Hello, I have the same circuit as yours to test a oscillation from that given Colpitts Oscillation, my problem is that it does not work, does not give any wave when debugging while using an oscilloscope. Feel free to check my design if there is any errors, I will gladly appreciate your help. Thanks.

*I am using a proteus software.

 

The node going to C2, C3, and C4 has no DC path to ground. Try a 1 meg ohm resistor from there to ground.

What warning did Proteus give you?

 

@marcmrda,
It works:

What is voltage of your DC source?

 

@marcmrda,
It works:
View attachment 253536
What is voltage of your DC source? View attachment 253556

The voltage of my DC source is 9v.

 

my problem is that it does not work

Watch this video:

In this 9V variant of oscillator distortions are reduced by resistor R5:

 

@marcmrda,
It works:
View attachment 253536
What is voltage of your DC source? View attachment 253556

When I tried to connect the oscilloscope, it does not show any sine wave, Is it the connection of my oscilloscope wrong or? I tried using your diagram and the dc source is 12v.

 

hi marc,
I have just tried Danko's circuit, it works fine.

Disconnect the scope from Transistor Collector and scope only the OUT connection.
BTW:
It takes time to run, so leave it running for say about a minute
E

 

@marcmrda ,
I do not know, will it work for you or not, anyway try it...
In ZIP you can to find file of project Colpitts-Proteus.pdsprj

 

@marcmrda,
Now - with oscilloscope:

 

Beautiful waveform!

I am just curious, I have used a couple of SPICE packages and they both would "freak out" (as we said in the '60's) if a node did not have a DC path to ground. I am amazed that you did not have to provide one for the node involving C2, C3, and C4. How did you get a better SPICE? (A somewhat serious question).

 

I am just curious, I have used a couple of SPICE packages and they both would "freak out" (as we said in the '60's) if a node did not have a DC path to ground. I am amazed that you did not have to provide one for the node involving C2, C3, and C4. How did you get a better SPICE? (A somewhat serious question).

If serious, then look at this simulation:

 

@marcmrda,
Now - with oscilloscope:
View attachment 253774

Thank you so much, sir.

 

@marcmrda,
Now - with oscilloscope:
View attachment 253774

Greetings sir, may I know what does C6 do in the circuit?

 

Thank you. My first impression is that there is something hidden in the simulation but I see that the version of LTspice that I am using supports that circuit and others like it. That'll give me something to think about. I don't want to derail this thread.

 

Greetings sir, may I know what does C6 do in the circuit?

In Proteus simulator, working in animation (particularly oscilloscope), appearingly startup function is absent,
therefore your oscillator do not works with oscilloscope.
So we use single pulse source for "kick-start".
Capacitor C6 separates oscillator circuit from 0.5 μs single pulse source.
- - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - READ please:
"The initial state of oscillators based on a tuned circuit such as phase shift, Wien Bridge and Crystal Oscillators will be defined by their DC bias conditions. If there are no noise sources in the circuit (the default state for all components unless otherwise specified such as resistors defined to have noise contributions) then there is nothing to nudge the circuit away from equilibrium and so it may never start oscillating.

Although in most cases such oscillators will eventually start up due to the ‘hidden’ noise source which is simply due to the mathematical noise generated by the finite resolution and rounding errors of the calculations carried out in running a simulation, this can take a very long time compared to the time taken to run the oscillator in a stable oscillatory state for a few cycles. Crystal oscillators in particular can take many hundreds of thousands of times the oscillator period to start up and reach a stable state.

To minimise the simulation time spent waiting for an oscillator to start, it is useful to introduce some initial start-up condition to ‘kick-start’ the circuit into oscillation.

The simplest way to kick-start most circuits in LTspice is to run a Transient (.tran) Analysis with the startup modifier appended to the end of the .tran directive."

"Another simple way to kick-start an oscillator based on a tuned circuit is to replace a simple DC supply source with a PULSE source set to an initial level of the desired power supply voltage but configured to generate a short pulse of the supply voltage plus or minus some small voltage. So for example a circuit with a 9V supply that is to run for 1ms with a time step of 1us could have a PULSE source set to an initial level of 9V pulsed down to 8.5V for 1us with 100ns rise and fall times. Or an initial level of 8.5V with a delay of 1us before a 100ns rise-time step up to a pulse level of 9V."
https://docs.easyeda.com/en/Simulat...onditions-and-starting-up-circuits/index.html
- - - - - - - - - - - - - -

I don't want to derail this thread.

Why? TS already got helped yet. So, it is o.k.

 

100 kHz Colpitts having low distortion

MicroCap version 4 was a challenge I now use NI multisim or LTspice, it's whatever you get used to.
I have had to clear instrument data, save and reopen file, for me this one works better than the other Colpitts variants.

The frequency was set using 50.6uH and 2) 100nF poly capacitors derived by Colpitts calculator.
The explanation is given on this link about why it works. Adjust the inductor by removing or adding windings.
https://www.calctown.com/calculators/colpitt-oscillator

 

My first impression is that there is something hidden in the simulation but I see that the version of LTspice that I am using supports that circuit and others like it.

Below is quote from Proteus documentation. They use 1TΩ resistor inside of simulator for capacitor leakage imitation.
Seems LTspice works by similar way. We can see result as capacitor current on simulation graph.
Quote:
"Here, the presence of coupling capacitor C1 means that the output probe has no DC path to ground. Consequently, the simulator cannot resolve the operating point for the output, because the operating point is computed with all capacitors open circuit. We have chosen to resolve this by making capacitors very slightly leaky. Therefore, in the absence of any other DC path, the operating point at the output is computed with C1 fully discharged.
The leakyness of capacitors is determined by the simulator control property GLEAK, which is an admittance with default value 1E-12Mho. Setting this value to zero makes capacitors non leaky, as with traditional SPICE simulators.
Apart from the simulation of the innards of DRAM memory circuitry we cannot foresee any problems with this scheme, and it will save relative beginners from many strange error messages. In any case, real capacitors generally have leakage considerably more than a million megohms."

 

That makes sense. That's what I had to do in earlier versions of SPICE.