开云体育

For the most part you need to add little inductors in series with each
component. There is no parameter or something similar that adds an
inductance everywhere.

Capacitors in LTspice do have an "equivalent series inductance".
(Right-click on the capacitor.) The inductance remains hidden on the
schematic.

For resistors, if you don't mind messing up the schematic a bit, you can
use an inductor to represent a resistor with series inductance, by entering
the resistance value as the "series resistance". Unfortunately the
resistance doesn't show up on the schematic. (Annotate your schematic
well.)

People can go overboard by adding stray inductance and stray capacitance
everywhere possible. You might not want to do that. You probably only
need to add it in a few places. Also, components have two leads, but the
two lead inductors are in series with one another so you only need one
inductor per component, not two.

If all you are trying to do is simulate this circuit to see how it
simulates (and not trying to replicate an actual circuit on the bench),
then one might argue that you do not need to bother at all, with all the
stray inductors. For the most part, the circuit SHOULD work without them.

It is a lot of work for a simple simulation. In my opinion it's a little challenge to receive a good result. So I will test it.

The biggest exception being that silvered wire.

I calculated and added a inductor as an alternative for the wire and it generates a first maximum in the frequency simulation. Maybe one third of the original.

Do you think I used the wrong models or the setup of my circuit is wrong?

Good question! Could be either or both.

This oscillator circuit looks "funny" to me because it lacks an explicit
positive feedback path, so I'm guessing it makes use of characteristics
internal to the transistor. And that is, of course, assuming that the
first transistor really IS the oscillator (which I think it has to be).

Oscillators are sometimes tricky to do in SPICE. Sometimes they work
beautifully; other times, not. There are loads of questions in this forum
about getting an oscillator to work right or work at all in simulation.
This one is tricky also because it is 900 MHz.

Are the two halves also coupled, with a K ?
No they are not. I thought if it is a coil with tap I can separate it
without using this. On the first hand I don't know how to use it. And on
the second I thougt, if it's ideal conducting the K doesn't matter.

You definitely should add the K coupling factor, if there is any coupling.
By leaving it out, it is 0 ... no coupling. That would be OK if L
consists of two coils that are physically separated, or mounted at right
angles to one another.

Add a SPICE directive (far-right icon on the icon bar) that looks something
like this:

K L1 L2 0.8

or some other amount of coupling between 0.0 and 1.0. My guess is that an
air-wound coil with a tap has a fair amount less than ideal coupling.

Andy

I calculated and added a inductor as an alternative for the wire and it
generates a first maximum in the frequency simulation. Maybe one third of
the original.

If adding the inductor there made a difference, then I think you are on the
right track. It probably means the first transistor is now oscillating.

Can you see the oscillation on that transistor, which wasn't there before?

You might calculate the resonant frequency between the inductor and the
varactor diode plus trimmer cap, and see how it compares with what you see
in the simulation.

Andy

Thank you for the instruction for the K factor.

If I have time left, I will try to handle the problem with the transistors. If it works, I will give you a feedback. But I think it is impossible for a amateur like me.

Maybe it works after adding each induction to the components.

Can you see the oscillation on that transistor, which wasn't there before?

Yeah, it gives me now a oscillation at about 1GHz.

Hallo Christian,

On Mon, 29 Jul 2013 17:41:19 -0000, christianvierck wrote:

I calculated and added a inductor as an alternative for the wire and it generates
a first maximum in the frequency simulation. Maybe one third of the original.

If that is the case, it might be that the second stage is meant to be a
tripler.

--
Regards,
Arwin.

In message <kt6alh+9g3j@...>, dated Mon, 29 Jul 2013, christianvierck <christianvierck@...> writes:

Thank you for the instruction for the K factor.

Since the tap only feeds the antenna, I suggest you forget the tap and just put a single inductor there.

If I have time left, I will try to handle the problem with the transistors. If it works, I will give you a feedback. But I think it is impossible for a amateur like me.

I don't understand how you can be an amateur if you have a professor.

Maybe it works after adding each induction to the components.

The circuit does require quite a lot of knowledge about UHF techniques, so your professor has set you a hard task. The first transistor is an emitter follower, and at UHF emitter followers have negative input resistance. The varactor (BB105), trimmer and the silver wire form a series tuned circuit, and the negative input resistance is supposed to cancel the circuit resistance so that the device oscillates. Good luck getting that to work in simulation! You need a very good model of the transistor.
--
OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk
Why is the stapler always empty just when you want it?

John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK

Since the tap only feeds the antenna, I suggest you forget the tap and
just put a single inductor there.

I think it doesn't change something on the frequency. But it could be the easier way.

I don't understand how you can be an amateur if you have a professor.

I mean I am a amateur using LTSpice. Because I only startet working with it a few days ago.

Good luck
getting that to work in simulation! You need a very good model of the
transistor.

I hope, I will find a solution.

Thank you.

In message <kt6efj+urt6@...>, dated Mon, 29 Jul 2013, christianvierck <christianvierck@...> writes:

Good luck
getting that to work in simulation! You need a very good model of the
transistor.

I guess you have that. See below.

I hope, I will find a solution.

In your previous post, you said it was oscillating at 1 GHz. To get the thing oscillating at all is good, but to get within 11% of the design frequency is very good.
--
OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk
Why is the stapler always empty just when you want it?

John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK

I guess you have that. See below.

Sorry, do you mean the model of the BB105
.model BB105 D(Is=.1p Rs=1 Bv=35 Ibv=10u Cjo=35p Vj=.75 M=.8)

or the model I use for the BRF92.
Here I have to trust the designers. ;)

In your previous post, you said it was oscillating at 1 GHz. To get the
thing oscillating at all is good, but to get within 11% of the design
frequency is very good.

Thanks for supporting. I am pleased with my work for today.



This is the result with the oscilatting transistor(blue) and the frequency at the antenna(yellow). No I have to find out, how I get the frequency of 900MHz on the antenna.
Inductions and the K factor are missing.

In message <kt6gov+l9n9@...>, dated Mon, 29 Jul 2013, christianvierck <christianvierck@...> writes:

Sorry, do you mean the model of the BB105
.model BB105 D(Is=.1p Rs=1 Bv=35 Ibv=10u Cjo=35p Vj=.75 M=.8)

or the model I use for the BRF92.
Here I have to trust the designers. ;)

Yes, I meant the BFR92. A model that was no so good probably wouldn't show the negative input resistance or would over-egg it, so that your oscillator would 'squeg' (OK, since you got good results today, you can research the meaning of that!).
--
OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk
Why is the stapler always empty just when you want it?

John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK

--- In LTspice@..., John Woodgate <jmw@...> wrote:

In message <kt5rjr+q9qr@...>, dated Mon, 29 Jul 2013, Helmut
<helmutsennewald@...> writes:

Be aware that all the components have inductance of 0.5nH to 1nH per mm
of wire length.

Specifically, that silver wire is an *inductor* and needs to be modelled
as such. You can find formulas for the inductance of a wire of specified
dimensions on the Internet.
--
OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk
Why is the stapler always empty just when you want it?

John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK

People (especially radio amateurs) get very hung up on using silver plated wire for inductors. Anyone with an iota of curiosity (read: diligence) can quickly establish that the conductivity and skin depth advantages of silver over copper are less than 6%. Given that the Q of an inductor is influenced far more by geometry, that is where to focus.

At 900MHz, the circuit should be modelled with most of the parasitics of components included, but frankly the circuit is such a bag of worms that it's probably not worth the effort. It was probably published after having been built once. Horrid. Yes, one of the major issues with this design is that in practice, the antenna matching will affect the frequency of the oscillator because there is little isolation, as the input impedance of the 2nd stage defines the output load of the oscillator stage. The tapped inductor in the amplifier output is intended to be an autotransformer, i.e. K>0, otherwise it wouldn't have been drawn thus.

I think the professor is just having fun with his students, although there an alternative interpretation.

It is definitely possible to use LTspice for RF simulation, even though it is not the ideal tool, because it doesn't really handle S parameters and transmission line structures natively. It requires quite a lot of additional work to fill in the gaps. Nevertheless, it is free and otherwise unrestricted. For oscillators and other non-linear RF circuits, however, it is about two orders of magnitude slower than harmonic balance simulators. That may or may not be important to you, possibly depending on whether you are being paid for what you do.

Regards,
Tony

It looks like you were doing an .AC analysis. You should be using a .TRAN
(transient) analysis.

I hate to say it, but the .AC analysis doesn't really show you anything in
this case.

Andy

A couple of other points:

The antenna load doesn't do anything. If you want it to be there, connect
the right end of that resistor to an AC ground (ground it through a
capacitor).

It looks like your power supply voltage, V1, is not set to any DC voltage.
Its AC value should be 0. Its DC value should be 6.

Andy

Hello CV,
Sorry for missing the question about the varactor. Maybe this willhelp to build the model:


BB105 equivalent should be MV2105:


Hope this helps

ME

It looks like you were doing an .AC analysis. You should be using a .TRAN
(transient) analysis.

Relating to the frequency in the circuit, I have to do an AC analysis. But I understand, that I have to use the .TRAN to simulate the oscillation.

The antenna load doesn't do anything. If you want it to be there, connect
the right end of that resistor to an AC ground (ground it through a
capacitor).

I thought it was right to simulate it with a single resistor, because the only thing I knew about antennas was that they are oscillating circuit. So I removed the imaginary content and only the resistor was left. I will improve it as you told me.

It looks like your power supply voltage, V1, is not set to any DC voltage.
Its AC value should be 0. Its DC value should be 6.

I know it, because the schematic told me it is a DC voltage. But I had to change it due to the AC analysis for the frequency.

People (especially radio amateurs) get very hung up on using silver plated wire for inductors. Anyone with an >iota of curiosity (read: diligence) can quickly establish that the conductivity and skin depth advantages of >silver over copper are less than 6%. Given that the Q of an inductor is influenced far more by geometry, that is >where to focus.

It sounds like I have to focus on the silver wire in the first case to get a presentable result.

I think the professor is just having fun with his students, although there an alternative interpretation.
That may or may not be important to you, possibly depending on whether you are being paid for what you do.

I can't give a feedback to this point. But it is very hard to discover how to get a result with such a circuit and null skills.

Oh thanks a lot. I will try MV2105 first and try to build an own model with your link afterwards.

--- In LTspice@..., "christianvierck" <christianvierck@...> wrote:

Oh thanks a lot. I will try MV2105 first and try to build an
own model with your link afterwards.

Hello,

The MV2105 is too different from the BB105. You should search for
a datasheet of the BB105.

Best regards,
Helmut

The MV2105 is too different from the BB105. You should search for
a datasheet of the BB105.

Okay thank you. I have found one.


I have searched on a website which sells devices linked with datasheets and didn't found a hint. After realising that this device is not manufactured for some time, using a serach-engine was a easy step. Now trying to get a representing model.