• LTspice tapped inductor

    From Clive Arthur@21:1/5 to All on Mon Aug 15 10:57:25 2022
    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a
    copper pipe busbar. It simulates a long, peculiar transmission line.

    I want to LTspice it. OK, lots of small inductors with some resistance
    and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and
    adjacent and being part of a single larger inductor. A tapped inductor
    is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    I know I can use an LTRA, but that doesn't simulate the discrete nature
    of the capacitance, and I really want to simulate the simulated line.

    --
    Cheers
    Clive

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Anthony William Sloman@21:1/5 to Clive Arthur on Mon Aug 15 03:43:28 2022
    On Monday, August 15, 2022 at 7:57:33 PM UTC+10, Clive Arthur wrote:
    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a
    copper pipe busbar. It simulates a long, peculiar transmission line.

    I want to LTspice it. OK, lots of small inductors with some resistance
    and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and adjacent and being part of a single larger inductor. A tapped inductor
    is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    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

    I know I can use an LTRA, but that doesn't simulate the discrete nature
    of the capacitance, and I really want to simulate the simulated line.

    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.

    --
    Bill Sloman, Sydney

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From jlarkin@highlandsniptechnology.com@21:1/5 to clive@nowaytoday.co.uk on Mon Aug 15 07:27:27 2022
    On Mon, 15 Aug 2022 10:57:25 +0100, Clive Arthur
    <clive@nowaytoday.co.uk> wrote:

    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a
    copper pipe busbar. It simulates a long, peculiar transmission line.

    I want to LTspice it. OK, lots of small inductors with some resistance
    and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and >adjacent and being part of a single larger inductor. A tapped inductor
    is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    I know I can use an LTRA, but that doesn't simulate the discrete nature
    of the capacitance, and I really want to simulate the simulated line.

    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?

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Anthony William Sloman@21:1/5 to jla...@highlandsniptechnology.com on Mon Aug 15 08:12:19 2022
    On Tuesday, August 16, 2022 at 12:27:37 AM UTC+10, jla...@highlandsniptechnology.com wrote:
    On Mon, 15 Aug 2022 10:57:25 +0100, Clive Arthur
    <cl...@nowaytoday.co.uk> wrote:

    I have an inductor wound on some 22mm plastic pipe, so essentially >air-cored. It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a >copper pipe busbar. It simulates a long, peculiar transmission line.

    I want to LTspice it. OK, lots of small inductors with some resistance
    and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and >adjacent and being part of a single larger inductor. A tapped inductor
    is surely a transformer, so how would I enumerate the coupling >coefficients, or is this something which can be ignored?

    I know I can use an LTRA, but that doesn't simulate the discrete nature
    of the capacitance, and I really want to simulate the simulated line.

    Why resistance wire?

    That might just be driven by application.

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

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

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

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

    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

    What's the application?

    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.

    --
    Bill Sloman, Sydney

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Clive Arthur@21:1/5 to Anthony William Sloman on Mon Aug 15 17:10:48 2022
    On 15/08/2022 16:12, Anthony William Sloman wrote:
    On Tuesday, August 16, 2022 at 12:27:37 AM UTC+10, jla...@highlandsniptechnology.com wrote:
    On Mon, 15 Aug 2022 10:57:25 +0100, Clive Arthur
    <cl...@nowaytoday.co.uk> wrote:

    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a
    copper pipe busbar. It simulates a long, peculiar transmission line.

    I want to LTspice it. OK, lots of small inductors with some resistance
    and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and
    adjacent and being part of a single larger inductor. A tapped inductor
    is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    I know I can use an LTRA, but that doesn't simulate the discrete nature
    of the capacitance, and I really want to simulate the simulated line.

    Why resistance wire?

    That might just be driven by application.

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

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

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

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

    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

    What's the application?

    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.

    --
    Cheers
    Clive

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From jlarkin@highlandsniptechnology.com@21:1/5 to clive@nowaytoday.co.uk on Mon Aug 15 09:23:54 2022
    On Mon, 15 Aug 2022 17:10:48 +0100, Clive Arthur
    <clive@nowaytoday.co.uk> wrote:

    On 15/08/2022 16:12, Anthony William Sloman wrote:
    On Tuesday, August 16, 2022 at 12:27:37 AM UTC+10, jla...@highlandsniptechnology.com wrote:
    On Mon, 15 Aug 2022 10:57:25 +0100, Clive Arthur
    <cl...@nowaytoday.co.uk> wrote:

    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a
    copper pipe busbar. It simulates a long, peculiar transmission line.

    I want to LTspice it. OK, lots of small inductors with some resistance >>>> and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and
    adjacent and being part of a single larger inductor. A tapped inductor >>>> is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    I know I can use an LTRA, but that doesn't simulate the discrete nature >>>> of the capacitance, and I really want to simulate the simulated line.

    Why resistance wire?

    That might just be driven by application.

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

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

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

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

    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

    What's the application?

    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.

    10r and 160 uF is a time constant of 1.6 milliseconds. L/R is around a microsecond. It's an RC network.

    Really 160 uF?


    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.

    Not with a 1.6 ms time constant.


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

    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?

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From bitrex@21:1/5 to Anthony William Sloman on Mon Aug 15 20:26:27 2022
    On 8/15/2022 6:43 AM, Anthony William Sloman wrote:
    On Monday, August 15, 2022 at 7:57:33 PM UTC+10, Clive Arthur wrote:
    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a
    copper pipe busbar. It simulates a long, peculiar transmission line.

    I want to LTspice it. OK, lots of small inductors with some resistance
    and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and
    adjacent and being part of a single larger inductor. A tapped inductor
    is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    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

    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

    I know I can use an LTRA, but that doesn't simulate the discrete nature
    of the capacitance, and I really want to simulate the simulated line.

    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.


    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From bitrex@21:1/5 to bitrex on Mon Aug 15 20:45:59 2022
    On 8/15/2022 8:26 PM, bitrex wrote:
    On 8/15/2022 6:43 AM, Anthony William Sloman wrote:
    On Monday, August 15, 2022 at 7:57:33 PM UTC+10, Clive Arthur wrote:
    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a
    copper pipe busbar. It simulates a long, peculiar transmission line.

    I want to LTspice it. OK, lots of small inductors with some resistance
    and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and
    adjacent and being part of a single larger inductor. A tapped inductor
    is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    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

    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
    0.9 it balks

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Anthony William Sloman@21:1/5 to Clive Arthur on Mon Aug 15 22:01:34 2022
    On Tuesday, August 16, 2022 at 2:11:20 AM UTC+10, Clive Arthur wrote:
    On 15/08/2022 16:12, Anthony William Sloman wrote:
    On Tuesday, August 16, 2022 at 12:27:37 AM UTC+10, jla...@highlandsniptechnology.com wrote:
    On Mon, 15 Aug 2022 10:57:25 +0100, Clive Arthur
    <cl...@nowaytoday.co.uk> wrote:

    <snip>

    What's the application?

    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.

    https://www.amazon.com/Inductance-Calculations-Dover-Electrical-Engineering/dp/0486474402

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

    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.

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

    Resistance is futile, but at least it is calculable.

    --
    Bill Sloman, Sydney

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Clive Arthur@21:1/5 to bitrex on Tue Aug 16 10:00:07 2022
    On 16/08/2022 01:45, bitrex wrote:
    On 8/15/2022 8:26 PM, bitrex wrote:
    On 8/15/2022 6:43 AM, Anthony William Sloman wrote:
    On Monday, August 15, 2022 at 7:57:33 PM UTC+10, Clive Arthur wrote:
    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a
    copper pipe busbar. It simulates a long, peculiar transmission line.

    I want to LTspice it. OK, lots of small inductors with some resistance >>>> and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and
    adjacent and being part of a single larger inductor. A tapped inductor >>>> is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    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

    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
    0.9 it balks


    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.

    --
    Cheers
    Clive

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From bitrex@21:1/5 to Clive Arthur on Tue Aug 16 11:08:39 2022
    On 8/16/2022 5:00 AM, Clive Arthur wrote:
    On 16/08/2022 01:45, bitrex wrote:
    On 8/15/2022 8:26 PM, bitrex wrote:
    On 8/15/2022 6:43 AM, Anthony William Sloman wrote:
    On Monday, August 15, 2022 at 7:57:33 PM UTC+10, Clive Arthur wrote:
    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire. >>>>> It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a >>>>> copper pipe busbar. It simulates a long, peculiar transmission line. >>>>>
    I want to LTspice it. OK, lots of small inductors with some resistance >>>>> and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and >>>>> adjacent and being part of a single larger inductor. A tapped inductor >>>>> is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    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

    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 0.9 it balks


    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Clive Arthur@21:1/5 to Anthony William Sloman on Tue Aug 16 16:41:48 2022
    On 16/08/2022 06:01, Anthony William Sloman wrote:

    <snip>

    https://www.amazon.com/Inductance-Calculations-Dover-Electrical-Engineering/dp/0486474402

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

    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.

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

    Resistance is futile, but at least it is calculable.


    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.

    --
    Cheers
    Clive

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Jeroen Belleman@21:1/5 to Clive Arthur on Tue Aug 16 17:43:51 2022
    On 2022-08-16 11:00, Clive Arthur wrote:
    On 16/08/2022 01:45, bitrex wrote:
    On 8/15/2022 8:26 PM, bitrex wrote:
    On 8/15/2022 6:43 AM, Anthony William Sloman wrote:
    On Monday, August 15, 2022 at 7:57:33 PM UTC+10, Clive Arthur wrote:
    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire. >>>>> It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a >>>>> copper pipe busbar. It simulates a long, peculiar transmission line. >>>>>
    I want to LTspice it. OK, lots of small inductors with some resistance >>>>> and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and >>>>> adjacent and being part of a single larger inductor. A tapped inductor >>>>> is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    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

    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 0.9 it balks


    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.


    Larry Benko measured coupling coefficients for a number of configurations.
    See his web page <http://www.w0qe.com/Technical_Topics/coupling_between_coils.html>.

    Jeroen Belleman

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From bitrex@21:1/5 to bitrex on Tue Aug 16 11:16:11 2022
    On 8/16/2022 11:08 AM, bitrex wrote:
    On 8/16/2022 5:00 AM, Clive Arthur wrote:
    On 16/08/2022 01:45, bitrex wrote:
    On 8/15/2022 8:26 PM, bitrex wrote:
    On 8/15/2022 6:43 AM, Anthony William Sloman wrote:
    On Monday, August 15, 2022 at 7:57:33 PM UTC+10, Clive Arthur wrote: >>>>>> I have an inductor wound on some 22mm plastic pipe, so essentially >>>>>> air-cored. It's over 120 turns, 700mm long and uses resistance wire. >>>>>> It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a >>>>>> copper pipe busbar. It simulates a long, peculiar transmission line. >>>>>>
    I want to LTspice it. OK, lots of small inductors with some
    resistance
    and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and >>>>>> adjacent and being part of a single larger inductor. A tapped
    inductor
    is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    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

    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 0.9 it balks


    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.

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Jeroen Belleman@21:1/5 to Clive Arthur on Tue Aug 16 18:16:32 2022
    On 2022-08-16 17:41, Clive Arthur wrote:
    On 16/08/2022 06:01, Anthony William Sloman wrote:

    <snip>

    https://www.amazon.com/Inductance-Calculations-Dover-Electrical-Engineering/dp/0486474402



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

    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.

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

    Resistance is futile, but at least it is calculable.


    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.


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

    Jeroen Belleman

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Clive Arthur@21:1/5 to Clive Arthur on Tue Aug 16 17:35:39 2022
    On 15/08/2022 10:57, Clive Arthur wrote:
    I have an inductor wound on some 22mm plastic pipe, so essentially air-cored.  It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a
    copper pipe busbar.  It simulates a long, peculiar transmission line.

    I want to LTspice it.  OK, lots of small inductors with some resistance
    and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and adjacent and being part of a single larger inductor.  A tapped inductor
    is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    I know I can use an LTRA, but that doesn't simulate the discrete nature
    of the capacitance, and I really want to simulate the simulated line.


    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.

    --
    Cheers
    Clive

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From legg@21:1/5 to clive@nowaytoday.co.uk on Wed Aug 17 11:24:39 2022
    On Tue, 16 Aug 2022 17:35:39 +0100, Clive Arthur
    <clive@nowaytoday.co.uk> wrote:

    On 15/08/2022 10:57, Clive Arthur wrote:
    I have an inductor wound on some 22mm plastic pipe, so essentially
    air-cored. It's over 120 turns, 700mm long and uses resistance wire.
    It's about 12uH.

    There are 30 capacitors connected evenly along the coil commoned to a
    copper pipe busbar. It simulates a long, peculiar transmission line.

    I want to LTspice it. OK, lots of small inductors with some resistance
    and the capacitors.

    But these small inductors are coupled by virtue of being co-axial and
    adjacent and being part of a single larger inductor. A tapped inductor
    is surely a transformer, so how would I enumerate the coupling
    coefficients, or is this something which can be ignored?

    I know I can use an LTRA, but that doesn't simulate the discrete nature
    of the capacitance, and I really want to simulate the simulated line.


    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Clive Arthur@21:1/5 to legg on Wed Aug 17 16:29:10 2022
    On 17/08/2022 16:24, legg wrote:
    On Tue, 16 Aug 2022 17:35:39 +0100, Clive Arthur

    <snipped>


    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

    https://m0ukd.com/calculators/air-cored-inductor-calculator/

    As I said, it seemed to give the right result when I measured the
    original coil, and thinking about it, these radio amateur guys have been
    doing this sort of thing for a good while.

    --
    Cheers
    Clive

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)
  • From Chris Jones@21:1/5 to Clive Arthur on Sun Aug 21 21:33:58 2022
    On 18/08/2022 1:29 am, Clive Arthur wrote:
    On 17/08/2022 16:24, legg wrote:
    On Tue, 16 Aug 2022 17:35:39 +0100, Clive Arthur

    <snipped>


    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

    https://m0ukd.com/calculators/air-cored-inductor-calculator/

    As I said, it seemed to give the right result when I measured the
    original coil, and thinking about it, these radio amateur guys have been doing this sort of thing for a good while.



    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

    --- SoupGate-Win32 v1.05
    * Origin: fsxNet Usenet Gateway (21:1/5)