Why Are My Colpitts Oscillator PSPICE Simulations Inconsistent?

3 replies · 6K views · last reply
darkbasic
Messages
2
Reaction score
0
Scanned textbook page showing a Colpitts oscillator circuit schematic with two capacitors, an inductor and a BJT transistor, with numbered exercise text beside it.
Handwritten derivation on lined paper showing small-signal circuit analysis equations for an oscillator, with a circuit sketch at the top and loop equations and algebra below.
Handwritten derivation on lined paper with a small circuit sketch at top, showing a transistor with labelled components, followed by equations for oscillation conditions and component values.



Hi,
I'm trying to simulate exercise 13.21(a) from Sedra-Smith, with:
  • Vcc=5V
  • f=100 kHz
and the following BJT model:
Code:
.model modn NPN(Is=6.734f Xti=3 Eg=1.11 Vaf=74.03 Bf=416.4 Ne=1.259 Ise=6.734f Ikf=66.78m Xtb=1.5
Br=.7371 Nc=2 Isc=0 Ikr=0 Rc=1 Cjc=3.638p Mjc=.3085 Vjc=.75 Fc=.5 Cje=4.493p Mje=.2593 Vje=.75
Tr=239.5n Tf=301.2p Itf=.4 Vtf=4 Xtf=2 Rb=10)

This is the circuit in pspice:

PSpice schematic of a Colpitts oscillator: NPN transistor Q1 (MODN) with inductor L1 2uH, capacitors C1 and C2 2u, C3 1000, resistors R2 1f and R1 25k, 1uAdc bias current source I1, and 5V and -5V supplies V1 and V2.


(I had to put R2=1f because otherwise the simulation didn't converge)

Since I have two conditions for oscillation:

Code:
Im{A*B(jw)}=0
Code:
A*B(jw0)=1

but three electrical reactancesto size, then I have one degree of freedom so I chosed C1=L.

I also chosed I = 1*10^-6 A which should be fine because the BJT works in the forward-active region.

Unfortunaly when I simulate it I get very different results when I change the Run Time or Max Step Size values:

Screenshot of a PSpice transient simulation window showing a dark plot with a faint, irregular waveform trace over a grid, with a results table panel at the bottom.
Screenshot of a PSpice simulation waveform window showing a mostly blank dark grid plot with faint traces, with a legend and a results panel below.
Screenshot of a PSpice transient simulation window showing a mostly blank black plot grid with faint traces, with the simulation status and settings panels visible along the bottom.
Screenshot of a PSpice simulation window showing a dark-background transient waveform plot with a grid, the trace displaying a periodic signal.



What's wrong? :-(

This is the project file, including the models library if someone wants to try it:
https://drive.google.com/file/d/0Bwe9Wtc-5xF1S0xQb2F2Mkh0REk/view?usp=sharing

Thanks
 
I do not know "Sedra-Smith", but I se several problems with your circuit.

1. The current source will take forever charge a 1000F capacitor (t =C3*V/I = 1000*5/1e-6 = 5e9 seconds or about 158years. You are trying for a frequency of about 700kHz, so go to a larger current and a much smaller capacitor (0.1μF should be large enough by far).

2. L and C are unbalanced. Try multiplying L with 10 and dividing C1 and C2 by 10.

Try this first and see what happens.
 
Finally I found the problem(s), there were many of them!

1) The biggest one were the initial conditions. After selecting "Skip the initial transient bias point calculation" (SKIPBP) in PSpice simulation's options everything got better.
2) Another big problem was in the math: I didn't size reactances well. I did it well, but just barely. In fact assuming A*B(jw0)=1 you barely get a persistent oscillation and a small rounding is enough to let it fade. So I assumed A*B(jw0)=100 when sizing reactances.
3) I had to put another small resistor in the project (R2=1f) because otherwise the simulation didn't converge, but it seems it was too small and I still had convergence problems in some circumstances. So I changed it to 1 mOhm instead.
4) The output capacitor took a long time to load (which wasn't a problem), but also lead to convergence problems in some circumstances. So I changed it to 1nF.
5) I also increased the current generator I1 to 1mA to get the oscillations sooner.
6) Finally I sized the reactances once again, assuming L=C1*10^3 to get more realistic values (but it works even if they are balanced).
7) Now THD is ~1% for the first 50 harmonics!

PSpice schematic of a Colpitts oscillator with NPN transistor Q1 (MODN), inductor L1 52.791u, capacitors C1 52.791n, C2 526.65n, C3 1n, resistors R2 1m and R1 25k load, current source I1 1m, and supply rails of plus and minus 5 V.


PSpice schematic of a Colpitts oscillator with NPN transistor Q1 (MODN), inductor L1 52.791u, capacitors C1 52.791n, C2 526.65n, C3 1n, resistors R2 1m and R1 25k load, current source I1 1m, and supply rails of plus and minus 5 V.
Screenshot of a Cadence schematic simulation window showing a large green plot area with black dots scattered across it, likely a waveform or scatter display; axis labels are too small to read.
Cadence PSpice waveform plot of a Colpitts oscillator output: a flat line near zero at the start that grows into a dense green sinusoid reaching about 5 V peak, with time on the horizontal axis.
Cadence PSpice waveform viewer showing a dense, evenly spaced sinusoidal trace in green on a black grid, with the time axis in microseconds and the amplitude axis ranging roughly from -5 V to 5 V.
circuit5.png
Screenshot of a Cadence PSpice AD simulation window showing an empty frequency-domain plot with a flat red horizontal line near the bottom and a green vertical cursor line at the left edge.


Thanks for your help Svein, it is much apreciated!
 
The reason you need a small resistance in series with the transistor base is because the (undamped) input has a small negative impedance which will tend to create a high frequency oscillation all by itself, ignoring L and C. Usually that does not create a problem in oscillators, but in amplifiers you need to watch out for those spurious oscillations.