Please help me with this colpitt oscillator

[Shweta_S]

I have been given the following circuit of colpitt oscillator( with the design values).
I have to check it practically and do it by pspice.
I finished it practically and got the output.
The hfe of the transistor is nearly 400.
When i did the pspice , i am getting amplitude of the output in the range of pV!!!
I don't know what the problem is . Are the design values wrong?

 

[keith1200rs]

You have some weird component values there! The usual problems with simulating oscillators are:

1. You need to kick start them

2. You need to ensure the maximum timestep is smaller than the period of the oscillator

3. If you have a high Q you need to wait a long time. I cannot remember the exact equation but the number of cycles is proportional to Q so with a Q of 10000 you might have to simulate for 50000 Cycles

Keith

 

[Shweta_S]

ya i know.. but it was not designed by me... and i don't know how to design it.

The circuit was just given to me like this.
Can you give me values for which the output might come?
Becoz i don't know the procedure of designing.

 

[E-design]

Must be something with your sim setup. Circuit simulates without any problem (10Vpp @ 24kHz) in Multisim.

 

[Shweta_S]

Oh really!!!... Is there any site where i can download multisim? I don't have it .

Thanks a lot.

 

[E-design]

https://www.ni.com/academic/multisimse.htm

You can also use linear tech free simulator LTspice

https://www.linear.com/

 

[keith1200rs]

Oh really!!!... Is there any site where i can download multisim? I don't have it .

Thanks a lot.

That won't solve your problem. You already have Pspice - you just need to learn more about how to use it. See my earlier suggestions. It simulates fine for me BUT you do need to ensure the timestep is not too large and that it has some sort of "kick". I usually just turn off finding the DC operating point on a transient analysis. A maximum timestep of 500ns and a simulation for a few hundred milliseconds is required before it fully settles down. It oscillates around 25kHz.

Keith.

 

[Shweta_S]

ya true keith... I have to show the output in pspice. I thought there was something wrong with pspice. I look into the suggestions given by you. But if i have doubt about them , please clarify them for me.
Thanks a lot.

 

[keith1200rs]

I used Pspice for years and now use SIMetrix, but all Spice based simulators are pretty similar. Usually just some syntax differences. Which version of Pspice are you using?

By the way, I set the potentiometer as a 100k fixed resistor although there seems to be enough gain for it to oscillate even if that is 10k.

Keith.

 

[Shweta_S]

Since the oscillator starts producing oscillation from noise, we got to introduce a small voltage here in order to start the tank circuit. Have I got this right?

How to kick start? Introduce an ac sin voltage source at the base of the transistor? Nope that doesn't work... I am not sure yet. Please help.

We have to give an initial kick right only for a few nanosec? is that what you mean ? If so how am I supposed to do that on pspice?

Thanks for all your help

Added after 2 minutes:

I am using version 9.1 and I have 9.2 in my laptop.
:!:

 

[keith1200rs]

There are different ways to kick it. One way is to make the power supply a pulses source. Zero volts initially then ramp it up to 18V quickly and stay there.

Another way is a small voltage kick somewhere. Just break the feedback loop, add a small pulsed voltage source which starts a a few mV and then goes to zero shortly after.

I am not sure if the syntax is the same for Pspice, but UIC on the .tran statement skips the bias point calculation in my simulator which is the method I often use e.g.

.TRAN 0 500m 0 500n UIC

Keith.

 

[Shweta_S]

Yay!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

I am so grateful to you Keith!!!!! Thanks a million.

I got it ... thank you

...........And one last doubt... plz explain the syntax of .tran ... I want to what all have you specified for the the kick start . I mean explain each term of that.
That would be very sweet of you.

Added after 2 minutes:

And one more request.
I really want to know all the basic syntax of Pspice... We are not taught of these topics.I learnt a bit on my own without any book or reference. So I need a good reference book or website that may help me to work on Pspice.

 

[keith1200rs]

There are various places you can download the Pspice Evaluation version manuals e.g.:

**broken link removed**

Hspice is pretty close to Pspice but there are some syntax differences. You are probably better off with one of the older manuals such as

www.eecs.lehigh.edu/resources/software/docs/hspiceManual.pdf

The reason for suggesting the older manuals/books is that the newer ones rely on graphically driving simulations from schematics and often don't document the command lines very well, even though that is what is used underneath.

If you want a book - a nice concise one was the book SPICE by Paul T. Tuinenga. I have the 3rd edition from 1995. I think it has been updated, but as a good, well explained book, if you find an old edition second hand cheaply I would get it.

You can find the .tran syntax in the Hspice manual - page 10-4. I am not sure if it it exactly the same for Ppsice.

Keith.

 

[Shweta_S]

Thank you very much.