-
I have designed and built this band pass filter for low frequency reception between 136kHz and 138khz, to block strong broadcast stations, using ELSIE. It works well. I have built a second one and I am wondering how to connect them in series, but with an input connector, a one filter in use connector, and another connector for both in series. Can I just permanently series connect them and have a co-axial socket on the first filter input, on the tap between them, and a final one on the output of the second filter, or is it not that simple? In other words will having the second filter permanently connected to the first but unused affect the first filter? Thanks
-
If you connect to a tap at the middle point, the presented impedance will be the parallel of the receiver and the second filter (without a termination). So, the match will not be very good, and therefore not only will maximum power transfer not occur, but the first filter will not be operating according to its design parameters.
In practice, you may well find that it works well enough, especially at such low frequencies, an SPDT switch at the tap is the way to do it by the book. With a DPDT, you could have a single output coax connector rather than two.
At higher frequencies, VHF and above, using physical switches in this way is more complex, either you use coax switches or coax relays, or fabricate it on boards with comtrolled impedances. -
Hi Chris,
I am not sure if I understood you question 100%, but these models and results may help:
Although it is not 'textbook', you may get away with it depending on the performance that you need.
The LTspice tool allows the filters to be connected together.
I have attached the LTspice model
Regards,
Jay_Diddy_B
-
You cannot chain odd filters. Obviously, the series branch of one filter, is in series with the series branch of the other filter, so that their inductances/resistances add and capacitances divide, and the filter response is all wrong.
Or shunt branches in parallel, for a pi (rather than tee) configuration. Same thing, just upside down.
You can chain even filters (so that the shunt branch of one filter, connects to the series branch of the next), at least with better expectations than above -- but you still cannot expect perfect results, except for very particular filter types (which I don't think are going to be any of the standard (Butterworth, etc.) prototypes), which support this symmetry.
Incidentally, I notice you've chosen the series-parallel topology, for a very narrow-band filter. This is usually a poor choice. At this low frequency, you can probably get away with it anyway, but you may find a coupled-resonator topology is better. In short, you transform the series (L+C) branches to parallel (L||C) branches, using mutual inductance (k ~= 1/Q) or other means of coupling (tapped inductors, series capacitors, etc.) to link them together.
The AADE filter design tool (available for free download) can calculate this type of filter.
Mind that you still need very good inductors, regardless: the Q factor of each inductor must be many times the filter Q, which is given by the filter's center frequency divided by its bandwidth (or, 136 / 2 = 68). You'll probably have reasonable results with Litz wire on #8 powdered iron cores, or wide-gapped ferrite cores, or very large air core coils.
The filter L and C values must be adjusted slightly to compensate for finite Q. The basic aim is to design the filter for slightly excessive sharpness and ringing; say, choosing a Chebyshev 1dB prototype when you actually want a Butterworth; this exchanges sharpness for insertion loss, so that your final result ends up as sharp as you intended, rolling off due to a combination of reflection and absorption (insertion loss) rather than pure reflection (as a lossless filter would).
Speaking of reflection, you can chain filters that are absorptive in their stop bands -- constant-resistance filters. Note, these are undesirable where high power handling is needed (say if you were rejecting an extremely powerful local 550kHz AM station, or rejecting the harmonics of your class D 136kHz transmitter). There's a best choice for everything.
Tim -
Thanks for the fast replies! I have taken a closer look, using a noise source I treated myself to, but which I previously didn't understand in so far as I hadn't realised what a low output level it had. I just tried using two Chinese broad band amps in series to up the level and fed the output through my single filter, into an SDR receiver and a bandscope. It seems the reality of the filter, whilst quite sharp, is NOT centered on the desired 136 to 137khz. Whilst I appreciate you saying this is not an ideal filter design, it's what I have on a stripboard (and you'll possibly condemn the use of miniature leaded inductors, I don't know...
). But it is what is for now, how might I shift the passband a bit lower, using readily available caps or standard leaded inductor values please? I don't think an trimmer cap anywhere in the circuit is practical, is it? Lots to learn, especially that a modelled circuit may not be the same when built 
Thanks again.
-
Hi Chris,
I am not sure if I understood you question 100%, but these models and results may help:
Although it is not 'textbook', you may get away with it depending on the performance that you need.
The LTspice tool allows the filters to be connected together.
I have attached the LTspice model
Regards,
Jay_Diddy_B
Hi Jay D, thanks very much for the SPICE models, that was very kind of you. I have posted above re shifting the pass band, once i get it centered correctly I will try two in series as I now have a crude means of looking at the filters in "real time"! -
Hi Chris,
The Monte Carlo feature of LTspice can be used to explore the effect of component tolerances.
{mc(100u,0.1)}
Means 100uH nominal value with 10% tolerance.
{mc(100u, 0.05)}
Means 100uH 5% etc.
The results from 5 runs are:
Normally more runs are need to get worst case.
But even from five runs, you need to trim some parts. I would measure the inductors and trim the capacitors.
I have attached the LTCspice model.
Good luck !!
Jay_Diddy_B
-
It seems the reality of the filter, whilst quite sharp, is NOT centered on the desired 136 to 137khz. Whilst I appreciate you saying this is not an ideal filter design, it's what I have on a stripboard (and you'll possibly condemn the use of miniature leaded inductors, I don't know...
).
Ew, mini inductors... those don't have very good Q's.
Consider, you set out to design a filter for -- well, hmm, you didn't really give a spec, you did say 136-138kHz inclusive, but it's not clear how tight around that you actually wanted.
Your filter sim shows about 7.6kHz BW, which implies a filter Q of 18. Commodity coils will get close, but not really be safely above; they certainly won't be the 200 specified in the simulation! You'd have to shop around to find better ones.
But if you're happy with a Q even lower than this, and don't mind a few dB more insertion loss, commodity parts will do well enough.
It's not a matter of me condemning something. That implies I care about some sort of judgement. I don't. It's your radio, it's all up to you if it's good enough or not. All I can tell you is whether some component is likely to meet your need.QuoteBut it is what is for now, how might I shift the passband a bit lower, using readily available caps or standard leaded inductor values please? I don't think an trimmer cap anywhere in the circuit is practical, is it?
Yeah, trimmers don't really come this large. Easy hack: put capacitors in parallel with what's already in the circuit, to increase their values incrementally. Tedious (lots of poking parts in and out), but it is what it is.
Incidentally, it's tempting to hold a capacitor in your fingers (or pliers or whatever), and poke the leads at the circuit. But be careful here, because your fingers have lots of capacitance and resistance. You can probably get away with this on the shunt branches (i.e., in parallel with your stage 3 / Jay's C2), because the impedance is low there. You probably won't get away with it on the series branches, which are high impedance, very sensitive to stray capacitance and resistance.
Easy enough to test -- touch one end of an inductor and watch the passband go off in the weeds!QuoteLots to learn, especially that a modelled circuit may not be the same when built
As I have said many times before and will likely continue saying forever -- it is a poor modeler who blames his tools. There is no bad model, only an incomplete model!
In this case, you've probably not modeled the input and output impedances correctly, and haven't specified the component values and losses accurately. (As Jay notes above, tolerances are important for a filter this tight -- something you cannot possibly get from commodity (typically 5% or worse) parts!)
Tim -
Thanks for the further replies and scans! One more quick question please, I have a still in calibration Fluke / Philips RCL meter that tests at 1kHz 9fixed). How imprtant is the measurement frequency when measuring inductor values, would I be better measuring at a higher frequency with something like an AIM4170 single port "VNA" type device?
-
Real components are far from ideal. Even at that low frequencies, inductors Q and self resonance will trash your filter. You must simulate it using "real" models. Do not underestimate the distributed capacitance of a 680uH inductor.
Also, generaly you cant cascade filters and expect a good response, as they will interact due to reflections, especially at the rejection bands. -
Before computer modelling how would such a filter be optimized, by using variable capacitors and variable inductors?
-
Not as easily; it was many years before filter synthesis was developed. The central challenge is working with polynomial roots, as a function of component values on one side, and certain constraints (like flatness, sharpness or delay) on the other.
The earliest filter design methods are the constant-k and m-derived types, developed by those smart guys at Bell Labs in the early 20th century ( https://archive.org/details/bstj-archives look for articles by Zobel and others). The basic relationship used is the image impedance method.
To put it most simply: using your paired filter example, at the node where the filters are joined, the output impedance of the one filter must match the input impedance of the other filter.
You can view filter impedance, in your simulator probably, by measuring input voltage at constant current (V = I*Z, so if I == 1, V = Z). Mind that Z is a complex (real + imaginary or magnitude * angle) parameter, and both components need to match (real matches real, imaginary matches -imaginary -- a conjugate match).
It should be clear that, for any filter other than a constant-resistance filter, it cannot self-match. A conjugate filter can match to its dual, however, which is in effect one thing I noted above -- a filter with a series output branch, must connect to another filter with a shunt branch.
TL;DR: ground-up filter synthesis is nontrivial, worth many decades of study. You're better off harnessing the knowledge others have derived painstakingly for you. Gain some basic knowledge, so you understand how they can, and cannot, be connected together (the algebra of filters, if you will), and choose the appropriate type as needed.
Tim -
Before computer modelling how would such a filter be optimized, by using variable capacitors and variable inductors?
Correct. Lots of manual tunning iterations until they got the desired response. Of course far from ideal and nearly impossible to get the figures achievable today with good modeling and EM simulation.
However some filters are still tunned nowadays, for example cavity or waveguide microwave filters, due to tolerances in the machining process.