# Common Emitter Amp - modelled vs actual outputs

Joined Dec 15, 2020
1
Hi All

So I modelled a simple CE amp in LTSpice (asc file attached) which indicated a gain in the input signal of about 4.5x.

I then breadboarded the exact same circuit (with an A50k pot on the output) and put a tone generator through it and only managed to achieve about 1.5x gain. Also tried a number of other transistors (PN100, BC549...) with the same result.

Note the transistor has a measured hfe of 354 (from a DMM with a transistor port), but the model in LTSpice is an unmodified BC547B (hfe about 295).

Is this discrepancy between modelled and real-world response normal? what can I do to push the signal amplification higher?

I've also attached my spreadsheet calculating the resistor requirements for biasing and capacitor selection - being very new to electronics, I'd be keen for some QA.

I'd be using these for audio circuitry - primarily guitar pedals, so input frequencies are likely to be between 30Hz-5kHz to allow for harmonics.

#### Attachments

• 77 KB Views: 24
• 1.6 KB Views: 39

#### Audioguru again

Joined Oct 21, 2019
5,166
This circuit's input impedance is much too low for a guitar pickup. Usually the pickup feeds 1M or more.
The low input impedance of this circuit will kill the level and high frequencies from the pickup.
When fed from a low impedance signal, the gain is increased with a bypass capacitor parallel to the emitter resistor.

#### Attachments

• 44.7 KB Views: 74

#### LvW

Joined Jun 13, 2013
1,561
I then breadboarded the exact same circuit (with an A50k pot on the output) and put a tone generator through it and only managed to achieve about 1.5x gain. Also tried a number of other transistors (PN100, BC549...) with the same result.

Note the transistor has a measured hfe of 354 (from a DMM with a transistor port), but the model in LTSpice is an unmodified BC547B (hfe about 295).
Is this discrepancy between modelled and real-world response normal? what can I do to push the signal amplification higher?
Please note that it is not the hfe value which determines the voltage gain.
It is the transconductance gm at a given operational point (dc current Ic) which is responsible for the gain.
(The BJT acts as a current source - driven by the voltage Vbe).
A higher hfe value (for a fixed operational point) allows a larger input resistance of the stage - that´s all!

#### ericgibbs

Joined Jan 29, 2010
16,370
hi Tim,
This LTS sim demonstrates the point in Post #3 regarding the effect of BF on the circuit Gain.
The BF values are shown on the diagram.

E

#### Attachments

• 36.8 KB Views: 51

#### LvW

Joined Jun 13, 2013
1,561
hi Tim,
This LTS sim demonstrates the point in Post #3 regarding the effect of BF on the circuit Gain.
The BF values are shown on the diagram.
Question: Is it really the BF value which influences the circuit gain?

I dont think so - because in both cases the DC quiescent point (operational point) is not the same (same resistor values are used in both circuits).
So - you are comparing two transistor stages with different quiescent collector currents Ic (different transconductance gm).

For my opinion, a fair comparison of two different transistors in a circuit should be done for equal DC operational conditions only.

#### Audioguru again

Joined Oct 21, 2019
5,166
How did you get a voltage gain of only 1.5 times? Mine shows a voltage gain of 4.5 times when biased with lots of current and a voltage gain a little less at 4.125V when biased with minimum current without any clipping.

Notice that on my simulations I show the DC output to show if the collector current is high or is low, and how far from clipping is the output.

#### Attachments

• 43.9 KB Views: 30

#### ericgibbs

Joined Jan 29, 2010
16,370
hi agu,

I just copied the TS's circuit as posted, no changes.
Used a BC547B_ from my standard.bjt and increased the BF to 350 for the right hand circuit on that sim.
The left side BC547 is the regular LTS transistor.

I would be interested if you can identify any differences.

E

BTW: Please post your asc file and I will give a run.

Update:
Clip from TS's opening post.
So I modelled a simple CE amp in LTSpice (asc file attached) which indicated a gain in the input signal of about 4.5x.

I then breadboarded the exact same circuit (with an A50k pot on the output) and put a tone generator through it and only managed to achieve about 1.5x gain. Also tried a number of other transistors (PN100, BC549...) with the same result.

#### Attachments

• 3.1 KB Views: 6

#### Ylli

Joined Nov 13, 2015
1,058
(with an A50k pot on the output)
Are you sure that is a 50K pot? What load is on the output of the pot? Gain falls to about 1.5 with a 240 ohm load.

#### Audioguru again

Joined Oct 21, 2019
5,166
Hi Eric,
When a transistor is close to cutoff then its voltage gain is reduced, the top of the waveform appears squashed.

#### ericgibbs

Joined Jan 29, 2010
16,370
hi agu,
Using the TS's original circuit.

The transistor in the LTS sim is not close to cut off, there is a 2V overhead voltage between Vc and Ve on the low Vout swing.

Also no distortion on the sine wave output, created a Vref sine wave source,[ see image] it overlays exactly the transistor Vout.

I suspect it could be a problem in LTS or the modelling.

E

#### Attachments

• 46.6 KB Views: 14

#### Audioguru again

Joined Oct 21, 2019
5,166
hi agu,
Using the TS's original circuit.
The transistor in the LTS sim is not close to cut off, there is a 2V overhead voltage between Vc and Ve on the low Vout swing.
Also no distortion on the sine wave output, created a Vref sine wave source,[ see image] it overlays exactly the transistor Vout.
I suspect it could be a problem in LTS or the modelling.
E
Hi Eric,
Tim wanted more gain so I added an emitter resistor bypass capacitor to cause the gain to be 120 times (with lots of distortion).

#### Attachments

• 63.5 KB Views: 13

#### Parkera

Joined May 3, 2016
96
I simulated Tim's original circuit and .stepped the hfe (the Bf transistor parameter) from 100 to 400. Using the .MEASure command, the voltage gain changed from ~4.40 to ~4.46 as shown in the SPICE Error Log. This is a very minor effect on the gain (+1.44%), therefore it can be stated for practical purposes hfe does NOT determine the voltage gain.

In the waveform pane, the yellow traces show the progression, at the collector, of a single cycle. Here you can see the DC quiescent point (measured at 2.5ms) changes from ~4.46 volts to 5.76 volts as the hfe is stepped from 100 to 400. The blue trace shows the AC coupled output waveform which normalizes the four hfe conditions to zero volts. This is what Eric demonstrated in post #4. While the DC quiescent operating point does change some with hfe, it is a fairly minor amount in the order of +2.6% (in this example), and in most situations the change is insignificant where the operating point is close to ½ Vcc.

What does significantly change with hfe is the amount of distortion produced. Using the .four command the THD is:
hfe = 100, THD = 0.238%
hfe = 200, THD = 0.133%
hfe = 300, THD = 0.104%
hfe = 400, THD = 0.091%
The distortion decreased ~262% as the hfe was increased from 100 to 400. This makes sense because the un-bypassed emitter resistor provides negative feedback and trades gain for lower distortion.

Using waveform math, the red traces show exactly how the gain of the stage changes at each point of the waveform when the hfe is stepped from 100 (lower trace) to 400 (upper trace). The huge "spikes" in the center and at the very edges appear exaggerated because a finite output waveform value is being divided by a (near) zero input waveform value. Note how there is progressively more curvature as the hfe is decreased indicating increasing non-linearity distortion, especially on the right-hand side when the transistor approaches cutoff. You can also see how the average gain is increasing slightly with hfe.

#### Papabravo

Joined Feb 24, 2006
19,284
In LTspice you should remember that the BF (Beta Factor) and the actual Beta may be different. They are not intended to be the same. Look at the Gummel-Poon model. I quote from the LTspice Help file

Q. Bipolar transistor
The bipolar junction transistor model is an adaptation of the integral charge control model of Gummel and Poon. This modified Gummel-Poon model extends the original model to include several effects at high bias levels, quasi-saturation, and substrate conductivity. The model automatically simplifies to the Ebers-Moll model when certain parameters are not specified.

Specifically it is the "Ideal maximum forward beta".

#### upand_at_them

Joined May 15, 2010
941

#### Parkera

Joined May 3, 2016
96
Papabravo - thanks for the clarification. Would I be correct in assuming that this is the same as Static Forward-Current Transfer Ratio listed on a transistor data sheet?

You have a negative feedback resistor at the emitter, which reduces gain and makes the overall gain less dependent on hfe.
You have a negative feedback resistor at the emitter, which reduces gain and makes the overall gain less dependent on hfe.
I completely agree. To be even more accurate you should include "little re", which is in series with the emitter resistor and adds to its value (26 ohms/milliamp + contact resistance if I remember my transistor theory correctly). The nice thing about simulators is you don't have to worry about "little re" if you are looking for 1st and 2nd order accuracy and you have good models.

You also have a feedback resistor from collector to base.
The 47K is from +9V, not the collector, therefore it does not contribute to feedback.

#### Bordodynov

Joined May 20, 2015
3,012
I did the calculation with different source impedance values:

#### Attachments

• 2.2 KB Views: 3

#### LvW

Joined Jun 13, 2013
1,561
To be even more accurate you should include "little re", which is in series with the emitter resistor and adds to its value (26 ohms/milliamp + contact resistance if I remember my transistor theory correctly).
...."a little re". To me, this sounds a bit "mystic".
I like to point out that this "little re" is the most important parameter of the transistor. It constitutes the connection between input and output: Transconductance gm=1/re=d(Ic)/d(Vbe).
Hence, re is nothing else than the inverse slope of the control characteristic curve Ic=f(Vbe).

#### Parkera

Joined May 3, 2016
96
I'm not diminishing the importance of the transistor re. When I was taught transistor theory circa 1970 the instructors used Re to represent the physical emitter resistor in the schematic diagram and re to represent the effective emitter resistance of the transistor itself. During discussions of circuit performance the verbal term "little re" was used to differentiate how much each one contributed to the overall circuit performance. I have also seen the term "little re" used in books on the subject, which is why I used it here too.

#### LvW

Joined Jun 13, 2013
1,561
I'm not diminishing the importance of the transistor re. When I was taught transistor theory circa 1970 the instructors used Re to represent the physical emitter resistor in the schematic diagram and re to represent the effective emitter resistance of the transistor itself. During discussions of circuit performance the verbal term "little re" was used to differentiate how much each one contributed to the overall circuit performance. I have also seen the term "little re" used in books on the subject, which is why I used it here too.
Yes - I know that some authors use in their formulas/explanations the symbol "1/re" instead of "gm" .
Why not - if one knows what it means and what it stands for!
Therefore, the question: What does it mean?
Is it really the "effective emitter resistance of the transistor itself"? No - I dont think so.
To me, it is even not a "resistor" - it is a "transresistance" which connects the voltage variation between two nodes (B and E) with a current change through two other nodes (C and E).
Rather, it is a quantity (and we are using the resistor symbol for such a transresistance) which appears in a model, which represents nothing else than the transconductance gm in the formulas for gain and input/output parameters .
(And very often I have experienced that students mix it with the ohmic resistor RE - therefore, I never use "little re".)

#### Parkera

Joined May 3, 2016
96
I think we are looking at the same thing on two different levels, with yours being the more technically correct. My level is what I will call first-order voltage gain of a common emitter stage where "Ae ~ -(0.9Rl/hib), the term hib may be considered as a small resistor in series with the emitter load". As a technician, I never needed to go much deeper than that and most circuits I worked on used an op-amp for gain and transistors for switches, current sources and current buffers and hfe was about all you worried about.