Author Topic: SPICE parameters for Germanium transistors?  (Read 17745 times)

PRR

Re: SPICE parameters for Germanium transistors?
« Reply #20 on: February 02, 2021, 11:41:57 PM »
..............these results are for silicon transistors...............

Not that it is is material related, but "all" Silicon will have refined junction processing, heavier on Collector.

Same for late Germanium.

Back in the beginning there were several crude ways to make transistors, and some of them made Collectors and Emitters the same. One is to pull a crystal from the melt while alternating N and P dopants so you get a zebra-stripe sausage. Then saw between alternate N stripes so you get P-N-P slices. Another is to put two P pills on a slice of N and bake the whole thing until it almost diffuses-through. Such techniques give no or some control of the two junctions.

And since the "reverse" properties were rarely interesting, they were not specified (don't promise more than the customer demands). And as the processes improved a given device may have different actual parameters in different eras.

I think if it matters to your designs you need to measure the devices you can get and work them into *your* copy of the model. BR is trivial. In a 9V world there may be little need to specify a reverse Early voltage but that's not hard.
  • SUPPORTER

Rob Strand

Re: SPICE parameters for Germanium transistors?
« Reply #21 on: February 03, 2021, 12:12:37 AM »
Quote
Same for late Germanium.
I suspect that's the case for the common parts.

The Ben Holmes articles actually give some numbers,

doc 16

doc 17

Doc   Result

16   Extracted/measured OC44: BF = 46 to 175, BR = 2 to 12
   Pairing min/max:   BF/BR ~ 23 and 14.6
   Taking the average BF = 111, BR = 7;  BF/BR = 15.8
 
17   Extracted/measured OC44 BF/BR = 12.6, AC128 BF/BR = 15.6

So a BF/BR of 15 is in the ball-park

A very leaky OC74 on my desk measured BF=43, BR=3.7, BF/BR = 11.6.

Quote
And since the "reverse" properties were rarely interesting, they were not specified (don't promise more than the customer demands). And as the processes improved a given device may have different actual parameters in different eras.
I don't recall it ever being published.  It might have appeared on one or two obscure datasheets.

Quote
I think if it matters to your designs you need to measure the devices you can get and work them into *your* copy of the model. BR is trivial. In a 9V world there may be little need to specify a reverse Early voltage but that's not hard.
That's always the case.  For spice models you don't want to be measuring stuff *unless* you are making an effort to match measurements on your desk.   It's always nice to have some representative behaviour "out of the box".   The biggest practical issue for spice models for germanium is the leakage.    If varies a lot and it does affect many circuits.

You have to be careful tinkering the gains of spice models.   Sometimes the effective gain in the simulation does not match the gain in the BF parameter.   The number in the BF parameter can be much higher.  The issue arises because the parameters which set the current dependent gain cause a reduction in the simulated gain compared with the BF number.  It's extremely difficult to tinker with those parameters by hand.
« Last Edit: February 03, 2021, 12:17:50 AM by Rob Strand »
The internet:  answers without the need for understanding.

Gert

Re: SPICE parameters for Germanium transistors?
« Reply #22 on: February 03, 2021, 08:48:15 AM »
Quote
I put a lot of stuff through optimizers so I get what you have done here. For some problems I'll use 500 or more random start points with large deviations then take that result and do another 500 with more smaller deviations. It does make a difference.

I have to admit that my description was perhaps a bit too concise; I did not want to overload my post with background information. In fact, my ‘initial guess’ was already the result of numerous manual or partly automated simulations which I had performed to get a clearer picture of where to search for the respective optimum. And of course, I also reduced the random deviations in the course of my successive optimization rounds.

Another point I had found out was that picking only the best solutions from the preceding optimization round for determining the next starting point was usually counter-productive because any such strategy tended to converge to a local optimum instead of the (supposedly) ‘true’ global optimum.

By the way: The MacSpice optimizer uses a refined version of the Nelder-Mead simplex method, which proved to be relatively robust with respect to the specific requirements occurring in the context of electrical and electronic circuits.

Quote
The only thing I could add is to have high and low leakage versions of the models.
Quote
The biggest practical issue for spice models for germanium is the leakage. It varies a lot and it does affect many circuits.

I've made a few heuristical studies in this direction. For the AC128, the maximum values of the collector-base leakage current can indeed be found in the Valvo datasheet; minimum values are not specified, though. The specified maximum is about 2.5 times the average leakage current for all temperatures. For other models, a slightly different factor might apply.

Changing IS accordingly, however, is not a particularly good idea as this parameter affects not only the leakage currents of both junctions, but also the 'Ie vs. Ube' characteristics—and this would inevitably violate my entire optimization!

Without going into details of the corresponding Spice-internal equations, a reasonable first-order heuristic might be to change only the leakage-current-related parameters ISC (and probably ISE accordingly) and XTI so that the red curve in my third plot is shifted upwards by the above amount. Some manual trials revealed that the following parameter changes would be appropriate for my AC128 model:

ISC := ISC * x
XTI := XTI * ³√x

Here, x=6 turned out to be a good choice. The other models will probably require slightly smaller values, but I haven't verified this explicitly. Note, however, that the third root of x might only be valid under the given circumstances, because the corresponding Spice-internal equations also contain XTB and 1/NC as exponents in this same context.

Incidentally, the above changes to the AC128 model didn't affect the other AC128 characteristics significantly, so this might even be a useful general-purpose strategy.

Quote
The leakage can vary widely even for the same part number.

This is true, of course, but it's not only the leakage current that can vary widely. For example, the current gain of the AC128 can vary by a factor of two (or even somewhat more) when taking the average value as reference. However, the primary purpose of my Spice models, and of many other Spice models as well, is to reflect the average behavior sufficiently well. Extreme values are better treated in specific simulations.

For this, I'm using Monte Carlo analyses with at least 1000 random samples, plus optionally extreme-value analyses when the number of parameters (i.e., variable component values) is not much greater than n=10. In the latter case, all 2^n feasible combinations of minimum/maximum parameter values are taken into account in separate simulations, and the minimum and maximum of the resulting curves is evaluated. These two extreme curves are then plotted together with the average curve.
« Last Edit: February 03, 2021, 11:55:46 AM by Gert »

Gert

Re: SPICE parameters for Germanium transistors?
« Reply #23 on: February 03, 2021, 09:00:26 AM »
Quote
I would assume that in a symmetrical device BR==BF within process tolerance.

There were indeed some symmetrical bipolar transistors on the market these days, for example, the AC130 from Valvo; and in this case, BR=BF would indeed be the right choice. I'm not quite a specialist in semiconductor manufacturing technology of the 1960s, but the measurements of relatively small batches of AC128 and OC44 transistors performed by Benjamin Holmes suggest that even these old transistors were quite asymmetrical in this respect; see:

http://www.dafx17.eca.ed.ac.uk/papers/DAFx17_paper_28.pdf

On the other hand, owing to their internal construction, these alloy-junction transistors should not be too far from symmetrical devices, theoretically. And because I hesitated to rely on just a few measured samples (at least several hundred samples from different production batches would normally be required for truly reliable results), I decided to go a bit more towards symmetrical devices and to use somewhat smaller values for the BF/BR ratios (10 instead of Benjamin Holmes' measurements of around 15). I considered this as a reasonable compromise between theoretical expectations and practical measurements.

Besides, many online available images of the internals of such germanium transistors clearly show that the base-emitter region is generally smaller than the base-collector region, which in turn substantiates the assumption that these transistors were not quite symmetrical. See, for example:

https://www.thegearpage.net/board/index.php?threads/x-ray-view-of-germanium-transistors-oc44-mullard-black-glass.935900
« Last Edit: February 03, 2021, 03:40:54 PM by Gert »

Gert

Re: SPICE parameters for Germanium transistors?
« Reply #24 on: February 03, 2021, 09:14:08 AM »
Quote
It's nice to have a model with a reasonable BR. If you run it in reverse at least it behaves half OK.  […]  I can't say I've verified the BR = BF/10 for germaniums but it looks reasonable.

In my opinion, any BF/BR ratio between, say, 5 and 20 would seem to be a more or less reasonable choice for my models. In fact, I simply decided to use a value around the geometric mean of these two extremes.

According to the respective Spice-internal equations, however, the various BJT model parameters are interwoven with each other in a rather complex way. Changing the above basic relation would therefore render my entire model-parameter optimization invalid, thus making it necessary to repeat at least the last few optimization rounds to obtain new sets of optimum parameter values—even if the resulting differences ought to be relatively small in the end.

But once more: The reverse mode of operation is of little practical importance for almost all circuits of interest.

Quote
Not the mention the current dependency. For the 2N3904 the BR drops to the 0.25 to 0.5 region at low currents.

In Spice, the current-dependency of both the forward and reverse current gain is modeled via the IKF and IKR parameters (forward/reverse high-current roll-off corners). Unfortunately, I could do this reliably only for the forward current gain, simply because the datasheets don't contain any information about the reverse mode of operation.
« Last Edit: February 03, 2021, 10:00:16 AM by Gert »

amz-fx

Re: SPICE parameters for Germanium transistors?
« Reply #25 on: February 03, 2021, 09:46:28 AM »
If you want to see how Ge transistors were constructed, there are some closeup pix on my site:

http://www.muzique.com/news/inside-ge-transistors/

One way to make the connections to the base wafer asymmetrical is to use a larger dopant pellet for the collector than the emitter. (Two to three times as large would be common.)

regards, Jack

Rob Strand

Re: SPICE parameters for Germanium transistors?
« Reply #26 on: February 03, 2021, 06:10:27 PM »
Quote
Another point I had found out was that picking only the best solutions from the preceding optimization round for determining the next starting point was usually counter-productive because any such strategy tended to converge to a local optimum instead of the (supposedly) ‘true’ global optimum.
Yes, that can be true.  You need to use a wide spread on the "first pass" and have many start points then the best from all that is as good as you can expect in terms of not getting stuck on a local minima.  The second phase is more about refining the accuracy of the estimate.   Some optimums are very shallow and the algorithms will not find the parameters very accurately (due to rounding).

Quote
By the way: The MacSpice optimizer uses a refined version of the Nelder-Mead simplex method, which proved to be relatively robust with respect to the specific requirements occurring in the context of electrical and electronic circuits.
I've had problems with Nelder-Mead converging to a true optimum.  Filter problems have the most problems because they have a lot of product terms (x1*x2) so the function is the opposite of a separable function.   Random starts helps it a lot.  I haven't spend a lot of time with the refinements which have come about over the last 15 to 20 years - there's so many!  Most of the time I use Quasi-Newton type algorithms.

Quote
Changing IS accordingly, however, is not a particularly good idea as this parameter affects not only the leakage currents of both junctions, but also the 'Ie vs. Ube' characteristics—and this would inevitably violate my entire optimization!
I understand where you are coming from here.    The datasheets present a typical Ie vs Ube, however, on real device the Ube for a given Ie varies from device to device.   For silicon devices the datasheets often indicate Ube variations of +/- 50mV for a given Ie.   If we were to fit Ie vs Ube to these extreme Ube cases the model IS values are just under a decade below and above nominal!  For silicon this the change in leakage has minimal practical effect.   If we have the same Ube variations for germanium the change in Is has a noticeable effect on leakage because the leakage is high enough.

The tolerance in Ie vs Ube cause an IS change which change the leakage compared to the baseline in the optimized model.  The other component comes directly as leakage which are the ISC, XTI parameters you mentioned.   We really need to measure Ube vs Ie to determine IS, then measure leakage.   The ISC, XTI values would be tweaked to take up the difference between the measured leakage and the leakage due to IS.   Not very convenient for a model.   That's why I was saying it's not clear how to handle the leakage.  If we accept an erroneous Ube then we can bundle the leakage in  ISC, XTI.
« Last Edit: February 03, 2021, 06:15:02 PM by Rob Strand »
The internet:  answers without the need for understanding.

Rob Strand

Re: SPICE parameters for Germanium transistors?
« Reply #27 on: February 05, 2021, 10:13:21 PM »
FWIW, here's an overview of the components of leakage.   The main point is it's made up of two parts which behave differently with voltage and temperature.



The internet:  answers without the need for understanding.

Gert

Re: SPICE parameters for Germanium transistors?
« Reply #28 on: February 09, 2021, 01:54:59 PM »
SPICE, Flicker Noise, and Leakage Current

There is one point which should be mentioned in connection with my SPICE models of the seven germanium bipolar transistors: the flicker noise parameters KF and AF. These two parameters control the flicker noise characteristics of the respective transistor, commonly denoted as 1/f noise.

This noise phenomenon is observed in semiconductor devices under biasing and becomes evident towards lower frequencies. It is characterized by a power spectral density which is typically inversely proportional to frequency. The frequency where this noise component is equal in magnitude to the inherent white noise in a semiconductor is known as the 1/f corner frequency.

For the AC127, one of the rare NPN transistors of that era, I had obtained the following parameters from my optimizations, yet still without 1/f noise:

.model AC127_V1 npn (
+  is=10.4u
+  bf=165 nf=0.875 vaf=50 ikf=0.383 ise=0.252u ne=1.22
+  br=16.5 nr=0.875 var=50 ikr=0.383 isc=5.58u nc=1.79
+  rc=0.94 re=0.271 rb=70.4 rbm=14.4 irb=1.33m
+  cje=220p vje=0.3 mje=0.5
+  cjc=294p vjc=0.3 mjc=0.5
+  tf=65.5n tr=655n
+  eg=0.67 xti=13.9 xtb=1.5 fc=0.5
+  tnom=25 )

As regards noise, little can be found in such old datasheets. Nevertheless, I wanted to include at least some reasonable estimates for the 1/f noise characteristics of these BJTs. This, however, turned out to become the very root of a fundamental SPICE issue…

For the AC127, one just finds the following information in the Valvo datasheet:

Rauschzahl bei Ucb = 5V, −Ie = 0.5mA, Rg = 500 Ohm, f = 1kHz, B = 200Hz:    F = 4dB (≤ 10dB)

‘Rauschzahl’ is the German term for noise figure. After all I could find out with reasonable effort, the 1/f corner frequency of such germanium BJTs at emitter currents in the order of 1 mA ought to lie in the lower kHz range, in which case the above operating point would lie in a frequency range where 1/f noise already plays a more or less dominant role.

For my noise simulation, I firstly trimmed the operating point of the AC127 under test in common-base configuration towards the above conditions. With a noise-free load resistance of 500 ohm (at −273.15°C) and a supply voltage of +5.25 V, the resulting collector and emitter voltages were +4.99998 V and −84.832964 mV, respectively; the base was (indirectly) connected to ground. The trimmed DC component of VG1 was −334.832964 mV. The corresponding SPICE netlist without this final trimming was as follows:

**
** Basic test circuit for the AC127_V2 model...
**
**                            RL1 ____
**                          +----|____|----o +5.25V
**                          |
**         ____ RG1         |
**   +----|____|----+       +--------------o out
**   |               \     /
**  _|_             e \   / c
** / ~ \              -----                o gnd
** \___/ VG1            | Q1 (npn)         |
**   |                  |                  |
**   |                  |                  |
**  ===                ===                ===
**

VX1  x1 0  DC 5.25V
VB1  b1 0  DC 0V
VG1  g1 0  DC 0V  AC 1V

Q1   c1 b1 e1  AC127_V2

RG1  g1 e1  500  RMOD temp=25
RL1  x1 c1  500  RMOD temp=-273.15

.model RMOD r ( )

.model AC127_V2 npn (
+  is=10.4u
+  bf=165 nf=0.875 vaf=50 ikf=0.383 ise=0.252u ne=1.22
+  br=16.5 nr=0.875 var=50 ikr=0.383 isc=5.58u nc=1.79
+  rc=0.94 re=0.271 rb=70.4 rbm=14.4 irb=1.33m
+  cje=220p vje=0.3 mje=0.5
+  cjc=294p vjc=0.3 mjc=0.5
+  tf=65.5n tr=655n
+  eg=0.67 xti=13.9 xtb=1.5 fc=0.5
+  kf=854f af=1
+  tnom=25 )

The resistor model ‘RMOD’ is needed to specify operating temperatures for the two resistors, at least in MacSpice. I then obtained the following values for the (external) terminal currents of the above AC127:

    Ic =   500.039 μA
    Ib = −39.0182 nA
    Ie = −500.000 μA

The reference direction of all three currents is into the terminals, that is, the base and emitter currents here flow out of the transistor. Besides the fact that the base current flows in the wrong direction (the AC127 is an NPN transistor), the absolute value of this current is significantly smaller than expected. Even for a modern silicon transistor, one would expect a base current in the order of 1 μA. But let me nonetheless continue.

For a noise figure of 4 dB at 1 kHz, and assuming AF=1 (i.e., genuine 1/f noise), a value of KF=854f was needed—provided that I haven't made a severe mistake in my noise simulation. The corresponding plot is attached (first plot below). From this plot, the 1/f corner frequency can be estimated to be a bit higher than 1 kHz, which is at least not unrealistic.

Yet another suspicious observation was that, following the same basic procedure as for the AC127, the finally obtained KF values for all my other germanium BJTs were significantly smaller, merely in the 15f to 40f range instead of the above 854f. To clarify this mismatch, I made a few more experiments with this otherwise seamlessly working AC127 model. And indeed, for a slightly higher emitter current of 503.571873 μA, MacSpice computed virtually no 1/f noise at all (second plot below).

After some further research, I was able to identify the reason behind this abnormal behavior: the base current of the AC127 at this particular operating point was virtually zero (Ib < 1 fA). It is well known that the leakage currents of germanium transistors are generally several orders of magnitude higher than for silicon transistors. And exactly this collector-base leakage current had completely overtaken the purpose of determining the operating point here. Thus, no additional external base current was required any more—and consequently, the respective SPICE equations didn't compute any 1/f noise!

From a physical point of view, however, such a behavior is not quite plausible. I am well aware that the noise figure of a BJT reaches a minimum for a certain emitter current under given circumstances (operating conditions, generator resistance, etc.), but it cannot really be that the 1/f noise vanishes completely at this operating point; otherwise, it would be relatively easy to construct amplifiers that are virtually free of 1/f noise.

To clarify this, I had to dive deeper into the respective SPICE equations. In the last attachment, you find excerpts from The SPICE Book (by Andrei Vladimirescu, John Wiley & Sons, 1994, pp. 381–384) where the underlying equations are explicitly given. Section A.2.1 contains the set of equations used internally by SPICE to calculate the collector and the base current of a BJT, whereas Section A.2.4 contains the set of equations for noise calculations.

Using the above AC127 model parameters and high-accuracy values of ‘Vbe’ and ‘Vbc’ from a separate operating-point analysis, I was able to reproduce the above ‘Ic’, ‘Ib’, and ‘Ie’ values with an absolute accuracy of better than 1 nA by explicitly applying the corresponding equations (A.8­), (A.9), and (A.10) from The SPICE Book. Thus, these equations seem to be correct and also correctly implemented in MacSpice. The minor differences are most likely due to internally used older values for the physical constants and are therefore negligible.

According to equation (A.22), the 1/f noise calculation is exclusively based on the external base current IB. The collector current IC does not contribute to the 1/f noise as equation (A.23) does not contain a corresponding term.

It should be noted that the notation used in equations (A.22) and (A.23) is a bit imprecise with respect to the currents IB and IC. Since the actual direction of these currents (i.e., their sign) does not matter in connection with noise calculations, only the absolute values are relevant. Hence, a more precise notation here would be |IB| and |IC|, respectively.

IB, in turn, is calculated according to equation (A.9) and consists of four distinct components:

    IB,1 = (IS/BF) ⋅ (eqVBE/NFkT − 1)
    IB,2 = (IS/BR) ⋅ (eqVBC/NRkT − 1)
    IB,3 = ISE ⋅ (eqVBE/NEkT − 1)
    IB,4 = ISC ⋅ (eqVBC/NCkT − 1)

IB,1 and IB,3 are currents flowing from the base to the emitter, whereas IB,2 and IB,4 are currents flowing from the base to the collector. The resulting external base current, which is later used in the 1/f noise calculation, is the sum of these four components:

    IB = IB,1 + IB,2 + IB,3 + IB,4

This may sound plausible, at least at first glance. When the operating point of the transistor is fully determined by its internal leakage currents, however, IB becomes zero, and this inevitably reduces the calculated 1/f noise to zero, too.

Therefore, let us look a bit closer at the above four current components. In the first instance, these are purely mathematical quantities appearing in equation (A.9), which need not necessarily have direct physical counterparts. In particular, IB,1 and IB,3 traverse the same junction, namely the base-emitter junction, whereas IB,2 and IB,4 traverse the base-collector junction. The internal charge transport across a junction in one or the other direction, however, cannot be distinguished in this way; only the resulting current is of interest here. Therefore, the above components can be pairwise combined as follows:

    IB,13 = IB,1 + IB,3
    IB,24 = IB,2 + IB,4

Furthermore, as IB,13 and IB,24 can be considered as independent, the resulting ‘effective base current’ for 1/f noise calculations—and perhaps for noise calculations in general—ought to be as follows:

    IB,eff = √(IB,13² + IB,24²)

I'm not really specialized in noise calculations, but this straightforward refinement would seem to be a simple, yet reasonable fix for the described 1/f noise issue. The attached plot illustrates this, here for a fixed Uce = 5 V (third plot below). In order to use a logarithmical y-scale, I had to plot the ‘IB’ curve in two parts: blue for negative values, green for positive values. The zero-crossing near 85 mV is clearly visible. The red ‘IB_eff’ curve illustrates my proposed fix for the described issue, revealing no abnormal behavior whatsoever.

As can be clearly seen from this plot, SPICE primarily fails in the vicinity of the zero-crossing of the external base current, in which case the computed 1/f noise comes out much too low; in some distance from this critical operating point, SPICE nicely converges to my proposed solution. I therefore decided to derive the 1/f noise parameters for my seven germanium transistors on the basis of these ‘corrected’ SPICE equations instead of the current, highly questionable equations. Without this, most of my SPICE models would have totally wrong KF values, up to two orders of magnitude too high.

Some SPICE users may be tempted to say: “Who cares about such old germanium transistors?” However, the same issue can also be observed in connection with silicon transistors, yet at significantly lower currents and/or higher junction temperatures.

So, in conclusion, one can say:

– SPICE fails to correctly compute 1/f noise of leaky BJTs for certain base currents;
– BJT models with specified 1/f noise parameters should therefore be treated with caution;
– this issue currently seems to exist in virtually all SPICE-based implementations;
– the proposed equations would supposedly fix this issue, if implemented…

Unfortunately, the original SPICE code has not been maintained, at least not at Berkeley, since the last official release of 1993 (SPICE 3f5), and an official contact person for such bug reports does not seem to exist nowadays at Berkeley.

Any comments or suggestions are welcome!








« Last Edit: February 10, 2021, 05:24:05 AM by Gert »

Rob Strand

Re: SPICE parameters for Germanium transistors?
« Reply #29 on: February 09, 2021, 08:21:51 PM »
Thanks again for posting.  It might take me a while to understand the all details.

One thing that stands out is your noise figure set-up.   I'm more familiar with Noise Figure in datasheets being quote for a common emitter configuration.  The source Rg is the source driving the base.  Is there something in the AC127 datasheet which implies a common base configuration?

Quote
Unfortunately, the original SPICE code has not been maintained, at least not at Berkeley, since the last official release of 1993 (SPICE 3f5), and an official contact person for such bug reports does not seem to exist nowadays at Berkeley.
I think there's weird bugs and quirks in many of the pre 2000 spice simulators.   It makes life hard.


EDIT:  Check out these for Noise Figure,
Ambrozy 1971,   input base
https://core.ac.uk/download/pdf/236629329.pdf

Toshiba 2018,p20,input base
https://toshiba.semicon-storage.com/info/docget.jsp?did=63511

Hatton 1951,   input emitter
https://open.library.ubc.ca/media/download/pdf/831/1.0103240/1

« Last Edit: February 09, 2021, 09:56:19 PM by Rob Strand »
The internet:  answers without the need for understanding.

PRR

Re: SPICE parameters for Germanium transistors?
« Reply #30 on: February 09, 2021, 10:06:52 PM »
> SPICE primarily fails in the vicinity of the zero-crossing of the external base current, ....
> Some SPICE users may be tempted to say: “Who cares about such old germanium transistors?”


The casual cynic is tempted to say: "the *designers* of SPICE did not want to care about such old germanium transistors". The apparent simplicity (at normal operating points) of good clean Silicon devices inspired development of calculators. And since Silicon was now readily available and clearly better, why muck around with the math of wheezy old devices?

You also have to be real unlucky to hit the base current null. (Unless you have no base resistor at all, which is done, but not in low-hiss amplifiers.)

As a cave-man, if I discovered this null in the math but not reliably in real life, I would (as you suggest) plot two points away from the null and sketch a curve between.
  • SUPPORTER

Gert

Re: SPICE parameters for Germanium transistors?
« Reply #31 on: February 11, 2021, 09:08:02 AM »
Quote
One thing that stands out is your noise figure set-up.

I have to admit that I had also been a bit irritated by the fact that the Valvo datasheets didn't specify the exact noise measurement set-up. Therefore, I simply tried both variants, common-base and common-emitter, but either set-up yielded almost exactly the same results. Some further Internet research confirmed this basic relationship, too.

I chose the common-base configuration because it was a bit easier to trim these circuits towards the specified operating points. Incidentally, these operating points were identical for all AC transistors for which noise data were explicitly given. For the older OC44 and OC45 transistors, I assumed a somewhat higher noise figure of 10 dB at 1 kHz, borrowed from an OC70 datasheet.

Quote
Check out these for Noise Figure, [...]

Thanks for these interesting links. Particularly Hatton's Master Thesis of 1951 might contain some valuable background information on this whole subject. But it will take me a while, too, to go through all these publications.

Another Master Thesis (by Thomas Frederick Brennan, 1967), which I had found useful for my purposes, is available at:

https://preserve.lib.lehigh.edu/islandora/object/preserve%3Abp-12258981

Gert

Re: SPICE parameters for Germanium transistors?
« Reply #32 on: February 11, 2021, 09:39:28 AM »
Quote
You also have to be real unlucky to hit the base current null. (Unless you have no base resistor at all, which is done, but not in low-hiss amplifiers.)

This is perhaps not as clear-cut as it might seem at first glance. In fact, the operating points specified for noise measurements of all AC transistors (except the AC128, for which no noise figure is given) happened to be not quite far from the zero-crossing of the external base currents. This may just have been a coincidence, but it would have prevented me from deriving correct KF values for all these transistors.

In particular, the KF values of my final SPICE models (i.e., 3.5f to 5.7f for the AC transistors) would have been significantly higher (850f for the AC127, 15f to 40f otherwise) when relying exclusively on genuine SPICE noise simulations. With such KF values, however, the majority of ‘arbitrary’ noise simulations with SPICE would have overestimated the 1/f noise by one or two orders of magnitude.

There are two different aspects, namely model creation and model usage:

The first, obvious aspect is that I wanted to derive reliable general-purpose KF values for all transistor models. For this, I had to take the given noise data, together with the specified measurement conditions, for granted, no matter whether SPICE was able to treat the corresponding operating conditions correctly in its built-in noise simulations. And because it had turned out that this was not the case, I could use SPICE here merely for the underlying operating point analyses. The actual noise calculations had to be performed explicitly, using the corrected SPICE equations; this required some non-trivial code implemented in the MacSpice front-end.

My finally derived KF values should therefore yield mostly correct results in all SPICE noise simulations—except when the operating conditions are too close to the zero-crossing of the external base current.

This leads us to the second aspect, the practical usage of these models. The main problem here is that it is virtually impossible to decide a priori whether the finally resulting operating conditions of a given circuit are sufficiently far from the zero-crossing of the external base current.

Let me take the test circuit for the intermediate ‘AC127_V2’ model from my original post as an illustrating example. Obviously, the operating conditions for the AC127 in common-base configuration are well-defined by the voltage sources VG1 (after adjustment) and VX1 and by the resistors RG1 and RL1: Ucb = 5V and −Ie = 0.5mA, thus not quite abnormal conditions. And as the base is connected to ground, the actual external base current does not have a noticeable effect on these operating conditions, right?

However, as already outlined in my post, this external base current is a priori undefined because it depends on the actual collector-base leakage current of the transistor. In this particular case, it just happens that the internal leakage current is almost equal to the external base current that would normally be observed without any leakage current. This is not easily predictable from the circuit itself, not even when taking the transistor-model parameters approximately into consideration.

In principle, at room temperature, the external base current in this particular circuit could assume any value between, say, 10 μA flowing into the base terminal and several μA flowing out of the base terminal. Hence, SPICE could compute almost correct 1/f noise values in some cases, but it could also underestimate the true 1/f noise by several orders of magnitude in some other cases. This is not quite a satisfactory situation in my opinion.
« Last Edit: February 11, 2021, 03:45:34 PM by Gert »

Rob Strand

Re: SPICE parameters for Germanium transistors?
« Reply #33 on: February 11, 2021, 12:48:28 PM »
Quote
I have to admit that I had also been a bit irritated by the fact that the Valvo datasheets didn't specify the exact noise measurement set-up. Therefore, I simply tried both variants, common-base and common-emitter, but either set-up yielded almost exactly the same results. Some further Internet research confirmed this basic relationship, too.

I chose the common-base configuration because it was a bit easier to trim these circuits towards the specified operating points. Incidentally, these operating points were identical for all AC transistors for which noise data were explicitly given. For the older OC44 and OC45 transistors, I assumed a somewhat higher noise figure of 10 dB at 1 kHz, borrowed from an OC70 datasheet.
Not long after I posted I started to come to the same conclusion.   I have read a lot of papers on noise and I've never noticed that result before.    Figure 7 of this 1954 RCA paper clearly shows the result,

RCA 1954,
http://216.92.159.216/Archives/RCA/RCA-LB/LB-964%20RCA%20Labs%201954%20Investigations%20of%20Noise%20in%20AF%20Amplifiers%20Using%20Junction%20Transistors.pdf
The internet:  answers without the need for understanding.