On Wed, 11 Jul 2018 03:51:31 -0700 (PDT), dakupoto@gmail.com wrote:

>Could some electronics guru here shed some light on this ?
>How do measure Q for say a capacitor using SPICE simulation ?
>I know how to measure reflection coefficient, insertion loss
>and SWR from a SPICE AC analysis. Any hints/pointers in
>regard to the Q measurement with SPICe simulation will be
>greatly appreciated. Thanks in advance.

No need to measure capacitor Q in Spice. You already know ESR and C,
because you control both.
But if you want to do the exercize, resonate your C with an ideal L,
do an AC sweep, and measure the center frequency and 3dB bandwidth,
and divide. Or simulate a classic voltage-booster Q-meter in time
domain.
--
John Larkin Highland Technology, Inc
lunatic fringe electronics

Reply by Tim Williams●July 11, 20182018-07-11

If it's just a C model, then:
- AC analysis
- Connect a current source, 1A, 0 deg, to the capacitor. Ground one side.
- The not-ground node has voltage V = Z*I. Read off real (resistance) +
j*imag (reactance) components directly.
- Q = reactance / resistance.
- If desired, take 1 / (2*pi*imag(VC)*frequency) to read off capacitance as
well.
This also works if the C is dependent (nonlinear), in which case you get the
small signal approximation (which is what AC analysis is). You may want to
do a parameter sweep, to measure the capacitance at other bias conditions.
This does not work if the C is equivalent over some time-varying function,
like a switched-capacitor filter, for which you need to do the transient
analysis and set up all your instruments (source, quadrature mixer,
detector..) just as you would measure the resistance and reactance IRL.
Tim
--
Seven Transistor Labs, LLC
Electrical Engineering Consultation and Contract Design
Website: https://www.seventransistorlabs.com/
<dakupoto@gmail.com> wrote in message
news:bebc685a-39f5-4eae-b320-739d031f064a@googlegroups.com...

> Could some electronics guru here shed some light on this ?
> How do measure Q for say a capacitor using SPICE simulation ?
> I know how to measure reflection coefficient, insertion loss
> and SWR from a SPICE AC analysis. Any hints/pointers in
> regard to the Q measurement with SPICe simulation will be
> greatly appreciated. Thanks in advance.

Reply by ●July 11, 20182018-07-11

Could some electronics guru here shed some light on this ?
How do measure Q for say a capacitor using SPICE simulation ?
I know how to measure reflection coefficient, insertion loss
and SWR from a SPICE AC analysis. Any hints/pointers in
regard to the Q measurement with SPICe simulation will be
greatly appreciated. Thanks in advance.