# simulating line filter

#### harinikrishna

Joined Apr 3, 2020
18
Hi,
good day..!
I am trying to simulate a line filter on LT spice based on the calculations made from the document

trying to meet the standards IEC/EN61000-6-3. . how do i design a common mode choke on LT spice to see the filter behavior on LT spice?

AC line filter
input : 240- 388V AC
frequency : 50Hz
used to feed a smps with switching frequency 200Khz

Thank-you
Warm regards
Harini krishna

Last edited:

#### harinikrishna

Joined Apr 3, 2020
18
Further to post no #9

Specifications are given.
Could anyone explain me a bit about -
1. How to calculate corner frequency for CM and DM noise if CISPR 22 say frequency range is 150 KHz to 30 MHz for CE and is that the same filter used for RE.
2. How to calculate Lcm(common mode) and Ldm(differential mode) choke
3. How to calculate X and Y capacitor.

Thanks !!!
Hi @mishra87
I am also looking to design an AC line filter for SMPS.
I found this application note to be helpful
even i am a bit curious to know how the calculate the the specifications as mentioned in the post
how did make progress in designing an emi filter?
Thank-you

Last edited by a moderator:

#### ronsimpson

Joined Oct 7, 2019
910
L9, L10 To be more accurate, see below. I do not use Rfe but Rcu and Cwi are important. Also in LT spice to make it a transformer you need to use ".K L9 L10 .98"

Probably should add Cwi and Rcu for L7,8.

Next the capacitors are also not perfect but have a resonant frequency. So add in resistance and inductance for them.

When testing in the lab V12,13 have a 50 ohm impedance. I know the power line has a complex impedance but they are not tested on the power line in the data sheet.

#### harinikrishna

Joined Apr 3, 2020
18
L9, L10 To be more accurate, see below. I do not use Rfe but Rcu and Cwi are important. Also in LT spice to make it a transformer you need to use ".K L9 L10 .98"
View attachment 216735
Probably should add Cwi and Rcu for L7,8.

Next the capacitors are also not perfect but have a resonant frequency. So add in resistance and inductance for them.

When testing in the lab V12,13 have a 50 ohm impedance. I know the power line has a complex impedance but they are not tested on the power line in the data sheet.

for capacitors and individual inductors ( l7 and l8) i chose manufacturer parts which are available on lt spice. should i still add the Cwi and Rcu for inductors capacitor inductor and resistance?
i have seen on many documents that the leakage inductance of common mode inductance can be used as the differential mode filter. so in the simulations do i need to add a differential mode inductance seperately?

#### ronsimpson

Joined Oct 7, 2019
910
Transformer leakage inductance can be set by ".k" or can be done with .K =1 and add two non coupled industrials.

If you can get spice files for the parts that's good. If not you can get close by adding in parts to make the L & C non ideal.

#### ronsimpson

Joined Oct 7, 2019
910
I took a capacitor from one of my projects and put it on a Vector Network Analyzer. Scan frequency 100khz to 100mhz. Source is 50 ohms impedance. The capacitor has a resonant frequency of 47mhz in the center of the picture. Above 47mhz it turns inductive. In spice I used the capacitor value, a inductor value that makes 47mhz and a resistor that will give 52db attenuation. The data sheet, the VNA, and LT SPICE all came up the similar pictures. (not actually)

I did not study the 315mhz resonant point. Another one at 670mhz and 1.032ghz. Some of that maybe my equipment.

#### harinikrishna

Joined Apr 3, 2020
18
Hi,
Hope you are doing good.
after running the LT spice simulations applying common mode noise at 5Mhz and differential mode noise at 500kHz, and found the results to be ( green graph : without emi
filter blue graph : with emi filter)
i am trying to achieve the limits for class B ( limits table in figure) and at 500kHz i am reading 58.8dbuV
how do i further tune the filter to achieve the limits, is it a trial and error method or i need to design the filter again?

In the limit table mentioned in the image,
the notes say " the lower limit shall apply at transition frequencies". I am a bit confused about what transition frequencies and lower limits on the notes. can you please help me with this?
Thank-you
Warm regards
harini Krishna

Last edited:

#### Marc Sugrue

Joined Jan 19, 2018
149
dbuV is
i have seen most of the measurements in dbuV.
but on LT spice when i do fft analysis, i see only db as units.
View attachment 216890\

How do i measure the y axis in dbuv so that i can see if my filter is meeting the limits.
What should be the amplitude of CM and DM ( common mode noise and differential mode noise)?
thank-you
Warm Regards
Harini Krishna
I would have thought that in LT Spice the db of whatever your measuring, so if your measuring V then your measuring dbV. If your measuring Current is dbA.

https://www.ahsystems.com/EMC-formulas-equations/typical-conversion-formulas.pdf

On a side note, Common Mode noise is quite often High Frequency in the region of Mhz as opposed to kHz. Are you sure your issue is not differential noise? A Common Mode flter will have fairly low differential impedance at 200kHz so would need fairly large Capacitors after it to be effective at 200kHz and a low SRF which would make it less effective at high frequency.

#### harinikrishna

Joined Apr 3, 2020
18
Hi,
Hope you are doing good.
after running the LT spice simulations applying common mode noise at 5Mhz and differential mode noise at 500kHz, and found the results to be ( green graph : without emi
filter blue graph : with emi filter)
i am trying to achieve the limits for class B ( limits table in figure) and at 500kHz i am reading 58.8dbuV
how do i further tune the filter to achieve the limits, is it a trial and error method or i need to design the filter again?

In the limit table mentioned in the image,
the notes say " the lower limit shall apply at transition frequencies". I am a bit confused about what transition frequencies and lower limits on the notes. can you please help me with this?
Thank-you
Warm regards
harini Krishna

#### Marc Sugrue

Joined Jan 19, 2018
149
Hi,
Hope you are doing good.
after running the LT spice simulations applying common mode noise at 5Mhz and differential mode noise at 500kHz, and found the results to be ( green graph : without emi
filter blue graph : with emi filter)
i am trying to achieve the limits for class B ( limits table in figure) and at 500kHz i am reading 58.8dbuV
how do i further tune the filter to achieve the limits, is it a trial and error method or i need to design the filter again?

In the limit table mentioned in the image,
the notes say " the lower limit shall apply at transition frequencies". I am a bit confused about what transition frequencies and lower limits on the notes. can you please help me with this?
Thank-you
Warm regards
harini Krishna
If your issue is truely common mode then you can lower the frequency of the 3db point of the filter to give more attenuation at the problem frequency, this will involve larger L's and C's with lower SRF so it will become less effective at higher frequencies but will provide you with more attenuation at lower frequencies. Alternatively you could add stages to create an higher order filter with smaller but more parts. This will give better HF performance due to better SRF of smalller parts.

Is this a real problem as opposed to a simulation?

Really it all depends on your load, high power and large inductance can become large in size and difficult to source - even for CM Mode chokes.

I'm not an expert on the actual specification but I assume Transitions to be at the point where the range changes but you have the potential to interpret 2 limits as they are between 2 ranges ( So for example 5Mhz could be interpreted as Quasi Peak 56db or 60dbuV without the note but the note states you must use the lower limit of 56dbuV @ 5Mhz.

Last edited:

#### ronsimpson

Joined Oct 7, 2019
910
good day..!
This project is very dependent on board layout, which is not in SPICE. It is dependent in primary to secondary capacitance in a power supply which is not in SPICE.

I do the best guess I can and them get the project tested. I need to know what frequencies and what type if noise. Next I go around looking for that noise source. Some times I find a diode that is ringing on a secondary. Or the drive of a MOSFET is too fast. Or change the snubber. There are many places to go looking for noise.

And I look at the SPICE of the filter. If I need -5db at 100mhz and 200mhz and the noise is common mode then I can change the filter. Or differential noise is a different change.