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
LTspice tapped inductor
Started by ●August 15, 2022
Reply by ●August 16, 20222022-08-16
Reply by ●August 16, 20222022-08-16
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.
Reply by ●August 16, 20222022-08-16
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
Reply by ●August 16, 20222022-08-16
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
Reply by ●August 16, 20222022-08-16
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
Reply by ●August 16, 20222022-08-16
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
Reply by ●August 17, 20222022-08-17
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
Reply by ●August 17, 20222022-08-17
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? > > RLhttps://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
Reply by ●August 21, 20222022-08-21
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
