|
Hi
folks. I just uploaded a file “Simple toroid transformer return loss
model.asc”. My problem is this: I am trying to model a ferrite-based toroid
transformer which has frequency dependent inductance and resistance values based
on its complex permeability curves which are a function of frequency. My
uploaded file shows the equivalent resistive and inductive component of the
primary as a function of frequency in the text shown at the upper right from 3.5
to 28 MHz. . I would like to simulate interpolated resistance values and
inductance values of the primary so I can have a single return loss curve as a
function of frequency as the toroid’s primary resistance and inductance values
change. I realize I can simulate interpolated parameter values in tables,
and I believe I can use a BI source with a frequency dependent equation plus use
of parameters, but I have not succeeded in getting this all together. I
did see a model of a frequency dependent resistor in the files. I can use
some assistance with my simulation on how to incorporate the frequency dependent
inductance and resistance values. Thanks for your help.
-Steve
(amateur radio call sign K1RF)
|
Hello Steve,
You could use a G-source with a Laplace-functions.
Place a G-source. Connect inputs and outputs together and replace it's value with a formula as below.
Laplace=1/(s*L+0.5)
This behaves like an inductor with inductance L and a series resistance of 0,5Ohm. "s" will be replaced with jw in the .AC simulation.
You could also change to make it frequency dependent.
Laplace=1/(L*s/(1+abs(s)*1u) +0.5)
Best regards, Helmut
|
Thank you Helmut. I will proceed with your recommendation.
-Steve
переключити цитоване повідомлення
Показати цитований текст
Sent: Wednesday, October 03, 2018 7:52 PM
Subject: [LTspice] Re: Modeling frequency dependent inductance and
resistance of a toroid primary
Hello Steve,
You could use a G-source with a Laplace-functions.
Place a G-source. Connect inputs and outputs together and replace it's
value with a formula as below.
Laplace=1/(s*L+0.5)
This behaves like an inductor with inductance L and a series resistance of
0,5Ohm.
"s" will be replaced with jw in the .AC simulation.
You could also change to make it frequency dependent.
Laplace=1/(L*s/(1+abs(s)*1u) +0.5)
Best regards,
Helmut
|
Hello Steve,
There is an example with skin effect using Laplace.
LAPLACE = 1/({RDC}*(1+ sqrt(s/.7e6)))
Skin_Laplace.zip
Best regards, Helmut
PS: You can search in this file all_files.htm for examples with "Laplace", "inductance" or "inductor".
all_files.htm
|
Hello Steve. Check out my inductance approximation option. See LRtest.zip in TEMP folder. Bordodynov.
04.10.2018, 08:57, "helmutsennewald@... [LTspice]" <ltspice@...>:
Hello Steve,
There is an example with skin effect using Laplace.
LAPLACE = 1/({RDC}*(1+ sqrt(s/.7e6)))
Skin_Laplace.zip
Best regards, Helmut
PS: You can search in this file all_files.htm for examples with "Laplace", "inductance" or "inductor".
all_files.htm
|
Thank you Alex. Got it. Wow you did a lot of work on this. I
need to study it to fully understand what you did. Thank you kindly.
-Steve
переключити цитоване повідомлення
Показати цитований текст
Sent: Thursday, October 04, 2018 2:29 AM
Subject: Re: [LTspice] Re: Modeling frequency dependent inductance
and resistance of a toroid primary
Hello
Steve.
Check
out my inductance approximation option.
See LRtest.zip in TEMP
folder.
Bordodynov.
04.10.2018, 08:57, "helmutsennewald@... [LTspice]"
:
Hello Steve,
There is an example with skin effect using Laplace.
LAPLACE = 1/({RDC}*(1+ sqrt(s/.7e6)))
Skin_Laplace.zip
Best regards,
Helmut
PS: You can search in this file all_files.htm for examples with
"Laplace", "inductance" or "inductor".
all_files.htm
|
|
|
On Tue, Oct 19, 2021 at 06:14 AM, Brian Machesney wrote: It simulates readily and represents a ferrite-loaded inductor
pretty closely. Coupling the inductors completes the transformer. When inductors are coupled, the current in the windings is changed (that is the point). The losses in the wire (and definitely in the core) will not be correct anymore. It won't matter much at low frequencies, however, EMI/EMC simulations might be in error. This paper uses LTspice and looks useful: K. Nomura, N. Kikuchi, Y. Watanabe, S. Inoue and Y. Hattori, "Novel SPICE model for common mode choke including complex permeability," 2016 IEEE Applied Power Electronics Conference and Exposition (APEC), 2016, pp. 3146-3152 -marcel
|
Hello everyone,
I am trying to simulate the common mode choke (CMC) impedance presented in Nomura's 2016 paper for Hitachi F1AH0972.
The paper is titled "Novel SPICE Model for Common Mode Choke Including Complex Permeability".
The results I get upon running the file are very different from what is shown in the paper.
Has anyone looked into this? I would appreciate your help.
I am uploading "Nomura_model_F1AH0972" in the Files/Temp folder.
Sincerely,
Nitish Agrawal
|
Well, 'very different' is not much help in
diagnosing the issue. You are looking at the input voltage
divided by the input current, with the other end of the CMC
shorted to ground? In this case, it might be good to upload a
picture of your result and a picture of the result in the paper,
to Files >= Photos and then tell us you did that.
On 2024-11-19 16:54, Nitish Agrawal via
groups.io wrote:
Hello everyone,
I am trying to simulate the common mode choke (CMC)
impedance presented in Nomura's 2016 paper for Hitachi
F1AH0972.
The paper is titled "Novel SPICE Model for Common Mode
Choke Including Complex Permeability".
The results I get upon running the file are very different
from what is shown in the paper.
Has anyone looked into this? I would appreciate your help.
I am uploading "Nomura_model_F1AH0972" in the Files/Temp
folder.
Sincerely,
Nitish Agrawal
--
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying
|
Hi John,
Thank you for looking into this.
I have uploaded two image files "Z_presented_in_Nomura_paper_Fig15.png" and "Z_simulated_LTSpice.png".
The first one shows the result as presented in Nomura's paper.
The second one shows the impedance plotted as -V(1)/I(V1) and inductance plotted as Im(-V(1)/I(V1))/(2*pi*frequency).
The simulated impedance has a resonance at 13kHz while Nomura's paper doesn't show that. The impedance values simulated and phase values do not match anywhere and it is not a scaling issue. The impedance simulated is higher by a factor of 10^4 but not in a scalar fashion.
Sincerely,
Nitish Agrawal
|
Your photos are not in the 'Nomura' album. It
shows its contents as '0 files'.
On 2024-11-19 18:34, Nitish Agrawal via
groups.io wrote:
Hi John,
Thank you for looking into this.
I have uploaded two image files
"Z_presented_in_Nomura_paper_Fig15.png" and
"Z_simulated_LTSpice.png".
The first one shows the result as presented in Nomura's paper.
The second one shows the impedance plotted as -V(1)/I(V1) and
inductance plotted as Im(-V(1)/I(V1))/(2*pi*frequency).
The simulated impedance has a resonance at 13kHz while
Nomura's paper doesn't show that. The impedance values
simulated and phase values do not match anywhere and it is not
a scaling issue. The impedance simulated is higher by a
factor of 10^4 but not in a scalar fashion.
Sincerely,
Nitish Agrawal
--
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying
|
Hi John,
The album name is "Nomura CMC model". I see two photos in there. I am not sure why they are not showing up on your end.
Sincerely,
Nitish Agrawal
|
.func does not do what you want.
.FUNC -- User Defined Functions
All parameter substitution evaluation is done before the simulation begins.
|
They are indeed there now, but are too
difficult to read, especially the LTspice result. I suggest you
set the background colour for 'waveform pane' photos to white,
and zoom in on the graph in the Nomura paper.
I see the resonance when I run your .ASC.
On 2024-11-19 18:47, Nitish Agrawal via
groups.io wrote:
Hi John,
The album name is "Nomura CMC model". I see two photos in
there. I am not sure why they are not showing up on your end.
Sincerely,
Nitish Agrawal
--
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying
|
Hi John,
I just uploaded the zoomed in image of Nomura's result and LTSpice impedance simulation on white background (-V(1)/I(V1)).
Sincerely,
Nitish Agrawal
|
Thank you. I suppose you have seen the message
about not being able to use .FUNC in the way you have.
On 2024-11-19 19:39, Nitish Agrawal via
groups.io wrote:
Hi John,
I just uploaded the zoomed in image of Nomura's result and
LTSpice impedance simulation on white background (-V(1)/I(V1)).
Sincerely,
Nitish Agrawal
--
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying
|
Hello Roy and John,
Thank you both for your comments. I was trying to understand Nomura's methodology by simulating it. Your message suggests that his implementation is incorrect.
Is that true? He does show close match to measured values in his paper. Just wondering where the disconnect is.
Regards,
Nitish Agrawal
|
I'm not sure, but I think you can't use .FUNC
with Laplace, because s is a variable. Does Nomura claim to have
used Spice simulation? I do not know whether his implementation
is correct. Does his graph have enough resolution to show the
narrow resonance? Do his measured values show it or any sign of
it?
On 2024-11-19 20:41, Nitish Agrawal via
groups.io wrote:
Hello Roy and John,
Thank you both for your comments. I was trying to understand
Nomura's methodology by simulating it. Your message suggests
that his implementation is incorrect.
Is that true? He does show close match to measured values in
his paper. Just wondering where the disconnect is.
Regards,
Nitish Agrawal
--
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying
|
Hi John,
Nomura specifically claims to have used LTSpice. His graph has no signs of resonance in the 12kHz region that the LTSpice sim shows.
Regards,
Nitish
|
John Woodgate
Roy McCammon