What clip's this inductor's voltage ? - Page 1
Forum section: electronics / projects

author: MathWizard
author_rank: Super Contributor
timestamp: October 13, 2023, 02:25:54 am
content: I'm working on a 5MHz TX/RX, I'm going for DSB-full carrier. For the TX, I've made another diff. pair mixer, and I'm tying to get the AM working by adding a tank circuit in some configuration. I had something similar work for a 1.4MHz TX/RX I made last winter, but overall it wasn't very good, or matched properly with the wire antenna.But today I'm just wondering why this output looks like it does, and why doesn't LTSpice have the same shape output ?It doesn't matter what combo of RF and AF I've tried, I get this octagonal shape, like stop signs. The output collector in the pictures is basically at 5V=Vcc. I've made a couple of similar circuits with nice looking modulation before, so IDK what goes wrong with this one, that make this stop sign shape. And so far I can't seem to recreate the same shape in LTspice. Overall the sim has been pretty similar to what I've been trying IRL.At 1st I had buffered the diff.amp's output, and had a parallel tank to ground, and that seemed to have similar problems, and not working good, getting that flat top to the AM. I was also trying with a class C amplifier after the diff amp, and so far that won't work nicely either.I've done basic Fourier series before, and RLC circuits, but if the sim doesn't get this output shape, I'm sure I won't either. So I haven't tried to calculate anything for the tank circuit, I just choose the frequency and 1nF to be a lot bigger than the BJT capacitance's. And when I tried 330uH and 3pF, I found the local AM stations showed up more in the circuit. I'll have to see what the internal capacitance are, so far I just did a rough capacitance-free gain version of the circuit.The inductor is just a common green, wire wound, through hole with ~0.5 ohms resistance, or less probably.

author: Kim Christensen
author_rank: Super Contributor
timestamp: October 13, 2023, 03:03:43 am
content: Is C3 an electrolytic? It's not going to do much at 5Mhz...Do you have proper power supply bypassing in the real world circuit? 10 - 100nF across the 5V rail.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 13, 2023, 04:25:28 am
content: Why asymmetrical emitter resistors (R8, R9)? (Why emitter resistors at all?)Check Q1 bias, measure node voltages. Also Q2/Q3 base/emitter voltage isn't much higher than Q1's (compare R5/R4, R2/R1), make sure there's adequate headroom there. Scope will show clipping waveforms if this is the case.C2 doesn't seem to be doing anything; it's too small for boosting AF gain, and RF bypass isn't needed here.The way I like to set up this circuit is, wire R4 and R2 in series (merge into one resistor, making an overall two-tap divider), run one resistor each from the upper bias node (R4/R5) to each base (with C3 on Q3-B still), and that way (R2+R4) sets the bias voltage between the top and bottom parts.Probably tweaking R1 to give symmetrical clipping (Q1 goes into cutoff at the low swing, same when it goes into clipping on the high swing) is what's missing in the waveforms as shown.Simulation tends to overestimate hFE, and your bias levels may simply be lower than expected from simulation. (The base divider being 10s of k vs. R3 being less than 1/100th is a bit iffy.) Individual Vbe differences may be relevant as well.Cheers!Quote from: Kim Christensen on October 13, 2023, 03:03:43 amCompared to a signal of some kohms? It'll do plenty... 1uF at say 2 ohms ESR and a couple 10nH ESL is still quite a low impedance here.Tim

author: duak
author_rank: Super Contributor
timestamp: October 13, 2023, 04:42:54 am
content: Are you using 10X probes and is the scope considering that in the measurement? The scope says it is, but if not, is the actual Q3 Vp-p is about 7.6 V? This circuit should have a fair bit of voltage gain.If it is about 7.6 Vp-p, I would bet that Q3 has its collector-base junction forward biased when the collector voltage drops much below the base voltage causing the envelope to be clamped.

author: Bud
author_rank: Super Contributor
timestamp: October 13, 2023, 05:51:15 am
content: Your biasing scheme is poor. Increase R4 to 47K or 51K to elevate the upper transistors pair bias and to give the lower transistor more voltage headroom on its collector.

author: MathWizard
author_rank: Super Contributor
timestamp: October 13, 2023, 02:02:45 pm
content: Yeah this is all on a breadboard too. Well the last time I made a TX, I did work out some eqn's and got the some modulation eqn from it. I'll have to do all that again, but this time with Cap's added.The biasing was chosen more or less just to have ~2mA tail current, 1.2mA on Q3 for some reason, and have Ve1 down low. Then I just pulled parallel Rbb's out of nowhere really. The output impedance, of the buffer, of the colpitt's osc, is ~13 ohms. Whatever audio amp I make I should try and maximize the power transfer into Q1.My goto eqn's for biasing with divider's and RE's, is to plug I_B=(V_BB-nVt*In(beta*I_B/Is))/(R_BB+(beta+1)RE) into my calculator and solve for I_B, once I've narrowed in on a VBB and RBB, and Vcc, etc.And work up the chain of voltages, and see what resistors will work for some RBB I often pull out of the air. And then usually at the end I'll go with the nearest easy R values, and solve it all one last time.I used Q2/Q3 emitter resistors since I know you should have them with some circuits like output power transistors, I should try and balance them better once I work out the eqn's in more detail, I was trying to make Vb2,3-Vc1 the same.As for C2, I had 47uF for a while, then 1uF, just to short the emitter. And IRL and in the sim, I had some asymmetry in the slew rate of the AM envelope, as it gets bigger then smaller. And I tried 1nF and nothing else, and that got rid of it in the sim and IRL.No the probes are set right, the 12R and tank circuit are just thrown on there. 1st I had a 1.5k-2k collector resistor, and no tank circuit, that was after another buffer. The small signal gain from Vb1 to Vout was ~-76V/V (without cap's in the eqn's, and it was about right). And yeah I have a good bench PSU and a 22uF on Vcc, on a protoboard I'd probably use a bit more, and have a 100n's as well, on most the transistor's in the full circuit.Ok I'll try and match Q2/3 currents better, but the sim still didn't have that stop sign shape. I guess I should try and match the BJT's aswell, and try others too, since it's on a breadboard.

author: Bud
author_rank: Super Contributor
timestamp: October 13, 2023, 07:18:17 pm
content: If it is on the breadboard it will be easy for you to try different bias resistors. Here is a sim to illustrate the point with V3=250mV modulating signal. With your R5 100K and changed it to 68K.Your problem is the upper transistor pair is biased too low which leaves only 0.2V voltage differential between C-E of Q1. Look at the attached pictures where I put DC voltage labels on Q1. With the changed R5 to 68K the headroom increased from 0.2V to 0.6V and the output signal is now looking good.

author: MathWizard
author_rank: Super Contributor
timestamp: October 13, 2023, 10:07:48 pm
content: Well I found a far easier way, just put the RF on the tail current, and the audio on Q2. And now I can use a parallel RLC tank between collector and Vcc, or put the LC tank on gnd and just have Rc alone. And I get a fairly nice AM signal, large or small. For 30mVp 5MHz and 270mVp 1KHz, I get ~160mVp , and has about the same shape as LTspice. Still could be rounder at the envelope peaks, but it happens with small or large signals.Compared to the last TX I made, I get a much much better magnitude gap between my carrier and the nearest radio station. And a couple of days ago, I had a bunch of AM radio stations getting mixed into the spectrum.Oh never-mind, I'm using the signal gen, I guess my Colpitts osc. will still be mediocre. I need to try some filtering, which will probably reduce it down to small signal levels, which is ok for this diff. amp mixer.I can input up to about 100mVp RF, before it can't modulate all the way without running into trouble with 540mVp AF (or was that 270mVp ~VE1), as the gain is fairly high at 5MHz. So for now that's fine, but I'll try and balance it better. This is a learning project as much as it is a practical RX/TX to the kitchen and basement.Actually the Colpitts looks ok, it has a CC buffer, then a 1nF 1uH tank, then straight into the mixer, with it's Rc=1.5k, and the same tank in parallel with Rc. I'll just have to reduce the input strength a bit more, and/or alter the biasing of the mixer. For now I get about 500mVp with zero modulation, but I can only get up to about 30-40% modulation before something gets squeezed.

author: MathWizard
author_rank: Super Contributor
timestamp: October 14, 2023, 10:53:34 pm
content: Ok I took some advice and increased the bottom RE to 470 at Ve~1V, and raised both base divider's. Now after some more low pass filtering and another amplification stage of the oscillator, I now have 290mVp of RF, and can fully modulate it with about 250mVp at 1kHz.It looks better, but is that suitable or typical for AM to feed into some power amp ? I'll have to compare it's AM output to the TX I made last winter.

author: MathWizard
author_rank: Super Contributor
timestamp: October 24, 2023, 02:05:02 pm
content: Now with ro's, Cpi's, Cu's and 1 bypass cap, I worked out the common-mode gain of the diff-amp modulator, so with the tank circuit too.And it's magnitude perfectly matches the AC model and BJT sim up to 1GHz, and the shape of the phase is about right, but I have the phase going from +180 to +5deg for 1Hz to 1GHz, but LTSpice says it's -180 to -365deg.In the Av_cm transfer function, that I've put into a spreadsheet and plotted, I had a negative constant term, so I said it's angle would be +180deg. So if I called it -180deg, then I'd get -180 to -365deg like LTSpice.Or I could add (-360deg) to my total Phase result. So what it LTSpice doing, and what should I be doing ?Also what's missing from the model that causes that other complex root dip at around 3GHz, that the BJT's are doing (red plot) ? I've seen that in other sim, but also missing in those models.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 24, 2023, 04:36:39 pm
content: Quote from: MathWizard on October 24, 2023, 02:05:02 pmNothing very meaningful, at the very least. Are any components (sources, R, L, C) set for parasitic parameters?BC547 certainly can't go that fast, and package impedances (pad, lead and bondwire inductance, and capacitance) must be considered, which I think the LTspice doesn't model (they're bare SPICE .MODELs, an approximation of the semiconductor within, not how it's connected). In any case, it looks like a resonance that should be simple enough to track down by adding and adjusting test values here and there.Tim

author: MathWizard
author_rank: Super Contributor
timestamp: October 25, 2023, 06:27:03 am
content: Good point, so IDK why I'm bothering going out to 100GHz. The real life circuit only has a gain of about 6V/V at 5MHz on a breadboard. I wonder what it would be at 120MHz, the max for my AWG.

author: MathWizard
author_rank: Super Contributor
timestamp: October 29, 2023, 08:38:56 am
content: Now working on these AC models of the circuits in LTSpice, with the diff-amp, the AC model perfectly matches the BJT sim, when I short 1 input and apply a source to the other.But for some reason, if I apply both sources to the AC model, I don't get any modulation at all. The AC model is just the small signal parts, and the gm's , so I don't get why the AC model won't do modulation. I re-copied the circuit to a new file, almost all nodes on the AC model are labelled. I don't get what the problem is, or what rule of LTSpice I'm conflicting with.And I just flipped the Q2 current source B3 in the model, it should be pointing up, just to make sure it wasn't the problem, but I uploaded it like that.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 29, 2023, 04:46:47 pm
content: Modulation is a bilinear operation, AC steady state (and the assumptions that underlie it and produce your circuit) is explicitly linear only. At best you get a superposition, due to the imbalance in the diff pair at the quiescent point approximated around.Note that AC analysis is single frequency, too; superposition isn't supported (other than DC, sort of, but DC is ignored by the assumptions). At best you'd see this in transient analysis.You can use a more developed circuit, say implementing Ebers-Moll in the B sources, to solve this; then you have a simplified transient circuit, which won't show saturation or anything, but you could add the B-C diode to approximate that.If you're curious how SPICE does it in the first place, the default BJT model is based on Gummel-Poon I believe.Tim