开云体育

It may be that the OP simply wants to determine what that current is (compute it). If that is the case, just run the simulation. When it is done, move the cursor over (almost) any component and you will be shown a graph of the current through that component. It is really easy.


You do, however, need to be aware that there is assumed to be a "positive" current direction. With some components, such as resistors, are difficult to tell which is the "right" way. If you had to rotate the component and rotated it the wrong way, you might end up with a displayed current that is the negative of the real current.


Jim Wagner
Oregon Research Electronics

Is anyboby here who can explain me how to calculate Ib in this circuit :
Draft2.asc.
I found no formula(s) on the web while LTSpice knows.

LTspice takes the "brute force" approach. It has all the network equations
for the entire circuit, and it solves for every branch current, using
iteration. That is, in effect, it makes a guess, then it evaluates it
against the network equations, then makes another guess (not a wild guess
but based on what the network equations say), evaluates again, and so on.
After some number of these tries, it concludes it is very close to the
"right" answer, and that's what it shows you. To be a "right" answer, the
voltages and currents must be consistent with the network equations. When
everything satisfies the network equations within certain tolerances,
that's when it stops the iteration routine, and shows you the answer.

Andy

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.

No, they MAY be resonant circuits but, being passive, they cannot be
oscillating circuits.

I think maybe he meant to write "the only thing I knew about antennas was
that they are resonant circuit."

If the circuit really is oscillating, the output voltage will go crazy

as the added generator sweeps through the oscillating frequency.

In an AC analysis, the oscillator will NOT be oscillating. AC analysis
finds the DC operating point, then linearizes all nonlinear devices
(transistors and diodes) at that point. Then it looks at your circuit as a
fully passive network and see how much of the applied AC propagates through
the circuit.

In a TRANsient analysis, if you also applied a small sine-wave signal and
swept its frequency, you may or may not see interaction between the applied
signal and the oscillator's own frequency. Chances are the applied signal
would "pull" (or is it "push"?) the oscillator and force it to lock up with
the applied signal.

Andy

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

I'm trying to work hierarchically, so I created a low level schematic (myblock.asc), created a symbol (myblock.asy) for that schematic, and saved both of them at C:&#92;Program Files&#92;LTC&#92;...&#92;lib&#92;sym to be able to access the symbol when bringing components.
However, when I place that symbol in top level schematic, I get an error of missing schematic(s) of the hierarchy. If I save the top level schematic at the same folder as the low level, i.e. at e C:&#92;Program Files&#92;LTC&#92;...&#92;lib&#92;sym, there is no error and everything works fine.

However, I'd like to save my top level schematic at another folder, so I probably need to point LTSPICE to low level schematic location... I tried to place a SPICE directive ".include C:&#92;Program Files&#92;LTC&#92;...&#92;lib&#92;sym&#92;myblock.asc", however, it didn't work.

Please advise
Thanks a lot

Hello,

You have to save the symbol and the schematic in the folder
of your top-level schematic.

Now here comes what you missed.
You can add a symbol from the folder of your top-level schematic.
Therefore open the "Select component" dialog. Then change the
folder in "Top Directory" to your schematic folder. Now you see
all the components(.asy) in your top-level directory.

Best regards,
Helmut

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.

Why do you say you have to do an AC analysis?

An AC analysis tells you nothing about what the oscillator is doing. It
won't tell you the frequency where it oscillates. It won't tell you even
IF it is oscillating. You MUST use a .TRANsient analysis to check for (a)
whether it oscillates, and (b) at what frequency.

The antenna load doesn't do anything.
...


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.

That's correct to use the resistor. At the antenna's resonant frequency,
the antenna looks like a resistor, to ground. (A quarter-wave antenna over
a ground plane probably looks like about 35 ohms, BTW.)

However, a resistor with the other end floating, or shorted across the
resistor, is just an open circuit (i.e., no load) because zero current
flows to it.

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.

This doesn't make sense. What you have is a 0V power supply with about 6V
of AC ripple. I can't figure out why you would want to do that, nor what
you would get from your AC analysis. Effectively, your AC analysis shows
you how much the AC ripple on the power supply feeds through to the output.
Also, with 0V DC applied, the transistors are non-functional.

I can't emphasize enough that you really need to be doing a TRANsient
analysis. I think you don't understand yet the purpose of an AC analysis.

Regards,
Andy

I'm trying to work hierarchically, so I created a low level schematic (myblock.asc), created a symbol (myblock.asy) for that schematic, and saved both of them at C:&#92;Program Files&#92;LTC&#92;...&#92;lib&#92;sym to be able to access the symbol when bringing components.
However, when I place that symbol in top level schematic, I get an error of missing schematic(s) of the hierarchy. If I save the top level schematic at the same folder as the low level, i.e. at e C:&#92;Program Files&#92;LTC&#92;...&#92;lib&#92;sym, there is no error and everything works fine.

However, I'd like to save my top level schematic at another folder, so I probably need to point LTSPICE to low level schematic location... I tried to place a SPICE directive ".include C:&#92;Program Files&#92;LTC&#92;...&#92;lib&#92;sym&#92;myblock.asc", however, it didn't work.

Please advise
Thanks a lot

--- In LTspice@..., legg@... wrote:

Given a plot of a pink or white noise voltage, and a synchronized plot of the current induced in a partially reactive load -

Will the 'normalized' ratio of the FFT plots be an indication of Z?

I'm looking at the low frequency end of the FFT, to avoid sampling issues. By normalized, I mean that 1 volt would produce 1 amp with both plots resolving to 0dB at the minimum sampled frequency (the load being partially inductive in this example).

It seems much too simple......

RL

Hello RL,

It will only work when you filter the FFT-output, but the
the FFT-results can't be filtered in LTspice. Thus you have
to export the FFT-data and process them in an external program.
This method only work with a linear system and it's precision
may be somewhat limited due to group delay variation.

Best regards,
Helmut

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

I can't tell you how much I love LtSpice, or how much I have LEARNED about electronics in general since using LtSpice. I am shopping for a new laptop running full-blown Windows, not a tablet running Windows-8-RT. Does LtSpice support touch screen gestures such as pinch/expand or finger swipes to move the schematic / plot window around?

Even without touchscreen gesture support, LtSpice has the best user experience of any free Spice-simulator/schematic-capture/data-plotting tool that I have ever used.

Thank you from the bottom of my heart to Mike Englehardt, Helmut, Linear Technologies, the usergroup, and anybody else I forgot for this great FREE product and user experience!

Hutchtronix

Hello,

Unfortunately I don't have a PC with a touch-screen.
I would be happy if somebody having a PC with touch screen
will answer this question.

Best regards,
Helmut

Moderator

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

I'm connecting diodes to relays and the diode symbol is
almost as large as the entire relay symbol. The appearance
of the combination and how the connections are made is very
awkward looking.

Hello Diane,

If you think THE relay symbol looks to small, you could redraw
the original symbol with the symbol editor. I recommend to use
another filename in this case, e.g. originalname_big.asy.

Best regards,
Helmut

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

Hi
Is anybody here who can explain me how to calculate Ib in
this circuit : Draft2.asc.
I found no formula(s) on the web while LTSpice knows.
Thanks.

Hello,

Let's assume an ideal transistor with base resistance Rb=0,
current gain B=BF=constant, Early voltage VAF=infinity and
the ideality factor NF=1.

Ib = (Is/B)*exp(Vbe/(NF*VT)

VT = k*T/q

k=Boltzmann constant
T = absolute temperature
q = electron charge

The default temperature in SPICE is 27 degree C.
This gives VT=25.8641mV.

If there is some Rb, e.g. 10Ohm, you can take is into account.
Vbe = Vbe_extern - Ib*Rb
Be aware that the current gain is a function of Ic and Vce too
if more parameters are set in the SPICE model.

I have uploaded an example using the basic equation.

Fies > Temp > ib_transistor.asc

Best regards,
Helmut

In message <kt8hbj+5vsb@...>, dated Tue, 30 Jul 2013, jean_claudeabeille <jean_claudeabeille@...> writes:

Is anyboby here who can explain me how to calculate Ib in this circuit : Draft2.asc. I found no formula(s) on the web while LTSpice knows. Thanks.

You can't find a formula on the Web, even though there is one, because it's not a practical thing. The base current is exponentially dependent on the base voltage and the junction temperature. LTspice assumes values in the exponential equation, but the slightest change can make a huge difference to the current. Every individual transistor will give a different result.

You simply don't use bipolar transistors with a fixed DC voltage between base and emitter.
--
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

Hi
Is anyboby here who can explain me how to calculate Ib in this circuit : Draft2.asc.
I found no formula(s) on the web while LTSpice knows.
Thanks.

If the circuit really is oscillating, the output voltage will go crazy
as the added generator sweeps through the oscillating frequency.

I don't know what I awaited, but I see a clear maximum. And it gets closer to 900MHz. Nice.

I simulated it with .TRAN and it worked well. The simulation through the first transisitor was congruant to the oscillation at the antenna.

In message <kt7o77+jld6@...>, dated Tue, 30 Jul 2013, christianvierck <christianvierck@...> writes:

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.

No, they MAY be resonant circuits but, being passive, they cannot be oscillating circuits.

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.

No, the SUPPLY voltage is always DC. For AC analysis, normally the INPUT voltage would be AC, but in this case the only input voltage you have is from the microphone, which doesn't help much to find out if the UHF part of the circuit is working. If the first stage is indeed oscillating, it provides its own input voltage in practice, but for simulating an AC sweep you need to add a generator somewhere in the UHF circuit, and in series between the 1 - 4 pF trimmer and earth looks a good place. I suggest you set the sine wave signal to 50 mV initially and sweep from 300 MHz to 3 GHz. Look at the output voltage at the collector of the second transistor.

If the circuit really is oscillating, the output voltage will go crazy as the added generator sweeps through the oscillating frequency.
--
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

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.

--- 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

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

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.

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.

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