• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Modelling a Mains Input Filter in LTspice?...input Z of LED current regulator?

Status
Not open for further replies.

Flyback

Well-Known Member
Hello,
Please advise on how to model our Mains Input Filter in LTspice for our LED power supply.
In our Non_switch_mode, offline LED current regulator, we have the Mains Input Filter as in the attached diagram “_Mains Input Filter”
We have done the AC sweep of it in LTspice by modelling the LED current regulator as a 10k impedance. (as in the attached LTspice schematic called “_Mains Input Filter _LTspice” We chose a high impedance because Current sources are high impedance.
Our LED current regulator works by kind of switching in different banks of LEDs as the mains rises and falls in the mains cycle.

So do you think it is reasonable to model the LED current regulator’s input impedance as a 10k resistor, as we have done in the schematic of the filter attached?
 

Attachments

MikeMl

Well-Known Member
Most Helpful Member
Likely, it is not appropriate to sweep the filter in the frequency domain. Since you are "switching", you need to characterize your filter in the time domain...
 

crutschow

Well-Known Member
Most Helpful Member
As Mike noted, you need to simulate in the time domain.
You need to simulate the complete circuit with AC input including the LED current regulator and switching.
 

Flyback

Well-Known Member
s Mike noted, you need to simulate in the time domain.
You need to simulate the complete circuit with AC input including the LED current regulator and switching.
Thanks, i have simulated it in the time domain, completely, and its fine. But we have an EMC scan which shows that we are 35dB too high at 150khz...so therefore i need to design a mains input filter which assures 35dB of attenuation at 150khz. As such i need the frequency domain scan. I have done an excel calculation to get the Magnitude vs frequency plot, but wished to check my calculations with ltspice. My plot from excel conforms to the one in ltspice, but i am not sure what impedance to use to model the input impedance of the LED current regulator?
 

MikeMl

Well-Known Member
Most Helpful Member
So why are you modelling a 50Ω source impedance? If it is a real 50Ω generator, then move the "In" node name to the right end of R1. If R1 is part of the actual circuit, then make Rs of the source 10KΩ or higher to simulate a current source.

Either use a voltage source with a big resistor in series with it, or use a current source directly.
 

Flyback

Well-Known Member
its a 50 ohm source impedance because when the regulatory people do mains conducted emissions testing they use a LISN upstream of the unit under test, and it has an impedance of 50 ohms, or at least it does from about 100khz upwards.
 

MikeMl

Well-Known Member
Most Helpful Member
its a 50 ohm source impedance because when the regulatory people do mains conducted emissions testing they use a LISN upstream of the unit under test, and it has an impedance of 50 ohms, or at least it does from about 100khz upwards.
So if your simulated source is a voltage source with a 50Ω output impedance, then make V1's Rser=50Ω. Still haven't told us if R1 is part of your actual circuit that you are testing, or it was supposed to account for the source impedance?

So what/where does a current source enter into the picture?
 

Flyback

Well-Known Member
Thanks, the current source it what the Mains Input Filter is feeding into.....the output of the current source is the LEDs.
The R1 is not part of the circuit under test, i put it there to represent the source impedance of the supply that the test house uses when they use their LISN.
 

ronsimpson

Well-Known Member
Most Helpful Member
Flyback,

1)I think the noise is from your "light bulb" so I moved the signal source to the right hand side.
2)The power line is very strange and unpredictable, For test purposes it is molded as 50 ohms. For you tests they force the power line to look like 50 ohms at the frequencies of interest.
3)To get a model of your filter you must make real world capacitor and inductors. You must model the resonant frequency! You must have the internal resistance added.
4) Right or wrong this is what I do.
upload_2017-4-17_15-41-17.png
We can talk about common mode vs differential mode noise, later.
 

Flyback

Well-Known Member
Thanks, this paper....
http://www.ti.com/lit/an/snva538/snva538.pdf
..shows the source being on the left. They also speak of the importance of knowing the input impedance of the power supply, because its impedance must be more than that of the output impednace of the filter otherwise input filter oscillations can occur as per the middlebrook criteria.
 

ronsimpson

Well-Known Member
Most Helpful Member
Thanks for the paper.
True, it does not matter which end the noise is injected into. (just hurts my head to think backwards)
Next time I will watch the input impedance of the power supply. In spice it is easy to set the noise impedance. (not as easy using a real signal generator)
Thank you
RonS
 
Status
Not open for further replies.

EE World Online Articles

Loading
Top