Maker Pro
Maker Pro

Astable multivibrator circuit making me astable

wingnut

Aug 9, 2012
259
Joined
Aug 9, 2012
Messages
259
Hi all

I was playing with the circuit below today. I found out that if the transistor is reversed so that if one puts the c where the e should be, the circuit still works but at a lower frequency. Attached below is a diagram of what I mean. This surprises me because this means current is flowing in the reverse direction to the normal NPN transistor functioning, in this case from from e to c. Could you please tell me if this is so or not. I do understand how the normal astable multivibrator circuit works

The Astable Multivibrator Circuit Diagram

An astable multivibrator circuit diagram with 2 LEDs
Thank you.
 

Attachments

  • Screenshot 2022-07-20 at 13.43.57.png
    Screenshot 2022-07-20 at 13.43.57.png
    251.1 KB · Views: 0

Alec_t

Jul 7, 2015
3,248
Joined
Jul 7, 2015
Messages
3,248
Most NPN transistors will work if the C and E connections are reversed, but the current gain differs for the two directions.
 

crutschow

May 7, 2021
520
Joined
May 7, 2021
Messages
520
Below is an LTspice simulation showing the characteristic curves of the same NPN transistor operating in both the normal and inverted mode:
Note that Q2 still operates as a transistor when inverted, but the gain is very low with a Beta of about 3, versus over 130 for the normal connection.
One interesting observation is that the Vce saturation voltage is much lower for the inverted mode, so for certain applications the transistor can be operated inverted if the minimum saturation voltage is needed.

upload_2022-7-20_10-16-31.png
 

roughshawd

Jul 13, 2020
255
Joined
Jul 13, 2020
Messages
255
Physicists and Inventors have argued about this for a long long time. Inventors worked out the numbers, but the phycisists built the device. The fact is that if you don't know that the amount of draw that circuit has running through it, then any device that can do the job will. (complete nonsense for the whimsical) Well, the truth is that the designers only want something that will work and not readily fail. When there is no draw, power stops, basically a thumbs up for POLR hacks like me!! Remember that you didn't hear this from me or here.... Proper resistance stops motor function!!!
You want to be real careful about what you say next... because any changes, at all, to the circuit, changes everything else that's connected to it.
 

wingnut

Aug 9, 2012
259
Joined
Aug 9, 2012
Messages
259
Below is an LTspice simulation showing the characteristic curves of the same NPN transistor operating in both the normal and inverted mode:
Note that Q2 still operates as a transistor when inverted, but the gain is very low with a Beta of about 3, versus over 130 for the normal connection.
One interesting observation is that the Vce saturation voltage is much lower for the inverted mode, so for certain applications the transistor can be operated inverted if the minimum saturation voltage is needed.

View attachment 55668
I went to https://www.falstad.com/circuit/index.html and went to the astable multivibrator circuit and reversed the e and the c of both transistors, and the Falstad simulation gets it completely wrong. Their circuit does not act as a astable multivibrator, but shows a steady current through both transistors. I have looked on Youtube at setting up LT Spice, and it's quite frightening unless one is 18 years old and planning a career in electronics.
 

crutschow

May 7, 2021
520
Joined
May 7, 2021
Messages
520
the Falstad simulation gets it completely wrong.
Falstad simulator may not properly model reverse operation of a bipolar transistor.
I have looked on Youtube at setting up LT Spice, and it's quite frightening unless one is 18 years old and planning a career in electronics.
Yes, LTspice does have a somewhat steep learning curve but there are many sample circuits and tutorials to help with that.
You don't have to have a career in electronics, just a hobby interest, to find a good simulator useful in determining how a circuit is likely to work before you build it.
Not sure what being 18 years old has to do with that. :confused:
 

wingnut

Aug 9, 2012
259
Joined
Aug 9, 2012
Messages
259
Falstad simulator may not properly model reverse operation of a bipolar transistor.
Yes, LTspice does have a somewhat steep learning curve but there are many sample circuits and tutorials to help with that.
You don't have to have a career in electronics, just a hobby interest, to find a good simulator useful in determining how a circuit is likely to work before you build it.
Not sure what being 18 years old has to do with that. :confused:
I took the plunge and installed LT Spice. As you said, there are good tutorials. I followed one on Youtube. The reference to being 18 was that the mastering of LT Spice may take some time. I may tomorrow try the astable multivibrator circuit on LT Spice with e and c reversed and see if it vibrates. Thanks for the reply.
 

wingnut

Aug 9, 2012
259
Joined
Aug 9, 2012
Messages
259
If it doesn't, post the .asc LTspice file and I'll take a look at it.
I created the circuit on LT Spice and attached the .asc file below. The capacitors are supposed to be 1uF each and I did not know how to make the transistors 2n222's. The .tran analysis showed a vibration of some sort but it did not look regular. Would you mind seeing if the circuit is acting as an astable multivibrator with the e and c in this configuration. Thanks.
 

Attachments

  • sAstableMultivib1.asc
    1.3 KB · Views: 1
Last edited:

crutschow

May 7, 2021
520
Joined
May 7, 2021
Messages
520
First rule of Spice. All Spice simulation circuits need a ground connection, so I added that.
Also you had D2 in the wrong place.
Note that you can use standard prefixes such as u, p, m, k, meg (not M), etc. for part values.
And the circuit takes a few ms to start, so I extended the run time to 50ms.
If you right-click on the transistor symbol, you can select the transistor you want.
upload_2022-7-22_7-54-49.png

Modified circuit simulation below:
It does oscillate, but with a crappy waveform.
Orientating the transistors correctly and increasing the values of R2 and R3 will improve that.

upload_2022-7-22_8-12-19.png
 
Last edited:

Alec_t

Jul 7, 2015
3,248
Joined
Jul 7, 2015
Messages
3,248
A completely symmetrical circuit, as in the case of a classic multivibrator, can confuse LTspice sometimes, and it helps if slight asymmetry is introduced so that oscillations can get started. Alternatively, the .uic directive can be used to specify a starting voltage/current for a particular node.
 

wingnut

Aug 9, 2012
259
Joined
Aug 9, 2012
Messages
259
First rule of Spice. All Spice simulation circuits need a ground connection, so I added that.
Also you had D2 in the wrong place.
Note that you can use standard prefixes such as u, p, m, k, meg (not M), etc. for part values.
And the circuit takes a few ms to start, so I extended the run time to 50ms.
If you right-click on the transistor symbol, you can select the transistor you want.


Modified circuit simulation below:
It does oscillate, but with a crappy waveform.
Orientating the transistors correctly and increasing the values of R2 and R3 will improve that.
Crutschow, thank you so much for the help. I tried for hours today but it would not work properly, presumably without the ground. The simulator kept working in 1us steps which I was unable to change but its all working fine now. Except, with the transistors the right way I don't get a vibration. If you have the time I would greatly appreciate you telling me why the correct circuit below will not vibrate. Thanks again.
 

Attachments

  • sAstableMultivib4.asc
    1.7 KB · Views: 2

crutschow

May 7, 2021
520
Joined
May 7, 2021
Messages
520
Except, with the transistors the right way I don't get a vibration.
Increase the value of R2 and R3 as I suggested (below):
With the low resistor values and the higher gain of the normally oriented transistors, both transistors just tend to stay fully on.
The oscillation frequency is lower, so you also have to increase the simulation time.

You can also be able to get it to oscillate if you follow Alec_t's suggestions in post #13.

upload_2022-7-22_9-38-19.png

upload_2022-7-22_9-53-45.png
 
Last edited:

wingnut

Aug 9, 2012
259
Joined
Aug 9, 2012
Messages
259
Increase the value of R2 and R3 as I suggested (below):
With the low resistor values and the higher gain of the normally oriented transistors, both transistors just tend to stay fully on.
The oscillation frequency is lower, so you also have to increase the simulation time.

You can also be able to get it to oscillate if you follow Alec_t's suggestions in post #13.

It's working. I can't thank you enough. It took me 20 minutes and watching a Youtube video just to find where LT Spice hid the common ground. In the same manner it took me most of the day trying to figure out LT Spice. Thank you that the day was worthwhile in that the simulation now works and I learned something in the end.
 

wingnut

Aug 9, 2012
259
Joined
Aug 9, 2012
Messages
259
A completely symmetrical circuit, as in the case of a classic multivibrator, can confuse LTspice sometimes, and it helps if slight asymmetry is introduced so that oscillations can get started. Alternatively, the .uic directive can be used to specify a starting voltage/current for a particular node.
Thank you so much for the help.
 

crutschow

May 7, 2021
520
Joined
May 7, 2021
Messages
520
It took me 20 minutes and watching a Youtube video just to find where LT Spice hid the common ground.
Some tips:
If you look at the Edit drop-down menu you will see the key shortcuts for common components, such as "G" for ground, "R" for resistor, "C" for capacitor, etc., and common commands such as F3 for Draw Wire, F4 for Label Net, etc. which save a lot of time when generating a schematic.

Note that labeling circuit (net) nodes (F4) should be done for all node voltages that you want to plot (especially input and outputs), so that you can readily see what is being plotted.
The node name can be any word or character that you want to use.
Also you can have a node symbol as Input, Output, or Bidirectional if desired.
Otherwise you get default hidden plot node names like n004 which tells you nothing about where on the schematic n004 is.
 

wingnut

Aug 9, 2012
259
Joined
Aug 9, 2012
Messages
259
I am hoping that you who have experience with LT Spice can help this newbie to LT Spice. I am trying to create a potentiometer circuit. Attached are two what look identical circuits, the top one of which does not work, the bottom one does. To me they look identical but not to Spice.

I get "Syntax error in .STEP command.
Expected sweep last value of source 'r1'"

Thank you.

upload_2022-8-1_5-59-15.png
 

Attachments

  • MyPotWorks.asc
    538 bytes · Views: 0
Last edited:

crutschow

May 7, 2021
520
Joined
May 7, 2021
Messages
520
Apparently LTspice does not like potmax/10 as part of the .step command.

If you want a 3-terminal potentiometer model, I can download the one I have.
 
Top