04-20-2009 04:44 AM - edited 04-20-2009 04:47 AM
What instrument or method can be applied to impedance analysis in a circuit?
If this circuit has included some capacitors and inductors, Multimeter is not its answer, heihei!
I need get circuit's Resistance and Reactance in Multisim!
Solved! Go to Solution.
04-20-2009 11:49 AM
Hi, Fangel.
To measure impedance in a SPICE environment, I usually add a 1 A current source at the node where I want to measure the impedance. The resulting complex voltage at the node is then equal to the impedance, since V = I*Z = 1*Z = Z. Make sure you zero out any other sources in your circuit.
Hope this helps,
Ed
04-20-2009 08:24 PM
Thank EBL for your friendship.
It's very good for your method to impedance analysis.
I reinforce your method, this current source should be settled with a frequency needed, because that Capacitive reactance is Xc = 1/2πfc and Inductive reactance is X l= 2πfl , and then the voltage value of Multimeter is RMS.
However, I yet can't get circuit's relevant Resistance and Reactance in Multisim.
04-24-2009 09:44 AM
I yet can't get circuit's relevant Resistance and Reactance in Multisim.
Has anyone any ideas on my trouble?
04-27-2009 03:27 PM - edited 04-27-2009 03:33 PM
Hi, Fangel.
The best way I know of to do what you want to in Multisim is to run an AC analysis from the Simulate menu, under "Analyses -->". Set up the frequency range and number of points, etc., the way you want them and run the AC analysis. After that, run the "Postprocessor" (also on the Simulate menu) and have it plot or list the complex voltage at your node of interest. As noted before, the voltage will be equal to the impedance when your test source is a 1 A current source.
For instance, if my node is V(1), I tell it to chart "frequency", "re(V(1))", and "im(V(1))", which will produce a table of complex impedances at all of the frequencies. See the attached image.
The series resistance is the real part (re(V(1))) and the reactance is the imaginary part (im(V(1))).
Hope this helps,
Ed