[SI-LIST] Transformer Spice Model
- From: "Thomas Beneken" <beneken@xxxxxxxxxxxx>
- To: <si-list@xxxxxxxxxxxxx>
- Date: Fri, 30 Jan 2004 10:28:11 +0100
Hi John,
this is what I took from the data sheet you provided:
Primary side open circuit inductance L14 is 1000 uH.
Stray (or Leakage) inductance Ls is about 8 uH.
Turn ratio n is 0.9:1.
Calculated:
Effective primary inductance Lp is L14 minus Ls is 992 uH.
Secondary side open circuit inductance L68 is Lp div by square of n is 1225
uH.
Coupling factor k is square root of Lp div by L68 is 0.996.
SPICE model:
L_L1 1 0 1000 uH
L_L2 2 0 1225 uH
Kn_K1 L_L1 L_L2 0.996
Simulation results for the lower frequency limit:
f/kHz a/dB
1 -11.5
10 - 0.59
100 - 0.09
Simulation results for the higher frequency limit:
f/MHz a/dB
0.3 - 0.18
1 - 1.22
2 - 3.55
Remarks/Conclusions:
DUT attenuation was simulated with a VNA model with 50 Ohm ports.
But DUT will be used in a 100 Ohms environment.
DUT bandwidth seems to be suitable for desired applivation.
By data sheet harmonic distortion is better than 85 dB.
So the linear model should do.
Regards, Thomas
-----Original Message-----
From: Thomas Beneken [mailto:beneken@xxxxxxxxxxxx]
Sent: Thursday, January 29, 2004 1:37 PM
To: 'si-list@xxxxxxxxxxxxx'
Subject: Transformer Spice Model
Hi John,
you may find this helpful for a start.
>From measurements:
L1 is the open circuit inductance of the primary coil
L2 is the open circuit inductance of the secondary coil
Ls is the stray inductance measured on primary side with secondary coil
shorted
Calculated:
Lp is effective primary inductance with Lp equals L1 minus Ls
n is primary to secondary turn ratio with n equals sqare root (Lp div by L2)
k is coupling factor with k equals square root (Lp div by L1)
M is mutual inductance with M equals square root (Lp times L2)
SPICE model for L1, L2, Ls: 45uH, 20uH, 5uH, k results in 0.943
L_L1 1 0 45u
L_L2 2 0 20u
K_K1 L_L1 L_L2 0.943 Kbreak
Tweak the equations as needed (What is in that data sheet?). You can put in
non-linearity by editing a core model (instead of Kbreak). Model parameters
are e.g. flux area, flux path length, gap, saturation factor.
Thomas
> -----Original Message-----
> From: si-list@xxxxxxxxxxxxxxx [mailto:si-list@xxxxxxxxxxxxxxx]
> Sent: Wednesday, January 28, 2004 3:46 AM
> To: si-list@xxxxxxxxxxxxxxx
> Subject: [SI-LIST] Digest Number 985
>
> Message: 1
> Date: Tue, 27 Jan 2004 11:40:58 -0600
> From: Chuong Nguyen <johnnguy@xxxxxxxxx>
> Subject: Transformer Spice Model
>
> Hi,
>
> Does any one know how to construct a transformer's spice
> model from its
> datasheet?
>
> thanks,
> jcn
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
