I am using to simulate DC and AC amplifiers of 2n3904 but it does not match with my theoretical calculations. My simple circuit is in attachment. Normally IB must be 28,12 uA but it seems 14.9 uA. Also for Ac analysis Vout/Vin should be about -268 but regarding to simulation it is about -180. Could you please help me to solve this problem.
In the Analysis Limits dialog, enter "100,0,20" in the "Temperature" box. This will step temperature from 0°C to 100°C in 20°C steps. This changes the transistor Vbe a bit:
Q1 bias current is (Vb-Vbe)/R1 so it depends on Vbe.
Q1 transconductance depends on bias current. Since there is no emitter resistor in AC, the AC gain of this amplifier is completely determined by Q1's transconductance (the inverse of its emitter resistance).
So stepping temperature acts a bit like picking a different transistor: each transistor will have a bit different Vbe.
I could also step Q1 hFe but this would have no effect here as the signal source impedance is zero ohm. If the signal source was high impedance, then Q1 base current, and thus its hFe, would also matter... so gain would vary according to dispersion of transistor parameters.
So, the gain of this circuit depends on transistor parameters, which means it won't be accurate at all. This is not the circuit to use if you want accurate gain.
You could add resistor R6 to reduce transistor dependent gain variation (and lower the gain). Note capacitor C1's ESR also matters since it is in series.
Another option is to use feedback. C1 ESR is set to 1 ohm.
With this circuit, gain is about 25, and it depends much less on transistor parameters.
Basically you can't get accurate gain above 10-30 with a single transistor. You need multiple stages. You can get inaccurate high gain though, which is useful for maximum open loop gain if feedback is used.
Could you please help me to solve this problem.
- the "model" you use to construct BJT formulas is weak (they normally are)
- the model Spice simulators is much more realistic (normally)
- the spice model has alterable parameters that may cause it to have stupid results
- you can't guarantee that every model is honed to perfection
- your circuit is highly reliant on beta to give you voltage gain (bad)
- it's bad because beta discrepancies will make performance variations both with temperature and from circuit to circuit if you built a few.
- how beta might change with other circuit currents and voltages is more adequately dealt with in a proper simulator with a decent model.
Your numbers don't seem that untypical when making hand calculation vs simulation calculations. Live with it and check the model but you can trust micro-cap as an actual simulation tool (I've run it for circa 15 years now). Yes it has hiccups now and then but, it's my turn-to solver.