1. Home
  2. Electronics Design
  3. Inductor saturation in LTspice

Inductor saturation in LTspice

I have been doing simulations of various switching power supplies in LTSpice, and it seems like the inductors never show any saturation behavior. I have even tried, for example, a stock 10 uH 10 amp inductor from their database, and applied 10 VDC. The dI/dt stays just about constant at 0.9 A/uSec up to at least 80 amps, and it only flattens out at about 2 mSec at about 438 amps, due to the 0.0226 ohms series resistance.

The documentation shows a way to simulate saturation and hysteresis with the following:

  • L1 N001 0 Hc=16. Bs=.44 Br=.10 A=0.0000251
  • Lm=0.0198 Lg=0.0006858 N=1000 I1 0 N001 PWL(0 0 1 1) .tran .5 .options maxstep=10u .end

I am not sure how to enter this information into an inductor model or a schematic. The standard models do not seem to allow parameters to be entered. I'll look into how I might be able to insert a new symbol that can use these parameters and provide a more accurate inductor model, but if anyone has already done this I'd appreciate some help.

It surprises me that LTspice does not include even a rudimentary modeling of real world inductor saturation, given that SwitcherCad essentially revolves around the use of inductors in almost every switching supply model. Most inductors specify inductance values at minimum current and maximum current, and then the inductance essentially drops to zero at saturation current. It seems that it would be simple enough to add this function to the inductor equation, and then simulations would be much more realistic.

Paul

Reply to
Paul E. Schoen
Loading thread data ...

OK, I found the -Right Click to access the inductor parameters, and it seems to work. I played with the value of N in the above parameters and found that N=14 gives about a correct value for dI/dt up to about 15 amps, after which it rises at a much greater slope.

The LTSpice ASCII file for my test jig follows. Any suggestions on even better modeling will be appreciated. I am weak in magnetics theory. Thanks.

Paul

=========================================================================

Version 4 SHEET 1 952 260 WIRE -400 64 -576 64 WIRE -576 96 -576 64 WIRE -400 96 -400 64 WIRE -576 208 -576 176 WIRE -400 208 -400 176 WIRE -400 208 -576 208 FLAG -576 208 0 SYMBOL voltage -576 80 R0 WINDOW 123 0 0 Left 0 WINDOW 39 0 0 Left 0 SYMATTR InstName V1 SYMATTR Value 10 SYMBOL ind -416 80 R0 WINDOW 40 36 108 Left 0 SYMATTR InstName L1 SYMATTR Value 10µ SYMATTR SpiceLine Ipk=10 Rser=0.0226 Rpar=942 Cpar=0 SYMATTR SpiceLine2 Hc=16. Bs=.44 Br=.10 A=0.0000251 Lm=0.0198 Lg=0.0006858 N=14 TEXT -610 232 Left 0 !.tran 1m startup

Reply to
Paul E. Schoen

"Paul E. Schoen" schrieb im Newsbeitrag news:480a70a8$0$19817$ snipped-for-privacy@news.coretel.net...

Hello Paul, If you only need saturation but no hysteresis, then there is a much simpler way.

Just replace the value 10u with the formula below. (Watch the 12.5 = 1/0.08, x is the coil current)

flux=10u*12.5*tanh(x*0.08)

Best regards, Hlmut

Reply to
Helmut Sennewald

Mike Engelhardt put together an interesting range of saturable magnetic structures that were dependant on varying parameters.

You should be able to find 'non_linear_inductor.asc' (~16K), and others, in the yahoo group SWCAD files page. Go to 'all_files.htm' and text search for the file name.

RL

Reply to
legg

I think you can see nonlinear effects more easily if you define a source impedance and give your inductor some turns. See attached.

RL

Version 4 SHEET 1 952 260 WIRE -400 64 -576 64 WIRE -576 96 -576 64 WIRE -400 96 -400 64 WIRE -576 208 -576 176 WIRE -400 208 -400 176 WIRE -400 208 -576 208 FLAG -576 208 0 SYMBOL voltage -576 80 R0 WINDOW 123 0 0 Left 0 WINDOW 39 0 0 Left 0 SYMATTR InstName V1 SYMATTR Value 10 SYMBOL ind -416 80 R0 WINDOW 40 36 108 Left 0 SYMATTR InstName L1 SYMATTR Value 10µ SYMATTR SpiceLine Ipk=10 Rser=0.0226 Rpar=942 Cpar=0 SYMATTR SpiceLine2 Hc=16. Bs=.44 Br=.10 A=0.0000251 Lm=0.0198 Lg=0.0006858 N=14 TEXT -610 232 Left 0 !.tran 1m startup

Reply to
legg

The Lg and N need to be in the Spiceline as I changed it above. It also worked well using the flux idea suggested by Helmut. Thanks all!

Paul

Reply to
Paul E. Schoen

This worked very well, and it is simpler. Now, for a coil that saturates at

5 amps, do I use:

flux=10u*5*tanh(x*(1/5))

or more generally:

flux = L * Isat * tanh(x/Isat)

That seems to work, although I'm not sure just how. I suppose one must understand how the term flux is used in the model.

Thanks!

Paul

Reply to
Paul E. Schoen

In the late '80's I was using (in PSpice)...

L = Lo/(1 + (I/IH)^2)

where I is the current in the inductor and IH is the current where the inductance falls to half of its no-current value.

...Jim Thompson

--
|  James E.Thompson, P.E.                           |    mens     |
|  Analog Innovations, Inc.                         |     et      |
|  Analog/Mixed-Signal ASIC\'s and Discrete Systems  |    manus    |
|  Phoenix, Arizona            Voice:(480)460-2350  |             |
|  E-mail Address at Website     Fax:(480)460-2142  |  Brass Rat  |
|       http://www.analog-innovations.com           |    1962     |
             
         America: Land of the Free, Because of the Brave
Reply to
Jim Thompson

I think that's useful only if the part itself is carved in stone.

Determining IH every time a turn is added, or shim altered to vary a gap is mental-labour intensive.

For a specific core shape and material, there is an interesting boundary showing up in the Hanna curves that might be useful to characterize in a brick wall saturation model, if those two features are unchanging.

RL

Reply to
legg

[snip]

Military/space application. Part _was_ "carved in stone", and that particular expression matched measurements quite closely.

IH was around 88 Amps BTW ;-)

...Jim Thompson

--
|  James E.Thompson, P.E.                           |    mens     |
|  Analog Innovations, Inc.                         |     et      |
|  Analog/Mixed-Signal ASIC\'s and Discrete Systems  |    manus    |
|  Phoenix, Arizona            Voice:(480)460-2350  |             |
|  E-mail Address at Website     Fax:(480)460-2142  |  Brass Rat  |
|       http://www.analog-innovations.com           |    1962     |
             
         America: Land of the Free, Because of the Brave
Reply to
Jim Thompson

"Jim Thompson" schrieb im Newsbeitrag news: snipped-for-privacy@4ax.com...

Hello Jim,

The equivalent inductance definition in LTspice would be

flux= Lo*IH*atan(x/IH)

My recommended function with tanh() has a steeper descent of the inductance versus current.

flux= Lo*IH*tanh(x/IH)

Best regards, Helmut

Reply to
Helmut Sennewald

[snip]

I use TANH quite often now in behavioral modeling...

(1) It's closely equivalent to the transition width of a diff-pair.

(2) It's convergence stable.

...Jim Thompson

--
|  James E.Thompson, P.E.                           |    mens     |
|  Analog Innovations, Inc.                         |     et      |
|  Analog/Mixed-Signal ASIC\'s and Discrete Systems  |    manus    |
|  Phoenix, Arizona            Voice:(480)460-2350  |             |
|  E-mail Address at Website     Fax:(480)460-2142  |  Brass Rat  |
|       http://www.analog-innovations.com           |    1962     |
             
         America: Land of the Free, Because of the Brave
Reply to
Jim Thompson

He may have, but that would not be the file you refer to below. :)

I created and posted a file of this name to the LTspice group about four years ago. But the one you are probably thinking of is named "saturating_inductor.asc". It contains twelve examples of inductor modeling approaches. Four are based on LTspice's unique flux=f(x) method, three are based on a method using standard b-sources, three use a generalized impedance converter to create an equivalent magnetic circuit (which can then have a "Bm" limit), and one uses current controlled switches.

The examples model saturation with "hardness" varying in degrees from no saturation, soft (continuous) up through abrupt (stepped).

LTspice Yahoo group members can download the file here:

formatting link

Group membership requires registration but is free of charge.

Regards -- analog

Reply to
analog

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.