Identify this common-base oscillator with a coaxial output network - Page 1
Forum section: electronics / rf-microwave

author: berke
author_rank: Frequent Contributor
timestamp: January 23, 2024, 09:03:43 am
content: In Bowick's "RF Circuit Design" page 110 you can see a page from a Motorola 2N5179 datasheet with the following oscillator:Questionsa) Is the network essential to the oscillator? (looks like it)b) If yes, what would an equivalent circuit be for simulation?c) How is this type of oscillator called?I did try to simulate that in LTSpice using a bunch of t-lines with open/short ends, but I don't really know what I'm doing and I don't get stable oscillations, and nowhere near 500 MHz.(EDIT: PS: Emitter connection was incorrect, see below.)Bonus points: What's a good way of extracting parameters (hybrid or scattering) in LTSpice from a transistor that's already in a circuit?

author: BigBoss
author_rank: Regular Contributor
timestamp: January 23, 2024, 03:59:54 pm
content: Quote from: berke on January 23, 2024, 09:03:43 am-This is a tricky base grounded oscillator. Because oscillator start-up depends on the load impedance, therefore the author used a "Sliding Tuner" to provide this condition.The feedback is supplied by CCEcapacitance ( maybe interwinding capacitance of RFC ) . L1 and Sliding Tuner Impedance both contribute into Oscillation Frequency-In order to predict the oscillation condition, you have to simulate this circuit by opening Feedback Circuit ( this is not possible in this configuration) and you have to examine the Open Loop Nyquist Criteria. Open loop gain must have a circle and crossing point 1+j*0 point.-Only nonlinear models are used in oscillator analysis, small signal scattering or hybrid linear parameters are useless.-Transient simulation of oscillator circuits are tricky and sometimes misleads you. Start up conditions might be satisfied but oscillator may not seem oscillating.-HB analysis gives you more deeper insight about the oscillators.-I hope you have already found the nonlinear model of 2N5179

author: berke
author_rank: Frequent Contributor
timestamp: January 23, 2024, 05:25:53 pm
content: Quote from: BigBoss on January 23, 2024, 03:59:54 pmThanks, besides the miswired emitter bias, adding a parasitic capacitance to the chokes did it, it's now oscillating in LTSpice, although not very cleanly.QuoteI used the model that was already in the "extended" LTSpice library that's floating around. The input impedance vs. frequency matches what's given in Bowick's book so I guess it's alright.QuoteWould a Middlebrook loop gain probe work in this situation?QuoteBut you talked about the Nyquist criteria which is defined for linear systems? You mean the small signal parameters are useless for determining starting or maintenance conditions?QuoteInteresting, I hadn't heard of harmonic balance. Is that somehow related, more general or more specific than Manely-Rowe relations (which apparently are useful for analyzing frequency multipliers)?

author: BigBoss
author_rank: Regular Contributor
timestamp: January 23, 2024, 11:30:07 pm
content: Quote from: berke on January 23, 2024, 05:25:53 pm-I don't know LTSpice what that probe is. I have no idea.-Yes, Nyquist criteria can be used in this system even tough the oscillator is nonlinear. I have meant that " small signal models (s-parameters etc.) are useless in nonlinear circuits". Otherwise even nonlinear systems can be linearized around operating point and Nyquist criteria is very useful to predict the oscillation frequency. But these small signal parameters are insufficient to characterize the oscillator's mechanism.-HB technique doesn't exist in LTSpice to my knowledge. But any professional simulator such as Keysight ADs, Cadence Spectre, Cadence MWOffice, Ansys Nexxim have it with different options.When an oscillator is examined, the analysis should be done into 2 categories.-Small Signal analysis (prediction of start-up and coarse frequency)-Large Signal Analysis ( details and exact results)An example for 2.4GHz VCO below.

author: G0HZU
author_rank: Super Contributor
timestamp: January 24, 2024, 12:17:55 am
content: QuoteDefinitely not true. Small signal s-parameter models are commonly used for the active device in an oscillator. They are most useful for looking for startup conditions and for out of band instability modes. In my experience small signal s-parameters are usually the very best model in this respect, especially for UHF oscillators.FWIW, I would definitely start off analysing any V/UHF transistor based oscillator using s-parameters and I'd treat this 2N5179 oscillator example as a negative resistance oscillator. At first glance it looks really complicated, but I would recommend you start analysing (just) the BJT as a negative resistance generator. Then add the other components. It should then make more sense what the designer was trying to achieve with the stubs etc.

author: G0HZU
author_rank: Super Contributor
timestamp: January 24, 2024, 02:00:25 am
content: QuoteNo, you don't 'have to' open the feedback circuit to look at the open loop gain to try and predict if/where it will begin to oscillate. It would be much better to simply analyse it as a 1 port device, i.e. a negative resistance oscillator. This analysis method is much simpler and usually works much better.

author: G0HZU
author_rank: Super Contributor
timestamp: January 24, 2024, 02:15:46 am
content: QuoteI think the main goal for this circuit is to allow a hand adjustable method to measure/prove the oscillator output power quoted (at the operating point) in the datasheet. I don't think this is meant to be a practical application circuit because it uses huge and old RF 'tee' connectors in that network. This network would be bad for microphony as well as being physically huge and wobbly. I think it is just a means to explore how much power can be extracted from the 500MHz oscillator by tweaking the line lengths and stubs etc. I don't think it's worth building it unless you want to take a nostalgic trip back about 50 years or so. I've seen this circuit used with other manufacturer's datasheets and I think the aim was the same. To be able to tweak the line lengths to achieve the oscillator output power at the operating point quoted in the datasheet for that particular transistor type. A different transistor type would require slightly different line lengths to get the power output. So the output network is big and clunky and adjustable.It's generally very risky to fit an adjustable (distributed!) network like this to a wideband negative resistance source like that 2N5179. This is because there will probably be several frequencies up above 1GHz where it can generate negative resistance and also achieve resonance at the same time. It might be possible to null some of these out by adjusting the coaxial line lengths, but I don't think this was the main aim. I think they just wanted to adjust for the target output power.

author: berke
author_rank: Frequent Contributor
timestamp: January 24, 2024, 12:50:15 pm
content: Thanks for your replies!QuoteIt's not specific to LTSpice, it's a way of measuring loop gain without manually opening the loop, see herehttps://www.edn.com/middlebrooks-and-rosenstarks-loop-gain-measurementsI don't have a five-digit software budget unfortunately so no Microwave Office for me...I was actually looking for a simple, realistic circuit to check calculations against while reading the book, so I jumped onto that oscillator circuit that looked simple, but clearly it's not and it's not even well-defined (hidden choke parasitic capacitances are required.)But the circuit simulates OK in LTSpice which tells me that the transistor model is good enough at least for learning purposes.What I want to do next is to learn how to extract small signal parameters from a transistor that is in an existing circuit. I expect this to boil down to running AC analyses at the proper operating point with sources at the input and the output and computing V/I ratios.

author: BigBoss
author_rank: Regular Contributor
timestamp: January 24, 2024, 02:04:17 pm
content: Quote from: berke on January 24, 2024, 12:50:15 pmI have never heard about that method neither in textbooks nor application notes. It looks like an ancient method but never heard.Anyway, if you learn more about the oscillation design and simulation techniques, I recommend you to read that book who has written by oscillator Guru Mr. Ulrich RohdeMWOffice of Cadence offers to students (if you are) free of charge license for a limited period. If you wanna work more on this RF circuits whatever are you should learn one of these simulation engines.https://www.amazon.fr/Design-Microwave-Oscillators-Wireless-Applications/dp/0471723428/ref=sr_1_9?__mk_fr_FR=%C3%85M%C3%85%C5%BD%C3%95%C3%91&crid=177ZCIWZH22LN&keywords=ulrich+rohde&qid=1706104889&sprefix=ulrich+rohde%2Caps%2C69&sr=8-9PDF Format version is also available in internet.If you want to extract small signal parameters of the transistor, bias the transistor with appropriate voltage and current, then do a s-parameter simulation.AC Analysis is not used to characterize a transistor. Once you obtain s-parameters, you can convert them to y,z,h,parameters.

author: G0HZU
author_rank: Super Contributor
timestamp: January 24, 2024, 06:12:51 pm
content: Hi berke, You can buy an advanced theory book and a $$$ simulator and the chances are that neither of them will help you that much if you are currently a newcomer to this stuff. The book 'might' have the equations to do this, but you might find an advanced book to be hard going at first.If you want to get an idea of how the circuit works, I still recommend that you analyse the common base BJT as a simple negative resistance generator.You have picked an circuit that is based on a classic negative resistance oscillator. It's possible to strip away a lot of that circuit and just look at the BJT datasheet and use a few simple rule of thumb equations (in Excel?) and you should be able to predict the negative resistance at 500MHz and what reactance the tuning network needs to present to the BJT to make it oscillate at 500MHz.This simple exercise would tell you (roughly) the effective output capacitance of the common base BJT at the collector (use the datasheet here) and also the negative resistance in parallel with it (you need to have a defined operating point in mind, eg 6Vce and 5mA Ic for example).Remember that this stuff was done 50-60 years ago without Microwave Office and even without pocket calculators. You don't 'need' either of them to begin to analyse this circuit in the small signal condition although using a calculator (or Excel) is much nicer than doing it by hand.BigBoss is making out that you need to have access to exotic books and learn how to use exotic CAD tools but in reality, this is a fairly simple circuit to study and understand even at 500MHz

author: G0HZU
author_rank: Super Contributor
timestamp: January 24, 2024, 06:44:49 pm
content: If you want to take it a stage further, and recreate what was done with the stub tuners (to try and prove that the 2N5179 oscillator can produce the 20mW claimed in the datasheet) then things become s lot more challenging if you want to model it. LTSpice might be OK at 500MHz but you could also look at QUCS Studio. I've not tried to use QUCS but it is free.That old output network using the transmission line stubs can be found in lots of old databooks and datasheets. It's sometimes referred to as a two stub matching network and sometimes a three stub matching network is used. It isn't just used with oscillators, it was also used at the output of UHF amplifier circuits given in various datasheets. The aim was the same, to tweak the stubs to prove that the BJT can produce the claimed output power in the datasheet.

author: szoftveres
author_rank: Regular Contributor
timestamp: January 24, 2024, 07:27:54 pm
content: In many ways this circuit looks like the standard "FM bug" oscillator, e.g. the tuned circuit on the collector, and feedback between C and E.I would guess the series LC feedback network needs to be tuned to the fundamental frequency, and whatever resonant network is on the collector needs to absorb the collector capacitance and also bring the node resonance to the fundamental, whether by passive LC components or by λ/4 stubs.It also seems as the transmission line network on the output serves a secondary purpose which is matching the high impedance node of the collector to a low impedance output. This also could be done with lumped LC components, however at 0.5GHz it is just more practical to adjust an adjustable line (as said on the photo), than fiddling with ultra-low value LC components. (EDIT: having said that, the LTSpice model posted above needs 50Ω termination on the output)

author: G0HZU
author_rank: Super Contributor
timestamp: January 25, 2024, 02:32:21 pm
content: Yes, it's just a common base oscillator and the stub network is just a way of matching the output for good power transfer to a power meter. I do have some experience analysing and designing this type of oscillator so can offer some advice if it helps.The 'easiest' analysis can be done by just looking at the BJT on its own in common base as it will generate lots of negative resistance across a huge bandwidth, eg up through 2GHz or so.There are some simple equations to estimate the negative resistance at a given frequency. This is based on the internal capacitances within the transistor and the gm at the chosen operating point. This gives a crude estimate of negative resistance at the collector. This will be in parallel with the output capacitance of the 2N5179. Looking at the datasheet this will be about 0.7 to 0.8pF although this will vary a bit with frequency.This estimates about -3000 ohms will be generated in parallel with 0.7pF at 500MHz at the collector of the 2N5179 at 10Vce and 10mA Ic.If the two turn coil L1 has about 13nH inductance then this needs about 7.8pF across it for resonance at about 500MHz. 0.7pF of this is in the 2N5179 so the stub network needs to present about 7pF to the circuit at 500MHz. There would need to be some sort of resistive loading added as well or the oscillator may settle well away from the initial startup frequency once it is in the large signal condition.The Rp of L1 could be an issue if it doesn't have good Q. It could cancel out a lot of the negative resistance and prevent startup. The same applies to the stub network. It needs to present about 7pF with a fairly high Rp in order for startup to happen.I'll try and demo this in the Genesys simulator. I've got some old s-parameter models of the 2N5179 here that were bundled with Genesys but these are in common emitter. I've also found some MMBT5179 transistors and measured one of these on a VNA to generate the s-parameters at various operating points in common base.

author: G0HZU
author_rank: Super Contributor
timestamp: January 25, 2024, 02:44:35 pm
content: The 1500MHz oscillator shown in the youtube video below is something I designed a year or so ago.This is a common base negative resistance oscillator that uses a transmission line resonator. I used an old BFR91 BJT in common base for the active device. It was designed in a hurry using small signal models.You can see that it is very stable and has very low close to carrier phase noise. Since making it I managed to find some thicker transmission line so I think I can improve it. The line is silver plated and has low loss.

author: berke
author_rank: Frequent Contributor
timestamp: January 25, 2024, 03:05:10 pm
content: Wow so many repliesThanks. Yesterday I started analyzing the circuit by replacing the transistor with the HF hybrid pi model. I'll spare you the hand-drawn sketches. One problem is that books usually give the CE model but don't explicitly say if it's only a common emitter model. Some of them substitute it in CB circuits as well. Not to mention HF simplifications which may be valid for CE but not necessarily for CB.Even though I replaced component blocks by equivalent symbolic impedances I'm getting lots of equations and the probability of making a mistake is 100%.For example I get something like\[i_1\left(1-\left(\alpha\frac{Z_E}{Z_E+r_e} - \frac{Z_{CE}}{Z_C \parallel Z_L}\right)\right) = \frac{v_{\mathrm{in}}}{Z_C \parallel Z_L}\]where $i_1$ is the current through the 50 pF cap.I need to redo it in Maxima. Once I get the symbolic equations I need to figure the actual hybrid pi parameters for the transistor, they didn't specify supply voltages but at Vcc=Vee=15 V current should be about 7 mA.Suppose I then get an output impedance plot. Would the resonance frequency show up as a dip (or peak)? Or maybe instead of impedance I need to look at some differential current gain between two branches?

author: geggi1
author_rank: Frequent Contributor
timestamp: January 25, 2024, 05:51:07 pm
content: When I read this post i remembered this web page.http://www.sm0vpo.com/use/resonator_1.htmThe design is very similar in how it is designed.

author: G0HZU
author_rank: Super Contributor
timestamp: January 25, 2024, 09:39:50 pm
content: Here's a plot of negative resistance vs frequency for the MMBT5179 biased at 6Vce and 3mA Ic. The MMBT5179 is the modern SMD equivalent of the classic 2N5179. They are both 'process 40' devices.To get this plot I've first extracted 2 port s-parameters using a VNA and then entered the model in the top sch1 circuit. You can see that if I place a 2k2 bias resistor at the input and do a 1 port measurement looking back into the collector, there is negative resistance across a huge bandwidth. I also plotted K factor for the sch2 circuit and combined both results on a single plot below. It looks like this BJT could oscillate as high as about 2.3GHz or so as K doesn't rise above 1 until just above this frequency.It shows a negative resistance of -2300 ohms at 500MHz which is slightly better than expected at this bias point. Note that -2300 ohms is more desirable than (say) -4000 ohms if you want lots of margin in the circuit. This may seem counter intuitive but see the calculations below.If (at 500MHz) the Rp of L1 was 5000 ohms and the Rp of the matching network was 9000 ohms then this is 3214 ohms when put in parallel. This is fairly close to -2300 ohms so there isn't much margin here unless more feedback is used in the circuit. It should still start up. Try working out -2300 in parallel with 3214 and the result is still negative. If the negative resistance was -4000 ohms then the parallel result of -4000 in parallel with 3214 would no longer be net negative.The big advantage of using VNA derived small signal parameters is that it's possible to predict the negative resistance of the BJT much more accurately compared to using a non-linear library model of the BJT. That's why I always try and do it the old school way using a VNA or with the manufacturer's s-parameter data.

author: berke
author_rank: Frequent Contributor
timestamp: January 25, 2024, 10:44:42 pm
content: Quote from: G0HZU on January 25, 2024, 09:39:50 pmI've just been trying to extract a negative resistance value in this CB configuration with LTSpice to no avail.I've biased the transistor at 3mA, 6V VCE as indicated with AC bypass, but I don't get negative real small signal vec/ie.Is vec/ie what is meant by negative resistance? I don't understand what I'm missing. If not that maybe an implicit termination or something like that?Would you be kind enough to show exactly how you biased and connected the transistor for your 2-port VNA measurement?

author: G0HZU
author_rank: Super Contributor
timestamp: January 25, 2024, 11:39:39 pm
content: If you aren't familiar with negative resistance then it can be a bit of a mind bender to try and work out what it actually means. However, in reality it actually makes perfect sense once you realise how it is defined and calculated.Have you ever used a CB radio and measured the antenna with a VSWR meter? Hopefully you have. The first thing you do is transmit and then calibrate the meter to full scale. Then you stop transmitting and change the meter to indicate VSWR. Then you transmit again and take the reading for the VSWR.What you are really doing is measuring the magnitude of the reflection coefficient of the antenna (a bit like how a VNA works) even though the meter is scaled as VSWR. Think of the full scale setting of the meter as a perfect reflection of 1. This would be an infinite VSWR that would be seen if you disconnected the antenna cable from the meter.Now it should be obvious that an antenna is a passive device so no matter how badly adjusted it is, you will never see the meter show a higher reading for reflected compared to the calibrated forward reading. The reflection coefficient is always going to be about 1 or less for a passive device.If the meter could also measure the phase angle of the reflected signal the meter could then use an equation to work out the complex impedance of the antenna. This would have a real resistance and a reactance. You are probably well aware of this equation.See the link below and try putting in a reflection coefficient of 0.333 and an angle of zero. This corresponds to a complex load of 100R and no reactance.https://leleivre.com/rf_gammatoz.htmlNow see what happens if you deliberately put in a reflection coefficient of 1.044 and an angle of -14.5 degrees. This has a reflection coefficient greater than 1 and can only happen with an active device (like a 2N5179 in common base with the emitter left unterminated)You should see -66 ohms for the real part of the impedance. A negative resistance!If the reflected waveform is greater than the input waveform then there 'must' be negative resistance present. A VNA can be used to measure this if used carefully.if you convert -66R, -j382 to the parallel equivalent at 500MHz and then convert to capacitance you should end up with about -2300R in parallel with about 0.8pF. This is what the VNA predicts the 2N5179 collector looks like in common base at 500MHz with the emitter effectively unterminated (eg with a high value resistance 2200R or maybe a choke here).

author: G0HZU
author_rank: Super Contributor
timestamp: January 26, 2024, 12:38:36 am
content: I suppose the next thing to do would be to make up an oscillator circuit in Genesys and then test it for real.If the capacitance of the 2N5179 is about 0.8pF then there needs to be about 130nH inductance added for resonance at 500MHz. However, a typical 130nH inductor will have some capacitance and so it would appear to be a much bigger inductance than 130nH at 500MHz.A coilcraft 82nH MIDI inductor looks like 118nH at 500MHz if their s-parameter model is measured at 500MHz. I also need to add a damping resistance of about 3300R to keep the gain margin very low. This resistor will have some self capacitance, especially if I use a leaded metal film resistor rather than SMD. So it could easily add another 0.2pF to the parallel tank.I also need to add maybe 3nH for short soldered connections to the 82nH inductor if I build the oscillator. The Rp of the 82nH inductor will be huge at maybe 85k ohm so this can be ignored. However, I've included it in the model below.This model predicts a net negative resistance (so it should oscillate) and resonance at 460MHz. See the marker is at resonance (zero capacitance) at 460MHz and the resistance is negative.The second image shows the simulated version using the VNA derived model of the 2N5179 and I've also used the official Coilcraft 2 port model of the 82nH inductor. This predicts oscillation at about 467MHz.There's very little margin left (in terms of negative resistance) because of the 3300R damping resistor but it should start up OK when built. I know this because I just built it on a piece of copper PCB

author: G0HZU
author_rank: Super Contributor
timestamp: January 26, 2024, 12:52:38 am
content: Here's an image of it running and the analyser shows oscillation at about 458MHz as expected. It should oscillate very close to the frequency predicted by the small signal analysis because I've damped it right down with the 3300R resistor. If I had used a 2700R resistor it probably wouldn't have started up.I've built it ugly style with direct connections and the base of the BJT is soldered direct to the groundplane. This layout technique should deliver results that are very similar to the simulation. If I had built it on a regular PCB with tracks and pads it would have shifted in frequency which would spoil the result.

author: G0HZU
author_rank: Super Contributor
timestamp: January 26, 2024, 01:52:01 am
content: For a bit of fun I tried changing the resonator to see how high in frequency I could get the MMBT5179 to oscillate. Earlier in the thread I showed a K plot (generated using my VNA data) that indicated that oscillation was possible up to just under 2400MHz (in theory) with the correct resonator attached.This was at a higher Vce and a slightly higher Ic so I tried to make the 2400MHz oscillator at this bias point. It's never going to quite make it to 2400MHz because this would require a lossless resonator but I managed to get really close after a couple of attempts. See the image below.This shows 2310MHz. I could probably get it to 2350MHz (before it stops oscillating) by using a different resonator but this is close enough I think... This should give some confidence in my ability to measure s-parameters with a VNA up at several GHz. I've been doing this stuff for many decades

author: berke
author_rank: Frequent Contributor
timestamp: January 26, 2024, 11:38:29 pm
content: Quote from: G0HZU on January 25, 2024, 11:39:39 pmThank you very much for all the detailed write-up.As far as hand-on experience with standing waves I've only played with a (homemade) bidirectional coupler and the SA's tracking generator, but I believe I understand complex impedances and reflection coefficients.I think my problem was with identifying the inputs and outputs of the common-base configuration which is what I'm not too familiar with. Turns out you apply the input at the emitter and take the output at the collector. Hard to get out of the habit of thinking of the base as an input.Anyway starting from there and using the definitions of two-port admittances I defined the following LTSpice contraption.I made the CB circuit into a symbol and instantiated it twice to be able to have AC-shorted inputs and outputs in the same run.By entering the proper current/voltage expressions in the LTSpice plot window I get admittances. Is this the correct way of doing this?There are no source impedances anywhere.Then using the admittance to scattering conversion formulas I get the following at 100 MHz, 5 mA, 6 V VCE, all values in SCode:y_i=.164-5.61e-3*iy_f=-.156+20.9e-3*iy_r=-72.4e-6-624.9e-6*iy_o=1.35e-3+993.9e-6*iwhich should be equivalent toCode:S11=0.718 < 1°S12=0.001 < 84°S21=0.270 < -7°S22=0.997 < -0°These parameters are at 100 MHz for the CB configuration at the specific bias conditions. Hopefully this is correct, I'm not familiar with the kinds of numbers I should expect. But I don't see any positive gain?The S parameters would be different for CE or CC, right? The datasheet sample included in the book (which I couldn't find online) gives admittance parameters yie,yfe etc. from the e index I gather that this is for a common-emitter configuration.EDIT: Plots.

author: G0HZU
author_rank: Super Contributor
timestamp: January 27, 2024, 10:52:50 pm
content: QuoteI think if you are new to the common base circuit, it really is worth exploring the (positive) internal feedback mechanisms it has and how to model them. Otherwise you will get lost in a soup of equations and even if the equations give good results you won't fully understand what is going on inside the BJT.So for now, I think you need to put your attempts at s-parameter measurements to one side.I think LTSpice has a VCCS model (voltage controlled current source) and this can be very educational as a BJT can be modelled as a voltage controlled current source quite well up at RF.A BJT biased at 3mA has a transconductance (conversion of input voltage to output current) of Ic/26 where Ic is in mA. This is 0.115mA/V or mho.A small RF BJT has various internal resistances as well as capacitances. One of these resistances can be modelled as an internal resistance from collector to emitter in the tens of k ohm range.So I would recommend you play with the simple model and the equations I've shown in the youtube video below. The resistance in the example video is about 27k ohm although this varies from transistor to transistor and also with bias point.The simulation in the video is for a VCCS model of the BFS17 at 3mA Ic but without the internal capacitances or any other resistances inside the BJT. Only the collector-emitter resistance is modelled. Also shown is a common base s2p model of the BFS17 at 3mA Ic. Also shown is a non-linear model of the BFS17. This is the library model of the BFS17 that is included with the Genesys simulator. Also shown is a result for the resistance at the collector using the simple equations given on screen for Rout. These equations are given in the lower left corner of the video in a text box.The important thing to spot here is that this resistance forms a potential divider from the output (collector) to the input (emitter) and because the input and output are in phase with a common base amplifier, this divider introduces positive feedback. Any external wave injected at the collector will be fed back to the input (emitter) via the divider and it will get converted to current by the conductance of the BJT. So this creates positively fed back current to the collector and this boosts up the impedance seen at the collector. The higher the input resistance (Rin) that is terminating the emitter, the more aggressive the feedback as the divider becomes much more effective with higher Rin values.This means that you can't simply guess the output resistance at the collector as being 27k plus the Rin resistance that is in shunt at the input.It will get boosted by the feedback due to the divider. If Rin is close to zero then the resistance 'will' be about 30k ohm but if Rin is increased more and more, the divider and the feedback start to boost the output resistance quite a lot.I'm not sure if the video helps or not, but you can see that the common base amplifier has positive feedback within the device due to the internal resistance. The impact of this can be calculated using the equations seen on the video for Rout at the collector. When the internal capacitances (and the base inductance) are added to the model, the collector resistance will go negative up at VHF and UHF. The non-linear model probably doesn't include any package inductance at the base. Some Spice models are like this too. This can cause errors when trying to work out how much negative resistance is being generated by the device.

author: G0HZU
author_rank: Super Contributor
timestamp: January 27, 2024, 11:26:02 pm
content: The second video below shows what happens when I add just a tiny amount of inductance at the base of the BJT. I only added 1nH to all three models.I also added the collector to base capacitance of about 0.5pF to the VCCS model. You can see that the resistance at the collector suddenly spikes up in the VHF region and then goes heavily negative up into UHF.This is why you can use the BJT in common base to make a simple negative resistance oscillator up at UHF. The various feedback mechanisms within the BJT all contribute towards the negative resistance up at UHF.Note that I've left the Q of the 1nH inductances at the default 1e6 value but it makes no difference in this case if I turn the Q of this inductance down to 5 in all three cases. So I just left it at default.I should also have biased the emitter of the non-linear BJT via a much larger bias resistor than 1k and then used a higher negative voltage as this would have kept the bias point more stable as I varied Rin. But this doesn't really matter much.I think the main thing here is that all three models agree very well. Also the VCCS model agrees exactly with the equation for Rout at the lower frequencies. The blue trace for the s2p model gets really noisy in places as this is because the VNA model is being really stretched here. The VNA can't measure the BJT very accurately down at low frequencies so there is some spiky noise on the trace. There's a lot of measurement uncertainty here but the general agreement with the other models is still quite good. The VNA model will be the best model up at VHF and UHF though...

author: G0HZU
author_rank: Super Contributor
timestamp: January 28, 2024, 12:14:06 am
content: Here's how BJTs are normally measured with a VNA for a common base BJT. The VNA has bias tee connections behind the calibration plane. So as long as the VNA is calibrated right at the input pins of the BJT, the model will only include the properties of the BJT in its SMD package.You can see that the bias voltages would need to be set for a given operating point, eg 6Vce and 3mA Ic. The SG1 voltage feeding the emitter bias tee would have to be negative in this case. The VNA power levels have to be set carefully to maintain the small signal properties of the BJT. It's quite a challenging thing to get right.My VNA can dynamically change the power level on each port and it has a very clever fixture compensation function. This allows me to zoom in and measure right at the pins of the SMD BJT as in the other image. However, this image of the SMD package was for common emitter measurement as you can see that it is the emitter that is grounded.

author: berke
author_rank: Frequent Contributor
timestamp: January 29, 2024, 03:44:33 pm
content: Some progress at last! So far I was using LTSpice exclusively, but I saw that NGSpice can compute S-parameters using the "sp" command. So I gave it a try.Code:COMMON BASE AMPLIFIERVsupply vcc 0 12Vbias Vb 0 2.5RC Vcc Vc 820RE Ve 0 330Q1 Vc Vb Ve 2N5179_FairchildVsource Vin 0 DC 0 AC 1 PORTNUM 1 Z0 50Voutput Vout 0 DC 0 AC 0 PORTNUM 2 Z0 50Coutput Vc Vout 10nCinput Ve Vin 10n.MODEL 2N5179_Fairchild NPN (Is=69.28E-18 Xti=3 Eg=1.11 Vaf=100 Bf=282.1 Ne=1.177 Ise=69.28E-18 Ikf=22.03m+ Xtb=1.5 Br=1.176 Nc=2 Isc=0 Ikr=0 Rc=4 Cjc=1.042p Mjc=.2468 Vjc=.75 Fc=.5 Cje=1.52p Mje=.3223 Vje=.75+ Tr=1.588n Tf=135.6p Itf=.27 Vtf=10 Xtf=30 Rb=10)Turns out the common-base amplifier works but it has low input impedance and high output impedance so that with a 50 ohm load it shows no gain. With emitter follower buffers I was able to simulate an amplifier with actual (although unstable.)Also it seems that "short circuit admittances" actually require the actual source/load impedances.With those changes I'm able to get the same Y parameters using both ngspice nad LTSpice. Converting to S-parameters should just be a matter of algebra.(Yes, ngspice can also plot Smith charts but LTSpice can't so for a quick comparison I used Cartesian plots.)