Hello, can somebody check my transistor amplifier schematic?

[michael1978]

C2 = 220uF is clearly a mistake. 220pF maybe, but an electrolytic would have a higher inductance than the tuning inductor.
I began to model the circuit with LTspice but have not made it oscillate yet.

Hello, realy, why in ads 2012 he worked, i also download simetrix simulation i built and i get error dcop(error)
i am try to download ads 2012 and to build and to see….

 

[michael1978]

C2 = 220uF is clearly a mistake. 220pF maybe, but an electrolytic would have a higher inductance than the tuning inductor.
I began to model the circuit with LTspice but have not made it oscillate yet.

It seems incongruous to have a 220uF cap in the middle of a HF oscillator (C1).

I rey also 220p but is not working

 

[michael1978]

I did not do it in ltspice because i start with varicap, and i did not find the model and i stop

 

[Baluncore]

You do not need a varicap to check this circuit. Just use a fixed capacitor, then you can step that parameter value.

Some oscillators won't, because of the numerical stability and the perfection of the SPICE model, so it takes a kick to get them going. Sometimes a big kick will give some idea of where the losses are and why it is so dead.

At other times only the smallest tickle is needed which is the case with this Clapp oscillator SPICE model. One solution is to set a starting current of say 1 uA in the first tuned circuit by using an initial conditions statement, for example;
.IC I(L1)=1u0

 

[Baluncore]

This circuit may start without a tickle, it depends on your partricular simulation parameters. Frequency is about 100 MHz.

The pattern is a beat between the pixel pitch and the 100 MHz sinewave.

Two LTspice files attached, remove the .txt extension to run.

 

[michael1978]

This circuit may start without a tickle, it depends on your partricular simulation parameters. Frequency is about 100 MHz.

View attachment 228585

View attachment 228586
The pattern is a beat between the pixel pitch and the 100 MHz sinewave.

Two LTspice files attached, remove the .txt extension to run.

Thank you lottttt sirr

 

[michael1978]

This circuit may start without a tickle, it depends on your partricular simulation parameters. Frequency is about 100 MHz.

View attachment 228585

View attachment 228586
The pattern is a beat between the pixel pitch and the 100 MHz sinewave.

Two LTspice files attached, remove the .txt extension to run.

Hello sir, how you did please, how you find the corrected transistor and varicap, i am jeloze than i don't know,

 

[Baluncore]

how you did please, how you find the corrected transistor and varicap,

I did NOT find the right components, I just made it work well enough to test. I could make the components if I needed them.
I selected the transistors because they will work in that application at 100MHz, they are not optimum.
I did not try to model the varicap as it is not needed to test the design.There are only two varactors in the Ltspice standard library. It is there on the diagram as a "place-holder".

There are many sources of extra models for LTspice. You can edit components from other versions of spice.
You could join the Ltspice group. https://groups.yahoo.com/neo/groups/LTspice/files
then watch https://groups.yahoo.com/neo/groups/LTspice/conversations/messages

See also; http://ltwiki.org/?title=Main_Page
http://www.analog.com/en/design-center/design-tools-and-calculators.html

 

[michael1978]

I did NOT find the right components, I just made it work well enough to test. I could make the components if I needed them.
I selected the transistors because they will work in that application at 100MHz, they are not optimum.
I did not try to model the varicap as it is not needed to test the design.There are only two varactors in the Ltspice standard library. It is there on the diagram as a "place-holder".

There are many sources of extra models for LTspice. You can edit components from other versions of spice.
You could join the Ltspice group. https://groups.yahoo.com/neo/groups/LTspice/files
then watch https://groups.yahoo.com/neo/groups/LTspice/conversations/messages

See also; http://ltwiki.org/?title=Main_Page
http://www.analog.com/en/design-center/design-tools-and-calculators.html

Ohh Man is difficult for me, i don't have experience, but i working cool a,
may i ask you someing did you here about simetrix spic i did the same like you did
and i get strange waveform

 

[tech99]

This looks like spurious oscillation at a much higher frequency. This is why RF engineers are special people.

 

[michael1978]

This looks like spurious oscillation at a much higher frequency. This is why RF engineers are special people.

You want to say is correct waveform?

 

[Baluncore]

may i ask you someing did you here about simetrix spic i did the same like you did and i get strange waveform

It looks to me like the circuit simulation is switching and ringing. Maybe SIMetrix is trying to make it switch like the switching-power circuit SIMetrix is designed to simulate. Apparently SIMetrix runs much faster than Spice, which might explain why it gets it so wrong.

I have not used SIMetrix, nor do I know the circuit or simulation parameters that you have used.

 

[michael1978]

It looks to me like the circuit simulation is switching and ringing. Maybe SIMetrix is trying to make it switch like the switching-power circuit SIMetrix is designed to simulate. Apparently SIMetrix runs much faster than Spice, which might explain why it gets it so wrong.

I have not used SIMetrix, nor do I know the circuit or simulation parameters that you have used.

Hello sir, i find good software, and i have gratis version 7.2 intro,, if you want i can send you...
sorry i make you tired, i make the same like your circuits i just change the transistor bfg520/PS
I configure SEE THE PICTURE

I change the resistor to bf199 and i get this(the same configuration)

 

[Baluncore]

It is hard to read your diagrams, but your C10 looks like 6.8pF. Increase that to 47pF, connected to ground. Open circuit the V3 source and run the simulation for 100usec. If it does not then start and run, you must experiment with a V3 pulse of 100mV or an initial current of maybe 100uA in L1=100nF.

Find the initial current or pulse needed to make it ring then die. That tells you the phase and gain are insufficient to sustain oscillation. Find out how sensitive it is to small changes in component values. Adjust one component at the time to make it ring at about the right frequency for a longer time. When you have sustained oscillation, reduce or remove the initial current used to initiate the oscillation during testing.

 

[michael1978]

It is hard to read your diagrams, but your C10 looks like 6.8pF. Increase that to 47pF, connected to ground. Open circuit the V3 source and run the simulation for 100usec. If it does not then start and run, you must experiment with a V3 pulse of 100mV or an initial current of maybe 100uA in L1=100nF.

Find the initial current or pulse needed to make it ring then die. That tells you the phase and gain are insufficient to sustain oscillation. Find out how sensitive it is to small changes in component values. Adjust one component at the time to make it ring at about the right frequency for a longer time. When you have sustained oscillation, reduce or remove the initial current used to initiate the oscillation during testing.

do you have simetrix, i can gi

It is hard to read your diagrams, but your C10 looks like 6.8pF. Increase that to 47pF, connected to ground. Open circuit the V3 source and run the simulation for 100usec. If it does not then start and run, you must experiment with a V3 pulse of 100mV or an initial current of maybe 100uA in L1=100nF.

Find the initial current or pulse needed to make it ring then die. That tells you the phase and gain are insufficient to sustain oscillation. Find out how sensitive it is to small changes in component values. Adjust one component at the time to make it ring at about the right frequency for a longer time. When you have sustained oscillation, reduce or remove the initial current used to initiate the oscillation during testing.

To which circuit with bc199 or bfg250?because i have 2 one with bc199 and the other with bfg250? i change c10 to 47p is more better waveform, do you have any software i can send you my file, and to run not 5u but 100usec, and to change only the voltage of v3 righ?

 

[Baluncore]

I do not need SIMetrix and I do not have time to learn to use it.
I have Ltspice, which works for me and is free. It has a big user group, forum and library.
If SIMetrix works for you, keep using it. If it does not work, switch to LTspice.

Transistor selection is not critical in that circuit. The transistor simulation model may be important.

 

[michael1978]

I do not need SIMetrix and I do not have time to learn to use it.
I have Ltspice, which works for me and is free. It has a big user group, forum and library.
If SIMetrix works for you, keep using it. If it does not work, switch to LTspice.

Transistor selection is not critical in that circuit. The transistor simulation model may be important.

But i try to bc199, in begin let say 4sec and is about 1.4VPP is good sinus waveform, after in the middle he change the waveform in bigger plus not normal waveform like i told you, NO SIR please don't misundersand me i thougt you know because they are spice, ok sorry what i said, you said to connect to ground C10 47P, and to change L1 to 100uA and V3 where to leave it?

 

[tech99]

I suspect that the spurious oscillation comes from the emitter follower. Try it without.
I also notice that the 220pF capacitors are unusually large for 100MHz. In practice, this might cause trouble due to unwanted resonances involving the self inductance of the component.
Also, I cannot see any purpose in C3.
I have usually found that the fewer components in the oscillator circuit the better, and I especially do not like the use of a resistor in the emitter of Q1 as it is shunting the tuned circuit. I have found the Hartley circuit to require fewest components and be the most reliable.

 

[Baluncore]

... and V3 where to leave it?

Keep V3 on the diagram, but make it open circuit. Keep one side grounded, the other side is no connection.

 

[tech99]

Also, I cannot see any purpose in C3.
.

Apologies, I realize it is a DC block.

 

[michael1978]

Keep V3 on the diagram, but make it open circuit. Keep one side grounded, the other side is no connection.

Ah ok i do it now

 

[michael1978]

I suspect that the spurious oscillation comes from the emitter follower. Try it without.
I also notice that the 220pF capacitors are unusually large for 100MHz. In practice, this might cause trouble due to unwanted resonances involving the self inductance of the component.
Also, I cannot see any purpose in C3.
I have usually found that the fewer components in the oscillator circuit the better, and I especially do not like the use of a resistor in the emitter of Q1 as it is shunting the tuned circuit. I have found the Hartley circuit to require fewest components and be the most reliable.

I will like to do what Balunce say

 

[michael1978]

Keep V3 on the diagram, but make it open circuit. Keep one side grounded, the other side is no connection.

No Sir, is not sinewave, is the same like i told you before, why he don't work in Gods Name

 

[michael1978]

Apologies, I realize it is a DC block.

but this circuit was working in ltspice, the transistor is now bf199 or bfg520/P nothing changes, only transistor

 

[michael1978]

No Sir, is not sinewave, is the same like i told you before, why he don't work in Gods Name

Ah ok i do it now

I change capacitor from 47P, 4.7p, and i chan 5u the transisent is sinewave good, but if i make 10u he destroyd after 5u in bad wafeform

 

[Baluncore]

We have a problem arising here because some component identifications has been changed by michael1978 in the latest diagrams. That needs to be fixed or it will lead to confusion.

I have usually found that the fewer components in the oscillator circuit the better, and I especially do not like the use of a resistor in the emitter of Q1 as it is shunting the tuned circuit. I have found the Hartley circuit to require fewest components and be the most reliable.

Different oscillators have different features. If adding a couple of components reduces harmonics by another 10dB then there will be applications where a higher component count can be an advantage. Reduced component count reduces costs in consumer equipment. It also reduces quality.

The problem with amplifier design is using feedback to advantage, while avoiding self oscillation. I see all named oscillators as being a rogues gallery of failed amplifier designers.

The oscillator being modeled here with the LPF to remove harmonics is a bit confusing. That is because the input and output impedance of the LPF module is not specified and so internal reflections from that LPF occur. I think that LPF is a liability.

 

[michael1978]

We have a problem arising here because some component identifications has been changed by michael1978 in the latest diagrams. That needs to be fixed or it will lead to confusion.Different oscillators have different features. If adding a couple of components reduces harmonics by another 10dB then there will be applications where a higher component count can be an advantage. Reduced component count reduces costs in consumer equipment. It also reduces quality.

The problem with amplifier design is using feedback to advantage, while avoiding self oscillation. I see all named oscillators as being a rogues gallery of failed amplifier designers.

The oscillator being modeled here with the LPF to remove harmonics is a bit confusing. That is because the input and output impedance of the LPF module is not specified and so internal reflections from that LPF occur. I think that LPF is a liability.

this is 150u

i don't understand, when i zoom is bad waveform, what to do next, what to do with lpf, you know, why i told about this simetrix, somebody told me is the best simulator, for that i said to you

 

[michael1978]

this is 150uView attachment 228718
i don't understand, when i zoom is bad waveform, what to do next, what to do with lpf, you know, why i told about this simetrix, somebody told me is the best simulator, for that i said to you

I don't understand also when i make 5u is good sinewave if it goes more is bad sinewave

 

[michael1978]

We have a problem arising here because some component identifications has been changed by michael1978 in the latest diagrams. That needs to be fixed or it will lead to confusion.Different oscillators have different features. If adding a couple of components reduces harmonics by another 10dB then there will be applications where a higher component count can be an advantage. Reduced component count reduces costs in consumer equipment. It also reduces quality.

The problem with amplifier design is using feedback to advantage, while avoiding self oscillation. I see all named oscillators as being a rogues gallery of failed amplifier designers.

The oscillator being modeled here with the LPF to remove harmonics is a bit confusing. That is because the input and output impedance of the LPF module is not specified and so internal reflections from that LPF occur. I think that LPF is a liability.

Hey my dear i fix it, somebody told me, i just change The R4 to 360 and is working THANK YOU A LOTTTT;;;...… SO THAT I MAKE TIRED. THANKS

 

[michael1978]

We have a problem arising here because some component identifications has been changed by michael1978 in the latest diagrams. That needs to be fixed or it will lead to confusion.Different oscillators have different features. If adding a couple of components reduces harmonics by another 10dB then there will be applications where a higher component count can be an advantage. Reduced component count reduces costs in consumer equipment. It also reduces quality.

The problem with amplifier design is using feedback to advantage, while avoiding self oscillation. I see all named oscillators as being a rogues gallery of failed amplifier designers.

The oscillator being modeled here with the LPF to remove harmonics is a bit confusing. That is because the input and output impedance of the LPF module is not specified and so internal reflections from that LPF occur. I think that LPF is a liability.

Sorry sir i wil like to ask the last one i think, everything was okej yesterday with sinewaveform, but today i connect the varicap and i start to get bad sinewave?
what do you think?

 

[Baluncore]

You must use the correct spice varicap model and parameters. I do not know which spice model varicap you are using.

You know the low and high frequency ends of the FM band. The Local Oscillator frequency range needed is offset by the IF frequency. You can calculate or simulate the capacitance needed to maintain oscillation at the ends of the band. Select from manufacturers data an available real varicap that provides the required variation in capacitance. Find or make a spice model of that varicap.

The BBY40 was originally used. I google 'BBY40 spice model' and find;
http://www.gunthard-kraus.de/Spice_Model_CD/Vendor List/Zetex/bby40.lib

* ZETEX BBY40 Spice Model Last revision 18/8/92
.MODEL BBY40 D IS=7.417E-15 N=1.058 RS=.1259 XTI=3
+ EG=1.11 CJO=64.39E-12 M=1.013 VJ=2.566 FC=.5 BV=45.12
+ IBV=.1232 TT=215E-9
*
* + ISR=1.731E-12 NR=2.27 IKF 9.882 (LATER SPICE VERSIONS ONLY)

Each version of spice uses a different way to create and integrate new component models. You must become an expert in your selected version of spice. Take a look at an existing spice varicap model and work out what parameters must be changed to make your BBY40 model.

You may have to change other component values such as the LO tuning inductance and the surrounding capacitors. The original paper with the circuit includes a section on LO tuning and varicap selection, see page 5 and 6 of “Local Oscillator for FM Broadcast Band, 88-108 MHz”, from Lund University, 2012.

 

[tech99]

Sorry sir i wil like to ask the last one i think, everything was okej yesterday with sinewaveform, but today i connect the varicap and i start to get bad sinewave?
what do you think?

A varicap (or varactor) diode is swung by the RF voltage as well as the DC tuning voltage, so it creates distortion and harmonics. Varactor diodes were used as efficient harmonic generators at UHF before high power transistors became available. They were also used in parametric amplifiers, providing low noise microwave amplification.

 

[michael1978]

A varicap (or varactor) diode is swung by the RF voltage as well as the DC tuning voltage, so it creates distortion and harmonics. Varactor diodes were used as efficient harmonic generators at UHF before high power transistors became available. They were also used in parametric amplifiers, providing low noise microwave amplification.

Yes i see yesterday the same version like sir Balunce had, but maybe simulator is wrong like say Balunce

 

[michael1978]

You must use the correct spice varicap model and parameters. I do not know which spice model varicap you are using.

You know the low and high frequency ends of the FM band. The Local Oscillator frequency range needed is offset by the IF frequency. You can calculate or simulate the capacitance needed to maintain oscillation at the ends of the band. Select from manufacturers data an available real varicap that provides the required variation in capacitance. Find or make a spice model of that varicap.

The BBY40 was originally used. I google 'BBY40 spice model' and find;
http://www.gunthard-kraus.de/Spice_Model_CD/Vendor List/Zetex/bby40.lib

* ZETEX BBY40 Spice Model Last revision 18/8/92
.MODEL BBY40 D IS=7.417E-15 N=1.058 RS=.1259 XTI=3
+ EG=1.11 CJO=64.39E-12 M=1.013 VJ=2.566 FC=.5 BV=45.12
+ IBV=.1232 TT=215E-9
*
* + ISR=1.731E-12 NR=2.27 IKF 9.882 (LATER SPICE VERSIONS ONLY)

Each version of spice uses a different way to create and integrate new component models. You must become an expert in your selected version of spice. Take a look at an existing spice varicap model and work out what parameters must be changed to make your BBY40 model.

You may have to change other component values such as the LO tuning inductance and the surrounding capacitors. The original paper with the circuit includes a section on LO tuning and varicap selection, see page 5 and 6 of “Local Oscillator for FM Broadcast Band, 88-108 MHz”, from Lund University, 2012.

Thank you, i have the same model, but maybe simulator don't work, because eveything is fine without varicap, when i connect varicap everything changes the harmonics, whatever i have to do one other
THANKS MAN. greetings

 

[michael1978]

You must use the correct spice varicap model and parameters. I do not know which spice model varicap you are using.

You know the low and high frequency ends of the FM band. The Local Oscillator frequency range needed is offset by the IF frequency. You can calculate or simulate the capacitance needed to maintain oscillation at the ends of the band. Select from manufacturers data an available real varicap that provides the required variation in capacitance. Find or make a spice model of that varicap.

The BBY40 was originally used. I google 'BBY40 spice model' and find;
http://www.gunthard-kraus.de/Spice_Model_CD/Vendor List/Zetex/bby40.lib

* ZETEX BBY40 Spice Model Last revision 18/8/92
.MODEL BBY40 D IS=7.417E-15 N=1.058 RS=.1259 XTI=3
+ EG=1.11 CJO=64.39E-12 M=1.013 VJ=2.566 FC=.5 BV=45.12
+ IBV=.1232 TT=215E-9
*
* + ISR=1.731E-12 NR=2.27 IKF 9.882 (LATER SPICE VERSIONS ONLY)

Each version of spice uses a different way to create and integrate new component models. You must become an expert in your selected version of spice. Take a look at an existing spice varicap model and work out what parameters must be changed to make your BBY40 model.

You may have to change other component values such as the LO tuning inductance and the surrounding capacitors. The original paper with the circuit includes a section on LO tuning and varicap selection, see page 5 and 6 of “Local Oscillator for FM Broadcast Band, 88-108 MHz”, from Lund University, 2012.

Sir you kno what i make it, i remove the filteres and they work? WITHOUT FILTER