LTspice questions

[Bill Bowden]

Does LTspice assume some value of Q when simulating parallel LC
circuits where the resistance of the inductor and ESR of the capacitor
are not specified? I notice I get different results where the L or C
resistance is not stated, but the simulator works ok and just displays
weird waveforms. It seems to assume something.

Another question I have is how to write a directive to sweep a
bandpass filter from F1 to F2 to get a dB display of the response from
input to output over the frequency range?

Thanks,

-Bill

 

[Fred Abse]

On Wed, 06 Jun 2012 20:48:34 -0700, Bill Bowden wrote:

Does LTspice assume some value of Q when simulating parallel LC circuits
where the resistance of the inductor and ESR of the capacitor are not
specified? I notice I get different results where the L or C resistance
is not stated, but the simulator works ok and just displays weird
waveforms. It seems to assume something.

LTSpice supplies a minimum damping resistance to inductors, unless you
turn it off in Control Panel/Hacks or override it with a specified value
for individual inductors. (Hint: specifying Rs=0 will confuse the
simulator in circumstances where there is no external damping, use some
value like 1E-18 in such cases.)

Another question I have is how to write a directive to sweep a bandpass
filter from F1 to F2 to get a dB display of the response from input to
output over the frequency range?

..ac <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq>

You need to specify a source of AC 0V.

Then plot the voltage at the output node. You can have Bode, Nyquist, or
Cartesian plots.

RTFM.

Try this: TURN OFF WRAPPING!

Coupling.asc
------------------

Version 4
SHEET 1 880 680
WIRE -32 96 -64 96
WIRE 96 96 48 96
WIRE 144 96 96 96
WIRE 336 96 272 96
WIRE 448 96 336 96
WIRE 144 128 144 96
WIRE 272 128 272 96
WIRE 336 128 336 96
WIRE 96 144 96 96
WIRE -64 160 -64 96
WIRE 448 160 448 96
WIRE 96 224 96 208
WIRE 144 224 144 208
WIRE 144 224 96 224
WIRE -64 320 -64 240
WIRE 64 320 -64 320
WIRE 144 320 144 224
WIRE 144 320 64 320
WIRE 272 320 272 208
WIRE 272 320 144 320
WIRE 336 320 336 192
WIRE 336 320 272 320
WIRE 448 320 448 240
WIRE 448 320 336 320
WIRE 64 368 64 320
FLAG 64 368 0
FLAG 272 96 V1
SYMBOL ind2 128 112 R0
SYMATTR InstName L1
SYMATTR Value 1m
SYMATTR SpiceLine Rser=0
SYMATTR Type ind
SYMBOL cap 112 144 M0
SYMATTR InstName C1
SYMATTR Value 2.53303e-9
SYMBOL voltage -64 144 R0
SYMATTR InstName V1
SYMATTR Value AC 1
SYMBOL res 64 80 R90
WINDOW 0 0 56 VBottom 2
WINDOW 3 32 56 VTop 2
SYMATTR InstName Rg
SYMATTR Value 10k
SYMBOL ind2 256 112 R0
SYMATTR InstName L2
SYMATTR Value 1m
SYMATTR SpiceLine Rser=0
SYMATTR Type ind
SYMBOL cap 320 128 R0
SYMATTR InstName C2
SYMATTR Value 2.53303e-9
SYMBOL res 432 144 R0
SYMATTR InstName R1
SYMATTR Value 10k
TEXT 96 376 Left 2 !.ac lin 1000 50k 150k
TEXT -80 408 Left 2 !.measure tmp max mag(V(V1))\n.measure BW trig mag(V(V1))=tmp/sqrt(2) rise=1 targ mag(V(V1))=tmp/sqrt(2) fall=last
TEXT 176 112 Left 2 !K1 l1 l2 {K1}
TEXT 80 392 Left 2 !.step param K1 0.01 0.2 0.02
TEXT 312 392 Left 2 !.probe V(V1)
TEXT 80 64 Left 2 ;Critical coupling occurs at K1=0.062547893

--
"For a successful technology, reality must take precedence
over public relations, for nature cannot be fooled."
(Richard Feynman)

 

[John Larkin]

On Wed, 6 Jun 2012 20:48:34 -0700 (PDT), Bill Bowden
<bperryb@bowdenshobbycircuits.info> wrote:

Does LTspice assume some value of Q when simulating parallel LC
circuits where the resistance of the inductor and ESR of the capacitor
are not specified? I notice I get different results where the L or C
resistance is not stated, but the simulator works ok and just displays
weird waveforms. It seems to assume something.

Another question I have is how to write a directive to sweep a
bandpass filter from F1 to F2 to get a dB display of the response from
input to output over the frequency range?

Click Simulate/Edit Simulation Command/AC Analysis and it will create
the directive for you. You will have to declare one of your generators
as the thing to be swept; Voltage/advanced/sine, fill out the form.


There are lots of plot options.


--

John Larkin Highland Technology Inc
www.highlandtechnology.com jlarkin at highlandtechnology dot com

Precision electronic instrumentation
Picosecond-resolution Digital Delay and Pulse generators
Custom timing and laser controllers
Photonics and fiberoptic TTL data links
VME analog, thermocouple, LVDT, synchro, tachometer
Multichannel arbitrary waveform generators

 

[Fred Abse]

On Thu, 07 Jun 2012 06:07:03 -0700, Fred Abse wrote:

You need to specify a source of AC 0V.

Correction:AC 1V


<FX: removes egg from face>
--
"For a successful technology, reality must take precedence
over public relations, for nature cannot be fooled."
(Richard Feynman)

 

[Bill Bowden]

On Jun 7, 11:54 am, Fred Abse <excretatau...@invalid.invalid> wrote:

On Thu, 07 Jun 2012 06:07:03 -0700, Fred Abse wrote:
You need to specify a source of AC 0V.

Correction:AC 1V

Thanks, I got it working. I was trying to sweep a LC frequency doubler
circuit (tuned to second harmonic) and observe the bandwidth at the
output. Spice gives me a -60dB result which I guess is the attenuation
of the fundamental. I was trying to figure out how far down in
amplitude the output at FX2 would be relative to the input at various
frequencies.

-Bill

 <FX: removes egg from face
--
"For a successful technology, reality must take precedence
over public relations, for nature cannot be fooled."
                                       (Richard Feynman)