I am new to KiCad ngspice. Everything I’ve tried has failed. Documentation is of no help as it does not address KiCAD 9. General posts on the intertnet are confusing as they address a much more experienced user than I, or the post is out-of-date referencing much older versions of KiCAD.
Issue 1. I am trying to make a symbol for a trifilar-wound ferrite core inductor to use in a simulation for a bandpass filter.
This is the circuit I am trying to create as a new symbol.
Issue 2: I cannot find a netlist editor or instructions on how to use it
Issue 3: Simulating the bandpass filter circuit using discrete components results on errors causing the simulation to fail. “run simulation not started Error: vector frequency not found!”
What you’re showing is not a trifilar coil. It’s three inductors in series. What is your idea of a trifilar coil? Please elaborate, then we might find the right symbol for you.
I could not find a symbol representing a trifilar wound ferrite inductor.
Trifilar wound inductor is three lengths of wire, laid in parallel, and wound around the toroid core.
This is how a trifilar inductor is usually shown in schematics. Is there a way to indicate phasing, such as a dot?
The total inductance is 3.96uH.
Thanks,
Roger, N1XP
At least in LTSpice, a coupled inductor (or transformer) is specified with inductance and coupling coefficient this way. The coupling of the windings is specified with that K statement and does not depend upon the placement of the coils in the drawing:
I understand you show a symbol for a transformer. I am trying to model a mutually-coupled toroid inductor with three physically parallel windings, electrically connected in series, not a transformer. This was the reason for showing three ferrite inductors in series on the simulation schematic. Physically and magnetically the performance is totally different from a transformer, especially at high frequency i.e., 7MHz.
The circuit using this, trifilar wound, toroid inductor is a Chebyshev derived band pass filter. The circuit was built, tested with a Vector Network Analyzer (VNA) and found to be within expected calculated performance specifications. The KiCAD ngspice modeled circuit is totally erroneous. Why?
Both of the two diagrams you have presented so far don’t show any coupling. You have to tell ngspice that the inductors are coupled. So place the following in a text box onto the Eeschema canvas: K1 L9 L10 L11 0.62
with 0.62 being the coupling constant (taken from your first schematic, but to be chosen by you).
To see if the inductor orientation is o.k., switch on the pin numbering (Show Pin Numbers) in the ‘Symbol Properties’ window. All pins 1 on top is like all dot marks on top.
If coupling and symbol orientation are o.k., but the simulation still shows a strong deviation from measurement, please post the project here as a zip file, so we can have a look.
Thank You. I will try this again but every time I try to place a mutual coupling statement in the schematic (K1 l9=L9 l10=L10 l11=L11 0.5) then running the simulation produces an error. I will have to run it again to copy the error statement as I did not save it. My mutual inductance statement format was found in several documents and produced by the net list.
I will use the simpler statement as you provided and try again.
The mutual inductor statement was changed as suggested. The simulation runs but still produces erroneous results. There are Warnings and a failure in the simulation.
Sounds to me like a tapped inductor. The “physically parallel” (trifilar wound) aspect will improve your coupling coefficient K as shown in my earlier screen grab. Except for that coefficient, you have similar if you put 3 equal windings on the one core and connect them in series without bothering to wind them trifilar.
Sure yes except you PROBABLY need phasing dots on your inductor symbols. I don’t think your schematic editor otherwise knows about the phasing/polarity of L4 and L5.
At least in LTSpice there are different inductor symbols; one or more each with and without the phasing dots.
It certainly IS a tapped inductor, if you were to connect the windings in series. I don’t think physical appearance (really the method of construction) is important, except (as I say) trifilar will give you a higher K = tighter coupling.
SFAIK if you were to instead use one wire to wind 3X turns and solder a tap wire at the two 1X points, the result (magnetically and performancewise) would be the same except for coupling coefficient. OK the interwinding capacitance would be different but I do not see that you are modeling that.
Yes.
But I see a different problem. Yiu can’t just add the three inductances of 1.32 uH together to get 3.96 uH when they’re wound on the same core. Inductance scales with the square of the number of turns.
“One good turn deserves another” but not if you have too much inductance already…
BTW I sorta wish the OP would use engineering notation (my personal preference) or Micro or Nano so we do not need to count the zeros.
I think the post above shows 1.32 uH (1.32e-6) and 2.64 uH (2.64e-6). Engineering notation works correctly in Excel and LTSpice. Does it work in NGSpice?
The warnings occur because there is the voltage source parallel to an inductor. It is not about the ac simulation, but the op which is determined before the ac.
There are two remedies:
Add a small series resistance to each inductor by .options rseries=1m
This is done by other simulators under the hood.
As there are only linear devices in this circuit, you may also suppress op detemination entirely by .options noopac
Transformers are technically really a subset of coupled inductors with a particular application in mind, as pointed out by @BobZ. Usually, the word “transformer” implies that the coupling coefficient between windings is high, or in in other words, the magnetizing inductance is much greater than the leakage inductance. But, the equations, and therefore the models, are the same.
Bifilar, trifilar, and n-filar windings are a particular method of winding to get a high coupling coefficient between the inductances due to each winding. Actually, the value of 0.6 in the simulation looks low to me because I would expect better coupling for a trifilar winding, but perhaps I am missing something here, like a low core permeability.
Don’t confuse the symbol with the model. It’s just a picture that points to the model. If you don’t understand the basic principle of coupled inductors, it would be a good idea to read up on it or you will be randomly simulating stuff and the odds of getting something right are slim.
Finally, at 7 MHz you might be getting close to the realm of transmission line transformers, and that’s a whole 'nother ball game. Hopefully you are not there, because modeling that is quite different from just coupled inductors. A rule of thumb would be to check that the length of the trifilar winding stretched out is << the wavelength at the frequency of interest. At 7 MHz, the free space wavelength is 42 m, so maybe you are ok to neglect transmission line effects.
If the above doesn’t sound familiar, you have a lot of learning to do in order to model this in spice. Start with coupled inductors, and this will be covered in an introductory textbook on electric circuits.
