Electronic – How to simulate the impedance for this LISN circuit in LTspice


I tried to simulate the following simplistic LISN circuit:

enter image description here

Below is the AC analysis with LTspice for two nodes:

enter image description here

enter image description here

But these above plots do not tell me anything related to the purpose of LISN which is impedance balancing. The idea of LISN to raise the grid impedance to around 50 Ohm, isn't it?. How can this circuit be modified so that we can see the impedance settles/stabilizes after a certain frequency? Can someone simulate and obtain that?


I might have found the answer after I read the following:

Since the currents exiting the device under test are dependent on the
load on the ac power cord, and this load is the impedance seen by the
device looking into the ac power outlet, which varies considerably
over the measurement frequency range from outlet to outlet and from
building to building, it is not sufficient to measure the noise
currents on the power cord with a current probe. Instead, the product
under test is connected to a LISN, which stabilizes the impedance seen
by the product looking out the ac power cord.

So instead, I simulated the Z = Voltage/Current at DUT node:

enter image description here

The impedance seen approaches to 47 Ohm and I increase R2 to infinity it approaches to 50 Ohm.

enter image description here

What do you think? Is this a correct way of demonstrating it?

Best Answer

When you measure conducted perturbation, you want to know the amount of noise produced by the equipment or device under test (DUT) which flows back to the source. The source can be the mains or another ac or dc generator like a battery for instance. The idea is to isolate the noisy converter from the source via a filter so that its pollution does not perturb other systems sharing the same power source.

The amount of noise which flows back to the source depends on its impedance. Characterizing a source impedance can sometimes be a difficult exercise. If we take the mains for instance, whether you are in a residential area or in a commercial building, the mains impedance will not be the same. There are not many documents showing the impedance variations of the mains but I remember tinkering with the LM1893 many years ago and the below graph was proposed in the data-sheet, showing how the impedance may vary depending whether you measure it in residential or commercial buildings:

enter image description here

If you fix by a standard a certain level of noise your power supply is allowed to inject, you can see that if you perform the measurement in building A and then in building B in a different country, you may have a completely different signature for the same converter. To avoid this problem, the comité international spécial des perturbations radioélectriques (CISPR) - oui, it is French - has defined a specific network that you insert between the source - the mains or a dc generator - whose role is to maintain a specific and known impedance for the measurement. This way, whether you run the measurement in the US or in Taiwan, you should collect the same amount of noise with the line impedance stabilization network or LISN. The schematic diagram of a LISN used to characterize offline switching converter appears below. It is coming from an old box manufactured by Rohde and Schwarz (you need two of these, one for L and another one for N):

enter image description here

If you want to sweep its output impedance, simply install a 1-A ac source across the connections where the DUT plugs and short the input which normally goes to the ac mains via an isolation transformer. If you now plot the voltage across the current source, the impedance is that voltage divided by 1 A: the displayed voltage curve is representative of the impedance you want:

enter image description here

For those interested by the complete SPICE model of the LISN, here it is:

.subckt LISN mainsN mainsL1 measN measL1 L1 N


L4 measL1 1 100nH

R9 1 0 1k

C7 1 2 1uF

L5 2 3 1.75mH

R10 3 0 100m

C8 2 L1 1uF

L6 L1 6 50uH

R11 6 7 10m

R12 7 8 3.33

C9 8 0 8uF

C10 7 0 10n

L7 7 10 250uH

R13 10 mainsL1 10m

C11 mainsL1 0 2uF

R3 mainsL1 0 100m

C4 measN 0 10pF

L2 measN 11 100nH

R5 11 0 1k

C5 11 12 1uF

L3 12 13 1.75mH

R6 13 0 100m

C12 12 N 1uF

L8 N 16 50uH

R7 16 17 10m

R8 17 18 3.33

C13 18 0 8uF

C14 17 0 10n

L9 17 20 250uH

R14 20 mainsN 10m

C15 mainsN 0 2uF

R17 mainsN 0 100m


and once encapsulated, it is wired the following way:

enter image description here