairly soft source-follower series-pass mosfet. The >> customer load could be most anything. >> >> I think it would be time-effective to simulate the control loop while >> the PC board is being fabbed, so we don't have to play with dynamics >> as much in the critical delivery path. >> I can simulate it as an analog loop using LT Spice, as I'm familiar >> with that and could get it done quickly. It would be handy if I could >> also use the same model in digital mode, which would add sampling >> delays and maybe even quantization. >> >> Any thoughts on how to do this? >> >> I note here that more and more formerly-analog control loops, things >> like switching power supplies, motor drivers, power amps, will be >> going digital in the future. Some of the ARM chips are selling for >> under a dollar. Analog parts will, I think, increasingly be used for >> things like amplification, and less for computation. >> >> John >> > > It can easily done with spice. > > The software delay can be modeled as a TLINE provided it is constant in > your system. > For switchers you model the switch as an averaged one (continuous > model). The sampling action is modeled by a 2 poles TF (look at Ridley's > paper "Accurate and practical small signal model for current mode > control", or I can try to dig in one of my previous HDs). > > With good modeling you can have average transient and AC (loop gain,...) > simulations which are real close to the actual circuit. > > That won't give you quantization though, and I guess this can't be > modeled as with sigma delta since you have a first order loop and > probably an almost constant signal. > > Maybe, but I never tried this, you can discretize the loop (only for > transient analysis) with use of B "arbitrary sources" within which you > use some integer part function. I don't know whether LTspice support B > sources, but you should find something equivalent... > >
Quantization looks like infinite gain, though, so unless it is wrapped inside of a sampled-time section it'll really slow down -- or completely crash -- the simulation. You can analyze fairly well for quantization by treating it as noise at the magnitude of the quantization, and the worst possible frequency. Just inject a signal at the quantization point, do a frequency sweep to figure out the sensitivity of the output to the quantization, and take the worst spot. Quantization always seems to seek to do the most damage possible, so treating it as worst case isn't paranoid. In this case, it really is out to get you! -- Tim Wescott Control system and signal processing consulting www.wescottdesign.com
On Mon, 29 Mar 2010 09:11:48 -0700, John Larkin
<jjlarkin@highNOTlandTHIStechnologyPART.com> wrote:

>I'm designing a gadget that uses an ARM uP, with 12-bit mux'd ADC and >a 10-bit DAC, to essentially make a current and voltage regulated >power supply. The ADC will measure voltage and current and the DAC >will control a fairly soft source-follower series-pass mosfet. The >customer load could be most anything. > >I think it would be time-effective to simulate the control loop while >the PC board is being fabbed, so we don't have to play with dynamics >as much in the critical delivery path. > >I can simulate it as an analog loop using LT Spice, as I'm familiar >with that and could get it done quickly. It would be handy if I could >also use the same model in digital mode, which would add sampling >delays and maybe even quantization. > >Any thoughts on how to do this? > >I note here that more and more formerly-analog control loops, things >like switching power supplies, motor drivers, power amps, will be >going digital in the future. Some of the ARM chips are selling for >under a dollar. Analog parts will, I think, increasingly be used for >things like amplification, and less for computation.
Might look at Visual ModelQ http://www.qxdesign.com/. It has been some years since I played with it but it does include blocks for, e.g., sample & hold functions, delays, and digital filters. IIRC, the free downloadable version is fully capable but won't allow saving more complex models. -- Rich Webb Norfolk, VA
Tim Wescott a &#2013265929;crit :
> Fred Bartoli wrote: >> John Larkin a &#2013265929;crit : >>> I'm designing a gadget that uses an ARM uP, with 12-bit mux'd ADC and >>> a 10-bit DAC, to essentially make a current and voltage regulated >>> power supply. The ADC will measure voltage and current and the DAC >>> will control a fairly soft source-follower series-pass mosfet. The >>> customer load could be most anything. >>> >>> I think it would be time-effective to simulate the control loop while >>> the PC board is being fabbed, so we don't have to play with dynamics >>> as much in the critical delivery path. >>> I can simulate it as an analog loop using LT Spice, as I'm familiar >>> with that and could get it done quickly. It would be handy if I could >>> also use the same model in digital mode, which would add sampling >>> delays and maybe even quantization. >>> >>> Any thoughts on how to do this? >>> >>> I note here that more and more formerly-analog control loops, things >>> like switching power supplies, motor drivers, power amps, will be >>> going digital in the future. Some of the ARM chips are selling for >>> under a dollar. Analog parts will, I think, increasingly be used for >>> things like amplification, and less for computation. >>> >>> John >>> >> >> It can easily done with spice. >> >> The software delay can be modeled as a TLINE provided it is constant >> in your system. >> For switchers you model the switch as an averaged one (continuous >> model). The sampling action is modeled by a 2 poles TF (look at >> Ridley's paper "Accurate and practical small signal model for current >> mode control", or I can try to dig in one of my previous HDs). >> >> With good modeling you can have average transient and AC (loop >> gain,...) simulations which are real close to the actual circuit. >> >> That won't give you quantization though, and I guess this can't be >> modeled as with sigma delta since you have a first order loop and >> probably an almost constant signal. >> >> Maybe, but I never tried this, you can discretize the loop (only for >> transient analysis) with use of B "arbitrary sources" within which you >> use some integer part function. I don't know whether LTspice support B >> sources, but you should find something equivalent... >> >> > Quantization looks like infinite gain, though, so unless it is wrapped > inside of a sampled-time section it'll really slow down -- or completely > crash -- the simulation. > > You can analyze fairly well for quantization by treating it as noise at > the magnitude of the quantization, and the worst possible frequency. > Just inject a signal at the quantization point, do a frequency sweep to > figure out the sensitivity of the output to the quantization, and take > the worst spot. > > Quantization always seems to seek to do the most damage possible, so > treating it as worst case isn't paranoid. In this case, it really is > out to get you! >
It's been a while I've looked at this but IIRC it's only one bit quantizer that have infinite gain. Multibit quantizers, as I guess John will use since he has plentiful bits ADC/DAC, have unit gain. I once used an ARM with 12b ADC/DACs to build a low OSR SD converter with real high resolution at almost no cost (the ARM was mandated for other things). Of course it wasn't more linear than the DAC on large signals, but the app was OK with that... -- Thanks, Fred.
Fred Bartoli wrote:
> Tim Wescott a &#2013265929;crit : >> Fred Bartoli wrote: >>> John Larkin a &#2013265929;crit : >>>> I'm designing a gadget that uses an ARM uP, with 12-bit mux'd ADC and >>>> a 10-bit DAC, to essentially make a current and voltage regulated >>>> power supply. The ADC will measure voltage and current and the DAC >>>> will control a fairly soft source-follower series-pass mosfet. The >>>> customer load could be most anything. >>>> >>>> I think it would be time-effective to simulate the control loop while >>>> the PC board is being fabbed, so we don't have to play with dynamics >>>> as much in the critical delivery path. >>>> I can simulate it as an analog loop using LT Spice, as I'm familiar >>>> with that and could get it done quickly. It would be handy if I could >>>> also use the same model in digital mode, which would add sampling >>>> delays and maybe even quantization. >>>> >>>> Any thoughts on how to do this? >>>> >>>> I note here that more and more formerly-analog control loops, things >>>> like switching power supplies, motor drivers, power amps, will be >>>> going digital in the future. Some of the ARM chips are selling for >>>> under a dollar. Analog parts will, I think, increasingly be used for >>>> things like amplification, and less for computation. >>>> >>>> John >>>> >>> >>> It can easily done with spice. >>> >>> The software delay can be modeled as a TLINE provided it is constant >>> in your system. >>> For switchers you model the switch as an averaged one (continuous >>> model). The sampling action is modeled by a 2 poles TF (look at >>> Ridley's paper "Accurate and practical small signal model for current >>> mode control", or I can try to dig in one of my previous HDs). >>> >>> With good modeling you can have average transient and AC (loop >>> gain,...) simulations which are real close to the actual circuit. >>> >>> That won't give you quantization though, and I guess this can't be >>> modeled as with sigma delta since you have a first order loop and >>> probably an almost constant signal. >>> >>> Maybe, but I never tried this, you can discretize the loop (only for >>> transient analysis) with use of B "arbitrary sources" within which >>> you use some integer part function. I don't know whether LTspice >>> support B sources, but you should find something equivalent... >>> >>> >> Quantization looks like infinite gain, though, so unless it is wrapped >> inside of a sampled-time section it'll really slow down -- or >> completely crash -- the simulation. >> >> You can analyze fairly well for quantization by treating it as noise >> at the magnitude of the quantization, and the worst possible >> frequency. Just inject a signal at the quantization point, do a >> frequency sweep to figure out the sensitivity of the output to the >> quantization, and take the worst spot. >> >> Quantization always seems to seek to do the most damage possible, so >> treating it as worst case isn't paranoid. In this case, it really is >> out to get you! >> > > It's been a while I've looked at this but IIRC it's only one bit > quantizer that have infinite gain. Multibit quantizers, as I guess John > will use since he has plentiful bits ADC/DAC, have unit gain. > I once used an ARM with 12b ADC/DACs to build a low OSR SD converter > with real high resolution at almost no cost (the ARM was mandated for > other things). Of course it wasn't more linear than the DAC on large > signals, but the app was OK with that... >
At the point of the quantization step the input moves an infinitesimal amount, and the output moves a finite amount. That's an infinite gain. With a 12-bit device, it happens 4095 times, instead of once. -- Tim Wescott Control system and signal processing consulting www.wescottdesign.com