Why Are My Colpitts Oscillator PSPICE Simulations Inconsistent?

  • Thread starter Thread starter darkbasic
  • Start date Start date
  • Tags Tags
    Oscillator Pspice
Click For Summary
SUMMARY

The forum discussion addresses issues encountered while simulating a Colpitts oscillator using PSpice with a specific BJT model. Key problems identified include incorrect sizing of reactances, initial conditions affecting convergence, and the need for adjustments in component values such as increasing the current generator to 1mA and changing the output capacitor to 1nF. The final configuration achieved a total harmonic distortion (THD) of approximately 1% for the first 50 harmonics, demonstrating improved simulation stability and performance.

PREREQUISITES
  • Understanding of Colpitts oscillator design principles
  • Familiarity with PSpice simulation software
  • Knowledge of BJT operation and characteristics
  • Experience with circuit analysis and reactance calculations
NEXT STEPS
  • Explore PSpice simulation settings, particularly "Skip the initial transient bias point calculation" (SKIPBP)
  • Research methods for sizing reactances in oscillator circuits
  • Learn about the effects of component values on oscillator performance
  • Investigate techniques for improving convergence in PSpice simulations
USEFUL FOR

Electronics engineers, circuit designers, and students working on oscillator circuits or using PSpice for simulation and analysis of electronic components.

darkbasic
Messages
2
Reaction score
0
hpscan002.jpg
hpscan005.jpg
hpscan006.jpg



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:

oscillatore1.png


(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:

oscillatore2.jpg
oscillatore3.jpg
oscillatore4.jpg
oscillatore6.jpg



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
 
Physics news on Phys.org
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!

circuit1.png


circuit1.png
circuit2.png
circuit3.png
circuit4.png
circuit5.png
circuit6.png


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.