Сircuit below oscillates in reality, but not oscillates in LTspice simulation.
How to simulate such kind of circuits in LTspice?



Oscillogram of real circuit:


LTspice simulation:

 

Сircuit below oscillates in reality,

Don't see how.
The simulated transistors both have reverse polarity voltage applied to them.
Post your real circuit schematic.

 

Don't see how.
The simulated transistors both have reverse polarity voltage applied to them.
Post your real circuit schematic.

See pictures:

Right hand transistor Q3 is buffer (full circuit is here: https://forum.allaboutcircuits.com/threads/watervox-or-electrical-double-layer-edl-in-action.197388/post-1867101).

 

what you have on board and what you have in simulation are two different things.
on board you have emitter of PNP transistor connected to +
but in simulation, emitter and collector are swapped on both transistors.


btw. not everything works in simulation.
here is a simple astable multivibrator that definitely works in real life but fails in LTSpice
which is why LTSpice includes its own 'educational' version...
base resistors are purposely mismatched to help start oscillations.
increasing their value some 10x does make the this circuit work as well.

 

here is a simple astable multivibrator that definitely works in real life but fails in LTSpice

That's a common misconception.
Don't panic.
It's not a simulation failure, it's a failure to communicate.
Many who use LTspice don't realize that it normally calculates the circuit DC operating point before the transient analysis.
In this case the circuit can settle into a quasi-stable DC state since there is no natural noise or asymmetries in the circuit.
If you omit the initial DC calculation by using either the startup or UIC option in the transient analysis, the oscillation occurs nicely, even if nothing is mismatched (below):

 

Don't see how.
The simulated transistors both have reverse polarity voltage applied to them.
Post your real circuit schematic.

For wide range of possible R1 value changes, without latching,
β of Q1, Q2 should be as close to 1 as possible.
Therefore Q1 and Q2 used in reverse mode (β=2-3).
See how oscillator works with transistors in normal mode -
one infinite pulse (latching):

on board you have emitter of PNP transistor connected to +

See:

 

@Danko
ooops, my bad... responded in haste and forgot to flip it back for this one.


@crutschow
thank you. i hardly touch it but that .. is a good tip. i guess being squeaky wheel did pay of..

 

Therefore Q1 and Q2 used in reverse mode (β=2-3).

Reverse mode is with the base and emitter interchanged.
You had the NPN and PNP reversed.

 

Reverse mode is with the base and emitter interchanged.

"Reverse-active (or inverse-active or inverted)
By reversing the biasing conditions of the forward-active region,
a bipolar transistor goes into reverse-active mode.
In this mode, the emitter and collector regions switch roles."
https://en.wikipedia.org/wiki/Bipolar_junction_transistor#:~:text=Reverse-active (or inverse-,and collector regions switch roles.

You had the NPN and PNP reversed.

Every transistor is reversed (collector and emitter interchanged).

ADDED:
Nobody answer my question - how to simulate this particular circuit?
Seems reversed mode not detailed in LTspice BJT models...

 

Seems reversed mode not detailed in LTspice BJT models...

LTspice does model BJT reverse mode operation.

I can't help you otherwise, since I still don't really see how that circuit is supposed to work.

 

same here...
starting with output low, C1 is charging and Q1 base potential is increasing.
at some point Q1 and Q2 turn on so the output (red) is high.
but capacitor voltage cannot change instantaneously so this rise means voltage increase on Q1 base as well.
this only helps drive both transistors into same direction which is steady state.
don't see how they will ever turn off... maybe something not obvious is taking place (tunneling?)

 

Сircuit below oscillates in reality, but not oscillates in LTspice simulation.
How to simulate such kind of circuits in LTspice?

View attachment 311056

Oscillogram of real circuit:


LTspice simulation:

Some basic understanding in electronics would help.
You need a bigger RLoad resistor in order to get enough basis voltage for Q2 to get into conduction.
Thats it, then it works fine



HTH Tiwag

 

Some basic understanding in electronics would help.
You need a bigger RLoad resistor in order to get enough basis voltage for Q2 to get into conduction.
Thats it, then it works fine



HTH Tiwag

Here is an optimized version which works more robust

 

Reverse β is set: BR=20 for Q1 and Q2.
Result: good coincidence.

LTspice diagram:


Oscillogram from real circuit:
------

 

We must subscribe to the requirements of Nature or it will not do what we want it to do!

Julius Sumner Miller

So I ask, did the circuit NOT work or did you just fail to understand it?

 

Reverse β is set: BR=20 for Q1 and Q2.
Result: good coincidence.

What is the final SCH and values?

 

What is the final SCH and values?

the original schematic with adjusted Beta-reverse-factor

 

What is the final SCH and values?

Nobody answer my question - how to simulate this particular circuit?

So, values of parts and circuit itself can not be changed, by definition.
Solution:
1. Measured reverse β of transistors Q1 and Q2 (about 20 in this case).
2. In transistor models value BR=3 replaced with measured value BR=20.