[LTSPICE] mixer needed

cool thanks, i was hoping for a symbol, this will do fine tho :) took me a little while to figure out the syntax from the help file but got it to do what i want now.

Colin =^.^=

"colin" schrieb im Newsbeitrag news:XxTse.22599$ snipped-for-privacy@newsfe3-gui.ntli.net...

Hello Colin,

You can have as many multiplier as you like. Use either a B-voltage source or a a B-current source for the required multiplication.

V=V(x1)*V(x2)

Don't forget to set a maximum timestep and to switch off data compression.

The quality of the settings can be checked with the FFT.

..tran 0 20m 0 10u ..options plotwinsize=0

Best regards, Helmut

LTspice/SwitcherCADIII is free SPICE with GUI from

. It outperforms the commercial SPICEs in many features. Give it a try!

The independent user group for LTspice is here:

I have no affiliation with Linear Technology.

Example:

• C:\Programme\LTC\SwCADIII\Draft13.asc V1 x1 0 SINE(0 1 1k) V2 x2 0 SINE(0 1 1100) B1 y 0 V=V(x1)*V(x2) ..options plotwinsize=0 ..tran 0 20m 0 10u ..backanno ..end

Schematic: draft13.asc

Version 4 SHEET 1 880 680 WIRE -176 160 -176 144 WIRE -176 256 -176 240 WIRE -176 352 -176 336 WIRE -176 448 -176 432 WIRE 96 160 96 128 WIRE 96 256 96 240 FLAG -176 256 0 FLAG -176 448 0 FLAG -176 336 x2 FLAG -176 144 x1 FLAG 96 256 0 FLAG 96 128 y SYMBOL voltage -176 144 R0 WINDOW 123 0 0 Left 0 WINDOW 39 0 0 Left 0 SYMATTR InstName V1 SYMATTR Value SINE(0 1 1k) SYMBOL bv 96 144 R0 SYMATTR InstName B1 SYMATTR Value V=V(x1)*V(x2) SYMBOL voltage -176 336 R0 WINDOW 123 0 0 Left 0 WINDOW 39 0 0 Left 0 SYMATTR InstName V2 SYMATTR Value SINE(0 1 1100) TEXT -160 40 Left 0 !.options plotwinsize=0 TEXT -160 8 Left 0 !.tran 0 20m 0 10u

ok my next problem is i need to introduce a sinusoidaly varying time delay into a signal, i cant think what i can use to do this, in the real world it is the result of varying transmision distance wich is what i wish to examine the effects of .. any ideas ? i cant use the sffm as it is not a single frequency.

Colin =^.^=

delay

Hi Helmut, thanks again, this would be fine if my signal was a single frequency, but then i cld use the sffm FM modulator, but unfortunatly i cant reduce it to a sinewave, i need something that effectivly adds PM to an existing voltage node within the simulator and i cant see any functions in b-Source that i could do that with.

maybe i need to do something like make a model for a transmision line and vary the length ?

I gues as a last resort I could make a lumped transmision line with varactors etc.

Colin =^.^=

"colin" schrieb im Newsbeitrag news:i4Xse.23556$ snipped-for-privacy@newsfe3-gui.ntli.net...

Hello Colin,

No problem. The B-source can do it. The variable "time" is available in the behavioral sources(B).

V=sin(2*pi*f0*(time+deltaTime*sin(2*pi*fdelta*time)))

With numbers:

V=sin(2*pi*1k*(time+0.1m*sin(2*pi*10*time)))

This is a 1kHz sine waveform with a varying delay of +/- 0.1ms and a frequency of 10Hz.

Increase your time window for the FFT to multiples of 0.1 seconds in this case. You should also rise the number of samples in the FFT to 131072. The spectrum looks like PM.

Best regards, Helmut

single

and

Hi, thanks again, this is interesting as there is no mention of the delay function in the help section, it pays to ask :)

I tried to put a variable in the delay, it would not accept the sine function eg V=delay(v(a),sine(time)) but it would accept V=delay(v(a),0.001+time/1000) wich gives the result expected it also accepted a voltage as the second term eg V=delay(v(a),v(b)) wich is interesting as i can use a sine voltage, however it does give rather jumpy results but i expect i can improve this with tstep etc.

I gues i could also add sinousoudaly varying amounts of the delayed and non delayed voltage.

Colin =^.^=

"colin" schrieb im Newsbeitrag news:sUXse.23584$ snipped-for-privacy@newsfe3-gui.ntli.net...

Hello Colin,

Sorry for misunderstanding your desire.

There is a delay function in LTspice, but it's only ok to use it with a constant delay. This means you could only change the delay in a stepped simulation(.step). It is not intended for varying delays.

V=delay(V(x1), 0.1m)

or

..step param DELAY1 0 0.1m 0.02m V=delay(V(x1),{DELAY1})

Best regards, Helmut

time

to

do

jumpy

delay.

Hi,

thanks yet again, I see, it is grinding to a halt during the simulation with sim speed going down 1to 1ps/s every time the delay apraoches zero wich is making it dificult to set a long enough time so i can see if the right spectrum is there.

il try and use the mix of two diferent but constant delays to see if this is better.

Colin =^.^=

"colin" schrieb im Newsbeitrag news:0LZse.23768$ snipped-for-privacy@newsfe3-gui.ntli.net...

Hello Colin,

I have seen very strange and wrong results when using a non constant delay.

Finally, I wouldn't trust a simulation which uses varying delay values in the delay() function.

Best regards, Helmut

it

examine

this is what i came up with finaly .. it produces a nice phase mod spectrum.

• C:\Program Files\LTC\SwCADIII\Draft5.asc V1 a 0 SINE(0 1 100khz) ..tran 0 .005 0 5n ..subckt phasemod in out BV out 0 V=(v(in)*(1+sin(2*pi*time*{freq}))+delay(V(in),{t})*(1-sin(2*pi*time*{freq}) ))/2 ..ends phasemod X1 a x phasemod t=.1us freq=1000 ..end

it would be nice to be able to put this into the transmision line symbol somehow

Colin =^.^=