Rick Campbell's One Transistor Amp Article

[AB2EZ]

Okay

The circuit you have shown is fine (except the 12V voltage source is drawn upside down). The schematic would look better (but the circuit would not work any differently) if the left side of capacitor C3 was connected to the point where C1 and R2 come together.

The reason you need C3 is to prevent R2 from affecting the biasing of the 2nd stage. Without C3, the combination of R2 (50 ohms) and R6 (150 ohms) in parallel would form the bottom resistor of the voltage divider. The result of that would be to have much too low a base bias voltage on the 2nd stage transistor, and the 2nd stage transistor will not be turned on.

Now to proceed...

Step 1. Temporarily disconnect the top of R5 from the 12 volt supply. This will remove the bias from the 2nd stage... and therefore the 2nd stage's transistor will not be turned on.

Step 2. Do not (yet) apply the 100 mV input signal (i.e. disconnect the input signal from the left side of C2).

Set 3. Turn on the 12V supply (the 100mV rf signal is not connected), and measure the following: a) the DC voltage from the base of the 1st transistor to ground; b) the DC voltage from the emitter of the 1st transistor to ground (i.e. the voltage across the 3 ohm emitter resistor).

Let me know what your measurement results are

Stu

[ssbothwell SWL]

emitter voltage: 0.23V
base voltage: 0.8V

how do those numbers look?

[AB2EZ]

The emitter voltage is okay (and about what I was expecting it to be)

The base voltage is too low. There are several possible reasons for this

a) Recheck your measurment. Make sure you are measuring the voltage from base to ground (not from base to emitter)

b) Make sure your measurement instrument has a high input impedance... i.e., you don't want to use a measurement instrument that has a 50 Ohm load built into its input. If you are using the oscilloscope to measure the dc bias, make sure the oscilloscope's front panel input impedance control is set to the "high impedance" input position.

c) Check the voltage between the collector of the 1st stage transistor and ground. What is your measurement result?

[ssbothwell SWL]

i've been using a Fluke 117 digital multimeter. i checked again and i got roughly the same values. i don't have my oscilloscope (or the second transistor) hooked up at all when doing these tests. the collector-ground voltage is 12.8V



what sort of voltages should i be expecting?

[W4AMV]

I see you are using LT Spice which is fine. I have used Sandia Labs 2n3866 model in switcher CAD with good results at frequencies to 200 MHz. If you bias the device near class C and allow yourself to adjust the collector impedance, than collector eff. can be quite good, above 50 %. Now the thermal problems assocaited with class A are not to restrictive and getting a watt from this device is possible. At a class A bias point it will be quite difficult! In any case, the nonlinear model for the 3866 will function quite nicely in LT Spice and you can experiment there and try a vast number of impedance matching approaches without picking up a soldering iron! Of course, this is a model, and in the end you will have to build the network and see how results match simulation. If you need more power... I have placed multiple 3866 devices in parallel... a bigger BIP device. Last count, I placed 10 in // and easily achieved several watts with 50+% collector efficiency. Again bias points are critical and all of this was CW, not AM. Linearity in my case was not an issue.

Alan

[W4AMV]

On this post for bias. To the extent that the device beta is not infinite, you are going to have to support a base bias current. So... your base bias network may not be "low enough in impedance value"... as a rule of thumb, run a base bias network current at least 1/10 x the collector current... so 50 mA Icq, set the base bias network up for 5 mA. Again, if there is a disconnect on the bench measure, your LT Spice and 3866 model should alert you to the disconnect. I have not looked at the details of your sch. ok, your base bias string is a bit lite at 6.2 mA. I would stiffen it up a bit. GL.

[AB2EZ]

I would have expected the dc base voltage (to ground) to be around 0.7 volts + the voltage from emitter to ground... but let's not worry about that for now.

Step 4. Keep the 2nd stage transistor on the "biased off" mode. Disconnect 1 side of C3, so that the 2nd stage is completely disconnected from the 1st stage

Step 5. Reconnect the 100 mV RF source to the input of the 1st stage (via C2), and measure the peak-to peak rf voltage at the following 3 points: base to ground; emitter to ground; collector to ground.

Let me know what the peak-to-peak reading are.

Stu

[ssbothwell SWL]

heres the readings stu:

emitter-ground: 60-70mV
base-ground: 60-65mV
collector-ground: 400-430mV
across the 50ohm load: 360-370mV
*all these values taken with the ground probe plugged into the breadboard directly next to the power supply negative probe.

its hard to confirming any of these readings. they start to fluctuate if i leave the power supply on, if i adjust any of the parts in their seating on the breadboard, and depending where on the breadboard i ground my oscilloscope and function generator. changes in any of those 3 factors can result in up to 100mV (and sometimes more) shifts in the readings on the collector and across the 50ohm resistor.

i'm also getting some weird 'theramin' like behavior when i connect the scope to the collector. i have the scope connected to the collector and ground. when i move my hand close to the transistor the voltage jumps to 680mV but when i am away from the transistor it is 400-430mV.

the emitter-ground and base-ground waves looked kinda noisy and the emitter-ground one looked a little 'squashed' and noisy. is there a website that shows images of common waveform distortions that i could browse to give you better visual descriptions?


w4amv,

i am using ltspice to draw schematics but i haven't gotten around to learning how to actually run and understand the simulations. is there a good book you can recommend on using spice/ltspice?

[W4AMV]

First off, the base bias on the 3866 per your schematic would be .923 V and assuming 0.7 V drop (nominal VBE) would place the emitter at .225 V. This is just a voltage divider rule calculation. So with your emitter R at 3 ohms, you would expect an emitter current of ~ 75 mA. Of-course this is ideal and you may not see this since device beta is not infinite.

I suggest you open up LT Spice and start by loading the EXAMPLE files and study how these circuits are built in simulation. There is an extensive help menu in LT SPICE and the example files are rich in content. I would put the 3866 to bed. Grab yourself a 2N2222... I nice simple Silicon transistor or better yet a 2N3904 or its complement, a 3906. The models for these devices ARE ALREADY IN LTSPICE. Now go build yourself a nice simple audio amp in LTSpice and get it working in LT Spice.  You already know how to do schematic entry, BUT YOU REALLY ARE missing a very powerful and cool simulator that is FREE. I have built some pretty involved circuits in LT Spice and its capabilities are great. It will provide you with a DC solution so you can check your DC bias points and then you can begin using the AC and transient analysis capabilities to look at far more complex questions. Bottom line... it is a great teaching tool. You can even model tubes and simulate those networks as well. Have FUN. On your direct answer on LT Spice text. LT Spice IS JUST SPICE... Berkley Spice developed back in the ~ 70's been around for quite some time but LT has a excellent GUI. SPICE (Special Program for Integrated Circuit Evaluation) has numerous texts available, you may be able to find them at your local library. Your time invested in learning how to use it will be well invested.

Alan 

[AB2EZ]

Based on your latest measurements and observations... I suggest that the next step is to work on incorporating a ground plane and improving the overall component layout.

At radio frequencies, long leads can act as inductors, and also radiate electromagnetic fields that cause circuits to exhibit (among other things) the kinds of proximity effects you describe.

Here is what I suggest

1. The entire circuit should be (re)built on top of (but, of course, not touching) an electrically conducting surface (usually referred to as a "ground plane"). For this prototyping activity, you can use something ad-hoc. For example, you could take a piece of scrap wood and cover it with a single, continuous piece of aluminum foil or a disposable aluminum cookie sheet.

2. You need to provide some electrical connection points in order to make connectons between some of the components and the ground plane. You could do this (for eample) by attaching a few short pieces of copper wire to the aluminum ground plane with screws and washers. [You can't solder to aluminum; but you can make a good electrical connection by just pressing the copper wire against the aluminum]. Then, when you need to connect a component to "ground", you can just solder it to the nearest copper wire connection point.

3. Lay out your circuit (starting with just the 1st stage, for now) on top of the ground plane... keeping all of the connections as short as possible (preferably every connection between two components, or between a component and the ground plane, should be less than 1 inch in length. If necessary, you can use pieces of electrical tape on top of the ground plane to keep components from touching the ground plane.

4. With respect to the 12 volt power supply:

Use a piece of electrical zip cord, or a twisted pair of wires to connect the + and - sides of the power supply to the circuit. Also (important), at the circuit end end of this connection, close to the circuit components, place one of your 0.1uF capacitors from the +12V lead to the nearest connection point on the ground plane. This will have the effect of making your circuit behave as if the 12 volt power supply was right next to the circuit.

5. With respect to the 100mV rf input signal. Make sure that the connection beteen the 100 mV rf source and the circuit is via a cable with 2 conductors (coaxial cable or a twisted pair). At the circuit board end of this cable, one conductor should be connected to the left side of C2 and the other conductor should be connected to the nearest connection point on the ground plane.

6. When making measurements, use one of the connection points on the ground plane as the place to attach the ground lead of your oscilloscope probe.

Use your ohm meter to verify that all of the connection points attached to the ground plane are electrically connected via the ground plane.

Doing the above (remember, you are still working with just 1 transistor stage) should: greatly reduce the proximity effect you observed, and greatly reduce the noise levels you observed... and will probably increase the ratio of the rf signal between the collector and ground to the rf signal between the base and ground.

Then you can move on to the next steps (e.g., to make some adjustments in the biasing to get rid of the distortion you observed on output waveforms).

Stu

[AB2EZ]

Here are the LTSPICE simulations for the 1st stage:

L= 100uH
V1 = 12.8V
V2= 0.1V peak-to-peak, 7MHz

Blue= base-to-ground: 0.95V average (DC) value and 0.1V peak-to-peak
Green = emitter-to-ground: 0.085V average value (DC) and 0.08V peak-to-peak
Red = across the 50 ohm load resistor: 0V average (DC) and 1.25V peak-to-peak (some distortion)

Voltage gain = 1.25 V / .1V =12.5
Average collector current = 28.4mA

Stu

[AB2EZ]

Here are the LTSPICE simulations for the 2nd stage:

L= 100uH
V1 = 12.8V
V2= 1.25V peak-to-peak, 7MHz
Note R4= 900 Ohms

Blue= base-to-ground: 1.6V average (DC) value and 1.25V peak-to-peak
Green = emitter-to-ground: 0.64V average value (DC) and 1.17V peak-to-peak
Red = across the 50 ohm load resistor: 0V average (DC) and 19.4V peak-to-peak (some distortion)

Voltage gain = 19.4 V / 1.25V = 15.5
Average collector current: 214 mA

Stu

[AB2EZ]

Here are the LTSPICE simulations for both stages:

L= 10uH [As long as L>10uH, the value of L doesn't matter]
V1 = 12.8V
V2= 0.08V peak-to-peak, 7MHz [Note that I have reduced the rf input slightly from 100mV to 80mV peak-to-peak]

Note R8= 900 Ohms; and I have also removed the 1st stage's 50 ohm load. That is: the combination of R2 and R8, and the input impedance of the 2nd stage's transistor, is now the rf load on the 1st stage. I have also added a 50 ohm equivalent series resistor, R5, to the input rf source (V2).

Blue= stage 1 base-to-ground: 0.95V average (DC) value and .057V peak-to-peak
Green = stage 1 emitter-to-ground: .085V average value (DC) and .045V peak-to-peak
Purple = stage 2 base-to-ground: 1.6V average (DC) and 1.21V peak-to-peak
Red = across the 50 ohm stage 2 load resistor: 0V average (DC) and 18.8V peak-to-peak

Voltage gain = 18.8V / .08V = 235
Average stage 2 collector current: 216 mA

Stu

[WA1GFZ]

good luck running a 2N3866 at that current

[AB2EZ]

Frank

I believe you!

I think the 2N3866 is the wrong choice for operation at this frequency and this power level:

a) It has too low a value of HFE (beta), in general; and certainly at collector currents above 50mA
b) Its f_T (unity gain frequency) is much higher than is needed for this application... leading to stability problems with simple layouts that would normally be adequate for this application.
c) Its maximum power dissipation rating is marginal for this application.

Once SWL gets the hang of things... he will probably need to switch to a different transistor in the final design.

Stu

[W4AMV]

Hi Stu. I believe in you simulation that NPN Q1 and Q2 are the default "ideal" LT models. You need to right click on the device, pick a new device, and load in a real model. There are about 30 or so NPN devices in the model library, starting with the 2N2222, 3904 next, etc.... The 3866 may be in the latest version of LT, not sure. If not the Sandia Labs site has a reasonable model. Or, you can build your own model from measured data.

Alan

[W4AMV]

Here is one model description for the 2N3866, not the one from Sandia Labs, but give it a try. The BF seems to large. It might be E2, not E3 !


******
* Spice Model
* Item: 2N3866
* Date: 8/11/10
* Revision History: A
* ==========================================================
* This model was developed by:
* Central Semiconductor Corp.
* 145 Adams Avenue
* Hauppauge, NY 11788
*
* These models are subject to change without notice.
* Users may not directly or indirectly re-sell or
* re-distribute this model. This model may not
* be modified, or altered without the consent of Central Semiconductor Corp.
*
* For more information on this model contact
* Central Semiconductor Corp. at:
* (631) 435-1110 or Engineering@centralsemi.com
* http://www.centralsemi.com
* ==========================================================
******
*SRC=2N3866;2N3866;BJTs NPN; Si;55.0V  0.40A  500MHz   Central Semi Central Semi
.MODEL 2N3866  NPN (
+ IS=13.232E-12
+ BF=1.2948E3
+ VAF=100
+ IKF=.13116
+ ISE=785.43E-12
+ NE=1.7362
+ BR=1.0408
+ VAR=100
+ IKR=3.3880
+ ISC=13.232E-12
+ NC=1.4860
+ NK=.72187
+ RB=8.9057
+ RC=1.7862
+ CJE=31.375E-12
+ VJE=.87558
+ MJE=.31831
+ CJC=7.3111E-12
+ VJC=.76419
+ MJC=.30725
+ TF=178.96E-12
+ XTF=10.044
+ VTF=10.275
+ ITF=5.8742
+ TR=10.000E-9 )
******

[WA1GFZ]

you will need a supply of liquid gas to make a 2222 or 3904 run at that current. The 3866 is a beast and as I said a week ago you are asking way too much power from it. The guy who did that amplifier article is smoking dog poo.
I've been playing with the 3866 for almost 30 years.

[AB2EZ]

Alan

I will try using that SPICE model a little latter this evening...

Frank

Off the top of your head, can you suggest a good choice of transistor for:

1 Watt output, class A (single ended), and <30 MHz applications?

Stu

[W4AMV]

Hi Stu. Here is the Sandia Labs model. I would use this. Note, the BF is reasonable in this listing. 

Let us know how it works out. I agree with the comments on 1 watt levels from the 3866... however, if you optimize the drive level, bias point, and conduction angle, it may be possible to do quite well. I know Rick and he conducts a class on high eff. PA design... you can see his notes and lecture slides on the WEB.

.model 2N3866/27C  NPN     (
+         IS = 9.798605E-15
+         BF = 145.568899
+         NF = 1.007933
+        VAF = 64.3030691
+        IKF = 0.3661244
+        ISE = 1.806705E-14
+         NE = 1.6207001
+         BR = 10.471
+         NR = 1.0003673
+        VAR = 8.322
+        IKR = 0.1449443
+        ISC = 3.326752E-15
+         NC = 1.1076801
+         RB = 15.986
+        IRB = 2.530217E-3
+        RBM = 0.01
+         RE = 0.02604
+         RC = 1.0359
+        CJE = 9.055532E-12
+        VJE = 0.6761546
+        MJE = 0.2754969
+         TF = 1.25476E-10
+        XTF = 13.0616413
+        VTF = 0.4699
+        ITF = 0.2828
+        PTF = 18.9645325
+        CJC = 7.054363E-12
+        VJC = 0.5769848
+        MJC = 0.3139067
+       XCJC = 1
+         TR = 9.098362E-8
+        CJS = 0
+        VJS = .75
+        MJS = 0
+        XTB = 1.831
+         EG = 1.11
+        XTI = 5.0205
+         KF = 0
+         AF = 1
+         FC = 0.9
+ )

[WA1GFZ]

A 2N3866 as a linear amplifier is good for maybe .25 watts with heavy bias.

[WA1GFZ]

The 2N3375 family of stud mounted devices. The 3375 has a 7.5 watt dissipation rating and can be used as a VHF power amplifier. Check the family that goes to 10 watt dissipation if I remember. I used one as the LO amplifier in my homebrew RX making >1/2 watt. The 2N5109 is a higher frequency version of a 3866. I think ft is above 1500 MHz. A pair in push pull will easily make 1/2 watt.  the 2N4427 another good device.
The ARRL Solid State has some very good information on broadband amplifiers for low power and RX use.

[ssbothwell SWL]

hi everyone. i just got home from an insane day at work. all this information looks fantastic and i will go through it all carefully when i am less exhausted tomorrow. thank you so much for all the help!

[ssbothwell SWL]

i figured out how to test circuits in LTSpice, hurray! this will be much more convenient for testing. how do i check current levels in the simulation?

stu, i copied your spice models and got the same results as you. when using the 2n3866 model the wave form is not quite a perfect sinewave. i'm attaching an image of my output with both stages running and a 2n3866.  http://i.imgur.com/kaljg.png

will this biasing method (voltage divider) be okay if i were to switch to a transistor that can better handle high current or am i going to need to setup a biasing system with temperature compensation?

[AB2EZ]

Hi

Good! LTSPICE is very useful for designing circuits... and the price is right. It has lots of capabilities that I have discovered, over time... and lots more that I haven't yet discovered.

A good tutorial reference is http://denethor.wlu.ca/ltspice/#IIIC

Plotting a branch current:

If you put your mouse pointer over a component that is in a branch (e.g. a resistor or an inductor), an arrow will appear. If you click on the arrow, the current in that branch v. time will be plotted. The reference direction of the plotted current will correspond to the direction of the arrow. There are (of course) ways to make the arrow point the other way. One way is to rotate the component by 180 degrees.

Modeling with a real transistor:

Yes... I tried using a number of different real transistors (but not yet a 2N3866) and obtained the same flattening of the lower half of the output waveform. The flattening appears to be associated with the voltage between the collector and the emitter being a bit too low. To fix the problem (at least in the simulation) I added a separate 18V voltage source for the collector (not the biasing) of the 2nd stage. I.e. the top of the 2nd stage inductor is moved from the 12.8V voltage source to the separate 18V voltage source, but everything else stays the same.

In a future implementation of a real amplifier, this moderate amount of distortion will not matter, because higher harmonics will be removed from the output by an output filter.

Using other transistors/biasing:
 
This biasing approach is okay for your first prototype. Once you get a basic, prototype, amplifier working there are a number of alternative approaches for biasing that will do a good job (or even a very good job) of keeping the bias adjusted properly as the transistor parameters change (with temperature or aging). My choice would be to use an op-amp to sample and compare the average emitter voltage to a stable reference voltage... and then employ negative feedback control to adjust the base bias voltage to force the average emitter voltage to equal the reference voltage.

Stu