LTspice tapped inductor

K L1 L2 ... Ln 0.2

lets you set up a single coupling coefficient (here 0.2) for a collection of inductors. Obviously more remote winding are less closely coupled.

I don't suppose that there's anything stop you doing a series of coupled inductors, say

K1 L1 L2 0.2 K2 L2 L3 0.2 K3 L3 L4 0.2

which wouldn't be entirely right either

My guess would be that the discrete nature of the capacitors won't make a lot of difference for frequencies where the wavelength is longer than a couple of sections.

Why resistance wire? With enough resistance (namely many ns tau per stage) it becomes a string of RCs, about as ugly a txline as possible.

What's total r ? How big are the caps?

Have you built one? What's the step response like?

What's the application?

That might just be driven by application.

He hasn't specified the resistance, or the capacitances, so the nature of the transmission line is obscure.

He says he has got one - maybe he built it. Clearly, measuring the actual step response is difficult for some reason or other so he wants to simulate it

Always a good question. Clive Arthur has posted here often enough that he should have known that he'd get asked it. He's not clueless newbie.

Trouble is, as ever, NDAs. I have built a simulator (maybe emulator is a better word) as described. The R is representative of the real R, as is the C - totalling 10R and 160uF, The L (12uH) is guestimated from a reasonable assumption of propagation velocity and length. Yes, it's very low impedance. It was quite a juggling act to get all the parameters about right.

It's simply not possible at this stage to test with the Real Thing, so my emulator will have to do, but I'd also like to Spice the emulator to speed up a few things. The Real Thing cannot be changed.

So the question is, how to Spice it? Is the mutual inductance between sections of a long air-cored inductor at all significant? Top signal frequency 100kHz.

This sort of thing is a weakness of mine, though less so than it was, which is why I ask.

Really 160 uF?

Not with a 1.6 ms time constant.

You could build a short section and measure it. Fiddle with Spice to match the measurement. Then you can add sections in Spice.

Is this a high voltage delay line?

Unfortunately LTSpice balks at doing the second and considers that a "non-physical winding possibility" and wants you to just do it the first way

Huh, that's weird. Actually it seems to only complain about non-physical winding for certain values of coupling coefficient when you set it up that way, if you set it like 0.2 it seems ok but if you try to do say

Chapter 16 - single layer coils on cylindrical winding forms - seems to be what you want. It goes from page 142 to page 162. I could scan them and e-mail you the images. Making sense of the content isn't easy.

Resistance is futile, but at least it is calculable.

I wonder if that's because, say, L8 has 0.9 coupling to L7 which has 0.9 to L6 etc, so L8 has 0.9 to L7 plus 0.9 x 0.9 to L6 (etc) which is >1 ? In which case, 0.5 would be the absolute max for a large number of inductors?

So I tried it (LTspice) with 5 inductors and 4 couplings, all equal. K = 0.58 fails, K = 0.57 works, and that's what passes for solid proof round these parts. I think "Clive's Constant" has a certain ring to it.

That could be a clue, but like I said, not really my area.

Ya I thought the same thing at first but also found the > 1 hypothesis wasn't the reason.

"Clive's Constant" works for me! 0.57 is probably large enough to accommodate adjacent tapped windings on an air coil

Er excuse me, I misunderstood your post at first. I had originally thought they had to straight sum to 1 but you've done the math correctly here, and 0.5 is the max in the _limit_ of infinite taps.

Thanks, Bill.

I think with your original suggestion of multiple two-part K factors using a common parameterised K coupled with Bitrex's observation about how these interact and John's pushing for more information I stand a good chance of getting somewhere. With luck, I should be able to adjust K to make the LTspice response look like my emulator.

If it works it'll save a lot of time. However, if it eventually turns out that the Real Thing is substantially different from the emulator, well, back to the drawing board.

And John, yes it is a delay line, though that's not its purpose. However, I do need to replicate the delay.

Larry Benko measured coupling coefficients for a number of configurations. See his web page

should let you work it out . I've even got a copy.

It's a pulse forming network? Radar? Lasers? Electrical weaponry?

Jeroen Belleman

Pragmatic approach...

Originally I used a web based air-cored coil calculator to design my coil, and it measured pretty close IIRC.

Just now, I used the same calculator to see what inductance half of my coil would be, that is, half the length and half the number of turns. It turns out that half the coil is only a couple of percent under half the inductance of the full coil, in other words, bugger all coupling.

(Of course, with perfect coupling, twice the turns would give 4 x the inductance.)

So assuming the calculator is right, I probably don't need to bother with coupling for my LTspice model, discrete inductors will do. That saves a lot of typing, or copying and editing.

Link?

RL

If you have the patience to create a 3d model of the inductors, you can simulate the coupling coefficients using FastHenry. It is open source. There is a model viewer and updated versions of fasthenry at fastfieldsolvers.com