quantizer for LT Spice

Shouldn't those steps spend equal time inside and outside the sine wave?

Grant.

Use round() instead of int():

SYMATTR Value V=round(5*V(X))/5

"John Larkin" schrieb im Newsbeitrag news: snipped-for-privacy@4ax.com...

Hello John,

Here is an example with the "Sample"-device.

Best regards, Helmut

Version 4 SHEET 1 920 680 WIRE -112 -16 -160 -16 WIRE 176 0 144 0 WIRE -160 32 -160 -16 WIRE 448 48 352 48 WIRE 592 48 544 48 WIRE 176 64 144 64 WIRE 544 80 544 48 WIRE -160 144 -160 112 WIRE -112 208 -160 208 WIRE 544 208 544 160 WIRE -160 256 -160 208 WIRE -160 368 -160 336 FLAG 544 208 0 FLAG 592 48 sq IOPIN 592 48 Out FLAG -160 144 0 FLAG -112 -16 s0 FLAG 144 0 s0 FLAG -160 368 0 FLAG -112 208 fs FLAG 144 64 fs FLAG 448 48 vs0 SYMBOL bv 544 64 R0 SYMATTR InstName B1 SYMATTR Value V=int(V(vs0)) SYMBOL voltage -160 16 R0 WINDOW 123 0 0 Left 0 WINDOW 39 0 0 Left 0 SYMATTR InstName V1 SYMATTR Value SINE(0 7.5 {f0}) SYMBOL SpecialFunctions\\sample 256 32 R0 WINDOW 3 0 0 Invisible 0 SYMATTR InstName A1 SYMATTR Value2 vhigh=1e6 vlow=-1e6 SYMATTR Value vt=0.5 SYMBOL voltage -160 240 R0 WINDOW 123 0 0 Left 0 WINDOW 39 0 0 Left 0 SYMATTR InstName V2 SYMATTR Value PULSE(0 1 0 1n 1n 10u {1/fs}) TEXT -176 -160 Left 0 !.tran 0 3m 0 1u TEXT -176 -128 Left 0 !.options plotwinsize=0 TEXT -176 -96 Left 0 !.param f0=1k fs=20k

Where's the CLOCK? ...Jim Thompson

That depends on your personal definition of "quantizer." Once the structure is there, one can play with the equation. I'll be simulating a 12-bit ADC and a 10-bit DAC, so exactly where the transitions happen doesn't matter much.

John

That does look a little nicer.

John

Hmm, I like zero accumulated errors, so your staircase waveform looked somewhat anorexic to me ;) I imagine the quantised waveform being filtered back to sinewave.

Yep, except I had no idea where to find the 'lever' to change it, but another poster already pointed that out.

Only recently did I start playing with LTSpice, much to learn as I've not used spice before (returning to electronics design after a 'short' break in 1993).

Grant.

"round" does look nicer, in having zero average errors through the quantizer. I'm mostly interested in how using the ADC and DAC in the NXP ARM will change the dynamics of a loop that I'm simulating as all analog but will in fact be digital. The uP has a 10-bit DAC, which isn't good enough, so if we oversample hard (100 KHz) and add some lowpass filtering downstream of the dac, we should be able to dither a few more bits. That part will be interesting to simulate, but doesn't care much how the quantizers round. The actual NXP ADC and DAC will do whatever they do.

I find the HELP in LT Spice to be a bit abstract and not terribly consistent. More examples would be great. At least one can come to s.e.d. and ususlly find somebody who knows how to do what you need.

For basic stuff, LT Spice is great and eesy to drive. I can't imagine how much it has cost the people who sell simulators.

John

Yeah, Mike E should be arrested for "using a computer to destroy their business model"... Why did you do it Mike?? :) :)

Seriously, LTSPice is great, thank you LTC.

The quantizer works fine. But when I poke a couple of quantizers into my control loop model, to simulate ADC quantization, it runs for hours instead of a fraction of a second. I don't know if it will ever finish.

There's a message at the bottom of the screen:

Damped Pseudo-Transient Analysis: 0.xxxxx time constants; blah blah press ESC to quit.

where xxx is increasing like an RC exponential, ie slower and slower.

What does all that mean?

I could program this system, quantization and all, in PowerBasic and I know it would run fast. But I may as well just build the board and see what happens, the best model being the thing itself. We can always tweak the code (or the specs!) as required.

John

Which simulator are you using? Perhaps the infinite steepness of the steps are causing problems. Maybe try to use an RC filter on the output.

Most home-brew behavioral modeling fails because the inexperienced modeler makes the function ideal, failing to understand what arbitrarily fast edges do to simulators.

Ideal diodes can do that :-)

That's why much of the behavioral stuff I've posted uses the TANH function... smooth, with ALL derivatives existing and finite. ...Jim Thompson

Good mixed-mode simulators (like what you find in Matlab or Scilab) "understand" sampled-time, and can naturally shift from continuous-time to sampled time. This is one of the things that I was "asking" for when I expressed an interest in mixing processor behavior with analog.

The simulator I pine for neither needs nor wants to simulate all the electrical states of the processor or controller -- it wants to do all of that numerically, and on a strictly sampled-time basis. But to do that it needs a clean break between continuous-time simulation and sampled time simulation.

(note too that when you're 'behind' the sampled-time firewall you can do things like quantization without causing problems with infinite slopes, as long as you don't have any algebraic loops).

I have the "fancy" mixed-mode version of PSpice A/D+, handling mixed analog/digital circuitry.

Plus I've made a number of personalized D2A and A2D "tools" to keep digital separated from analog... keeping the screaming speed.

My behavioral 10-bit A-to-D runs in minutes, while the fully device-level version takes all night :-) ...Jim Thompson

The nice thing about using Spice to simulate a mostly-digital control system (I'm using LT Spice here) is that I can drop in models of mosfets and opamps and zeners and such, the actual analog parts that will be outside the uP. And all the schematic/sim/graphing tools are familiar. The more general system sim programs probably don't do a very good, or at least very easy, model of electronic components. And LT Spice is free!

I'd do it in PowerBasic except that I think the sampling and quantizations are unlikely to have much practical effect on my control loop, and we can tweak the ARM code as needed to make it work. I was interested to see if/how the loop would self-dither itself, but I'll just wait to see the real thing.

John

Hi and greetings from pakistan.

I need to understand a little bit about how to implement this code in LTspi ce since i am relatively new and have no previous experience in spice envir onment (except for a LAB), i would like to know how to implement this quant izer netlist in LTspice. Because whenever i try to run the code (by saving it as .cir file) , it gives some error like Multiple flag syntex error. Kin dly guide me as this is very important for my final year engineering projec t.

Thanks !

Hi and greetings from San Francisco. It's chilly and foggy here right now. What's the weather like in Pakistan? Are you having that heat wave?

Here's a quantizer:

Version 4 SHEET 1 880 680 WIRE 48 48 0 48 WIRE 112 48 48 48 WIRE 384 48 320 48 WIRE 432 48 384 48 WIRE 0 96 0 48 WIRE 112 112 112 48 WIRE 320 112 320 48 WIRE 432 128 432 48 WIRE 0 224 0 176 WIRE 112 224 112 192 WIRE 320 240 320 192 WIRE 432 240 432 208 FLAG 0 224 0 FLAG 320 240 0 FLAG 112 224 0 FLAG 432 240 0 FLAG 48 48 X FLAG 384 48 OUT SYMBOL bv 320 96 R0 WINDOW 3 -51 189 Left 2 WINDOW 0 -53 6 Left 2 SYMATTR Value V=int(5.1*V(X))*0.2 SYMATTR InstName B1 SYMBOL voltage 0 80 R0 WINDOW 3 -60 206 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 WINDOW 0 -59 7 Left 2 SYMATTR Value SINE(0 1 1k 0 0 0 3) SYMATTR InstName V1 SYMBOL res 96 96 R0 WINDOW 0 52 41 Left 2 WINDOW 3 52 71 Left 2 SYMATTR InstName R1 SYMATTR Value 1k SYMBOL res 416 112 R0 WINDOW 0 47 31 Left 2 WINDOW 3 47 68 Left 2 SYMATTR InstName R2 SYMATTR Value 1k TEXT 536 200 Left 2 !.tran 0 .005 0 1u TEXT 552 72 Left 2 ;QUANTIZER TEXT 576 120 Left 2 ;J Larkin

Copy that into a text editor and save as QUANT.ASC. Then LT Spice should open it. Click the "runing man" symbol, then probe around.

Wow, that was easy...thanks you very much, sir !

And we are having a monsoon here, so a really lot of clouds coming from eve ry where. Also, there are floods in every river of Pakistan (due to heavy r ain) and they are causing some serious damage to the whole economy. Please keep praying for us and for me as well ( because i am having a very bad thr oat ache :@)

Again, thank you very much !

BTw, one more thing i need to know is that how do i get the whole circuit o f quantizer (All those bunch of gates, capacitors,resistors etc we use )? I mean the way you told me to get waveforms just gives a simple input output circuit and its waveforms. I , and my groupmates, need to understand more about that quantizer circuit and that little input output circuit isnt much helping ....Thanks again :)