Astable multivibrator simulation-floating nodes problem spice

Thread Starter

Baydith

Joined Jan 17, 2012
4
Hey, during our lab we had to solder a simple astable multivibrator, but the supervisor gave us such resistor values that nothing was visible on the oscilloscope. Therefore, I want to make a simulation of multivibrator circuit in PSPICE, but strangely, I have problems with floating nodes. I have NEVER had such problems with PSPICE and I have used it several times to simulate OP-AMPS circuits, etc.I have tried adding a resistor of high value to the ground node, but still the same problem. I have carefully attached all wires, ensuring there is no problem with doubled wiring and/or unconnected nodes.

I'm posting the screen as well as the .sch file...

Any help ?
 

Attachments

t_n_k

Joined Mar 6, 2009
5,447
I don't use PSPICE. But I would think (at least) V1 should be a fixed DC source rather than a waveform generator. Perhaps you also need to set initial conditions for the capacitor voltages. What analysis mode are you using - transient?
 

Thread Starter

Baydith

Joined Jan 17, 2012
4
Yep, transient. Well, u're right, since it's an astable multivibrator I don't need pulse source, since it's spontanously switches off and on the transistors...But I don't think it's such a problem, I think that may be the problem is with wiring, but I tried doing it all over again, ensuring the wiring is ok and it still sucks...As for the initial charge on capcitors, yep, it may be true, but I still should be able to run the simulation, just that the traces would be off...
 

crutschow

Joined Mar 14, 2008
23,538
The Error message says Node GND is floating. Thus, for some reason, the simulator thinks your ground symbol is not actually connected to your circuit or it is an incorrect symbol. That is likely causing the other floating error messages.

Try deleting and reconnecting the ground.
 
For what it's worth, I've had a lot of trouble getting oscillator circuits to simulate properly using Mentor Graphics tools. I've tried all the suggestions on kick starting it, but I've found its usually not even worth my time.
 

Thread Starter

Baydith

Joined Jan 17, 2012
4
I replaced the transistor model with a different one, of similar properties and now it's all working. Guess the library file of 2N3904 was messed, anyway, thanks for help! /close
 

Adjuster

Joined Dec 26, 2010
2,148
For what it's worth, I've had a lot of trouble getting oscillator circuits to simulate properly using Mentor Graphics tools. I've tried all the suggestions on kick starting it, but I've found its usually not even worth my time.
It is well known that oscillators can be difficult to start in simulations, but I've done it many times, as have many other people, some of whom use this site and have posted examples. I would say it really boils down to a few main subject headings:

  1. Like any other simulation model, the circuit must not contain some mistake that simply stops it working. This is by no means a given.
  2. The DC working point simulation that is the usual starting point for Spice (etc.) transient analysis does not always give a result favourable for oscillator circuits to start. In certain cases, difficulty in getting the simulation to oscillate for this reason may give a clue that real-world starting may not be reliable, particularly if power is applied very slowly. Sometimes this indicates a problem with biasing. A loop gain analysis of the circuit treated as an amplifier may show whether conditions for oscillation to start are present.
  3. Simulations may not supply enough of the randomness (noise) found in real life to start oscillations. An artificial signal source may be required to provide some disturbance
  4. This problem in simulation may sometimes be resolved by skipping the initial bias point analysis, or by setting one or more initial conditions (such as a capacitor voltage), or possibly by providing a pulse to start the oscillator after power-up.
  5. In the real world, the oscillator may need to be changed so that it naturally powers up with good loop gain, or alternatively a deliberate starting "kick" may be applied on every power-up. Personally, I am however not very enthusiastic about circuits which require this, partly because I suspect that some may be subject to non-recoverable stalling due e.g. to a glitch.
That's not the whole story, but I felt the need to explain because I feel that the OP may be helped by having a more considered view.
In my opinion, the statement that it is not worth simulating oscillators is a considerable exaggeration.

I enclose a few examples of oscillating LTSpice circuits.
 

Attachments

Last edited:
In my opinion, the statement that it is not worth simulating oscillators is a considerable exaggeration.
Haha yeah, true. I should have qualified that with, 'for my situation'

I appreciate the insight. Very interesting and helpful post!
 

crutschow

Joined Mar 14, 2008
23,538
I agree with Adjuster's post. If you can't get an oscillator to oscillate in a simulator after using his suggestions, then the oscillator circuit likely has a problem or error. It's usually not a problem with the simulator.
 
Top