I am working on understanding BJT transistors through trying to get LTspice IV to produce results that I expect. Of the many pages I've read about transistors, I am currently working off of this one: http://www.learnabout-electronics.org/bipolar_junction_transistors_04.php.

I am trying to (1) identify the range of voltages (by looking at the graph) that are this transistor's active region.
But, where does the ground go? I placed it in the only place it seems to make sense, but it means that I am not able to measure the place it seems to me that the results will appear, presumably because it is just going to be 0V.

After I get that resolved, I want to create a graph that has a sine wave p-p entirely in the active region for the input, and see the same sine wave except with its amplitude enlarged by a DC voltage. This is what I think a pre-amplifier does. I have not yet digested the idea that the transistor is current controlled instead of voltage controlled, which I was hoping to deal with by adding a resistor--after getting something working.

My LTspice IV file is attached along with a snapshot of it. What am I misunderstanding?

 

But your circuit is not a voltage amplifier. Transistor without any external components is nothing more than a piece of a semiconductor with ability to control the current flow.

http://forum.allaboutcircuits.com/threads/common-emitter-amp-doubts-and-questions.91084/#post-663195

 

Your SignalOUT is grounded so obviously the output from that is zero.
You need a collector resistor if you want amplification. And you need to bias the transistor if you want AC amplification.
Suggest you read about common-emitter amplifiers such as here, for example.

 

In addition to grounding your output signal, you have no mechanism of limiting the base current, thus as soon as you forward bias the transistor (about 0.6 V to 0.7 V base-emitter) you will get a very large base current that, in the real world, will destroy the transistor.

 

Thanks all! It's nice to have a direction to go that I know is good. Your answers also indicate that I will finally (perhaps) learn about what all those resistors around a transistor pre-amp circuit are for.

 

It sounds like you've got a cart-before-the-horse situation at play. You are trying to understand a transistor pre-amp circuit before understanding a transistor.

Take a step back and spend some time learning about the characteristics of transistors and then the real simple circuits that can be made from them. That will expose you to the resistors that you often see in such circuits and the roles that they play. Then learn about the basic amplifier topologies and what their characteristics are and why the components around the transistor are and what they do and how they do it. Then you will be ready to understand that preamp circuit.

 

I am specifically trying to learn about transistors, that's why my 'pre-amp' circuit is just a transistor. I just happened to be using a pre-amp context for this post. If I don't keep a practical goal in mind, I lose interest before I get to where I need to be (regarding transistors in this case). My problem is I keep finding horses that need to go before the other horses, especially regarding transistors, which can have such varied applications. For a novice, it sure hasn't helped that the basic physics explanation is different on every web site. After reading plenty I stumbled on an explanation that included (for a change) the importance of the various degrees of doping and why they need to be that way.

 

The physics of why and how a BJT transistor works are very math and modern physics heavy, so lots and lots of analogies have been developed over the years in the attempt to make reasonable mental models of the effect of what goes on in a transistor, usually completely ignoring the actual physics. Some of these models are extremely whimsical including having a leprechaun or other being inside the transistor monitoring the base current and controlling a valve between the collector and emitter in response. Which model works best is very individualistic. I tend to prefer the mathematical models (such as the Ebers-Moll equation) most of the time.

 

My mind tends to shut down when I see lengthy or complex math formulas so I usually go with the simplest black-b0x model that works.
Thus I use a current-controlled current-source model for using BJT's in switching or large-signal applications, and a voltage-controlled current-source (transconductance) model for small(AC)-signal applications.

Of course all my designs are augmented by Spice simulations and Spice uses advanced models, such as Ebers-Moll's, to improve the predicted circuit operation over my hand calculations using the above simple models.

The internal doping of the transistor substrate may be of academic interest but it's of no help in using the transistor in a circuit.

If you want to look at the characteristics of a bare transistor then you can do a characteristic curve plot, which changes thew base current in small steps while changing the collector voltage and observing the collector current such as shown in this article.

 

GregJ7,

You appear to be trying to do 2 different things in 1 circuit, and not quite getting either one done.
(1) Plot the characteristic curves of the transistor model.
(2) Connect the circuit to work in the active region to amplify a sine wave.

Part (1)
LTSpice can do (1) for you. Here is what typical characteristic curves look like (from your link):

http://www.electronics-tutorials.ws/amplifier/amp_2.html

Here's how the graph is created: A current source injects IB into the base. A voltage source creates VCE across the collector. For each blue curve, IB is fixed at a value, starting at 10uA, and VCE is swept from 0 to 13 V. Then IB is set to a higher value, and VCE is swept again. This is repeated for each Ib value that for which you want a curve.

Now, look at those curves. On the left side, the curves are relatively vertical. This area is called "saturation". The bottom of the graph, where Ic and Ib are both zero is called "cutoff". Digital circuits stay primarily on those 2 regions. The area where the curves are relatively flat is the "active" region. This is where amplification gets done.

You can do this with LTSpice with a DC analysis.
Curve trace a 2sc945
Ib 1 0 0 ; 1 is the base node. 0 is always GND. 0 amps injected.
Vce 2 0 0 ; 2 is the collector node. 0 volts at the collector.
Q1 2 1 0 2sc945 ; your transistor
.model 2sc945 npn IS=blah blah ; (type your model parameters in here, blah blah won't work)
.DC Vce 0 13 0.1 Ib 0 100u 10u ; Sweep Vce from 0 to 13V in 0.1V steps. Repeat with Ib=0, 1, 2, 3, 4, 5mA
.END
I'll leave it as an exercise for you to draw that schematic or you can simulate this netlist directly. There's a useful skill. Making a netlist into a schematic.

Part (2)
Now you want to "build" an amplifier in LTSpice. The link you gave is actually decent at telling you how to do this. Just remember that there are 2 distinctly separate parts of the transistor circuit design and analysis:
1. The DC part, also called biasing.

This is where you set the operating point of the transistor. There are no capacitors or signal sources yet. The collector voltage will need to be set to about 50% to 60% of Vcc, to allow enough room above and below the bias point for your output signal swing, when you finally hook it up. The procedure and equations given in your link (http://www.electronics-tutorials.ws/amplifier/amp_2.html) do a good job of walking you through this.​

2. The AC or small-signal part of the analysis.

This is where you need a signal source and possibly coupling and/or bypass capacitors. Everything in the link is correct, but it is incomplete. What the author has not done or explained to you how to do is set the values of C1, C2, and Ce.
These capacitors block DC (C1, C2) or bypass--that is short out--resistors for AC signals. But what is AC? It is signal frequencies. The values of C are what separates DC from AC.
I've run out of time, but for now, try 1uF for C1 & C2, and 100uF for Ce. Experiment with different values. Verify that larger values of C let you amplify lower frequencies, and if you choose C too small, you won't amplify the frequencies you want.

Build the circuit from your link in LTSpice, and see how it goes.

Regards​

 

Also, try playing around with the R values, and see what effect each one has.