Astable Multivibrator VBE spike Question/Problem

Thread Starter

Bserar79

Joined Oct 24, 2018
17
Hello guys!

I'm quite ashamed to start my first post here with a question, but this project is grinding my wheels for quite a few days now, and i have reached a dead stop.

So, the problem is with this astable (which you can find all over the internet explained in millions of ways, but nowhere do they say about the huge negative VBE voltage which will break the transistor in the long run). Anyway, making some final checks to this project today i noticed this huge negative VBE, researched on the internet and found how to protect the transistors with the commutation diodes. Placed the diodes, made some adjustments to the capacitors, and everything is working, apart from one thing:

When the transistors switch on, there is a huge spike in the VBE (at about 1V, i'll upload a picture with the simulation). This produces a collector current of about 300mA and this is a problem, as the transistors's maximum Ic is 100mA. Even worse, the power dissipation on that spike is something like 2W, way above the 250mW maximum rating for the transistor.

So, the questions are:
1)Is it ok to leave the circuit like this, with the huge spike? (asking this as is a very short pulse which i think will not really affect the transistor in the long run)
2)If it's not ok, what could i do to solve this?

Thank you all in advance, i already spent too much time on something so simple...

Untitled1.png Untitled2.png Untitled3.png
 

crutschow

Joined Mar 14, 2008
28,207
Those current spikes are so short that it's unlikely they will hurt the transistor.

Alternately, a way to reduce the spikes is to put D1 and D2 in series with each transistor base instead of from base to ground.
This will still protect the base-emitter junction from excessive reverse bias voltage.
This assumes that the current spikes are due to the rapid discharge of the capacitors through D1 and D2.
The side effect, is that the oscillation frequency will be reduced.
 

Thread Starter

Bserar79

Joined Oct 24, 2018
17
Thank you very much crutschow! I just tried putting the diodes in series with each transistor base and it worked! Unfortunately, i have to make the frequency adjustable, 80-400Hz. The top 10 ohm resistors are normaly pots, but in the rage of not getting the circuit to work i replaced them with resistors :). Guess i'm gonna stick with the diodes from ground to base, hoping the real thing does not put out smoke when i'll present the project :).

Thank you very much, again!
 

Thread Starter

Bserar79

Joined Oct 24, 2018
17
I tried to do that, but maybe my knowledge about the multivibrator is still lacking, or not really sure. I changed R20 and R21 to 200k, and the capacitors at 33n. This indeed gives me about 90 Hz (which is an okey margin). Now, by decreasing R20 and R21 to 150k, i would assume the capacitors are going to charge faster, thus increasing the frequency, but when i simulate it, this is what happens:

Untitled6.png Untitled7.png
 

ebp

Joined Feb 8, 2018
2,332
You need to show us about a tenth of the time interval you are showing so it is possible to resolve some semblance of detail.

You could try about 200 ohms between the clamped base and the "other side" (e.g. between D1 cathode & left side of C2 & equiv other way). It will change the timing somewhat.
 

danadak

Joined Mar 10, 2018
4,057
The 1N4148's are pretty fast diodes, so that spike makes me think
you have excessive lead length between diode junction and EB junction
of transistor. Basically layout issues introducing a lot of L. If you expand
scope trace on Vbe breakdown what does it look like ?

I part company with crutschow on leaving the design with repetitive breakdown
of the transistor, especially since we do not know what current level is occuring
in that junction under breakdown. Its well known Vbe breakdown introduces some
significant and permanent issues in Bipolars.

http://downloads.hindawi.com/journals/apec/2001/053209.pdf


Regards, Dana.
 

crutschow

Joined Mar 14, 2008
28,207
I part company with crutschow on leaving the design with repetitive breakdown of the transistor,
That's not what I proposed,
I said to put the diodes in series with the base to prevent reverse breakdown.

Below is my LTspice simulation:
The transistor current spikes are now only a few mA.
The frequency is 52Hz for a value of 50k for R3-R6, and 445Hz for a value of 8k.

upload_2018-10-24_16-39-3.png
 

Thread Starter

Bserar79

Joined Oct 24, 2018
17
Wow, thank you! Wasn't expecting so much help. I'll try to answer to everything. Ebp, here is a simulation for the first 20 ms (maximum step size of 0.0000001)

Untitled8.png

I also tried the clamped 200 ohm resistors, here are the first 20ms:
Untitled9.png

Now, danadak, i don't even know what to say. I didn't even know that orcad has inductance and so on for its standard models. i can zoom on the vbe breakdown, here you go (hope i got what you asked for):
Untitled10.png

So, you are suggesting that i completly remove the protection diodes, and just have on the base -8.4 volts? (that's about how much is the negative bias in this circuit). Will it work long enough for the presentation?

Also thank you all so much, you are just great!
 

danadak

Joined Mar 10, 2018
4,057
I may have to withdraw my comment about Vbe breakdown, was not
paying attention to the scale on what I thought was scope shot, as I now
see its spice plot. And scale shows its only 1 V. But until that region/spike
is expanded we will not know what the - pk value actually is. Scope would
have to be pretty fast to do that.

But my bet is on the 1N4148s did do their job and clamped Vbe reverse
before breakdown occurred.

My apologies to all. I will go back to peeling potatoes where apparently I
still have some talent left :)

By the way what would put this inquiry to bed would be a scope shot of
the base junction with a low C probe. Again though I think the 4148's are
going to do their job, in either configuration.


Regards, Dana.
 
Last edited:

Thread Starter

Bserar79

Joined Oct 24, 2018
17
Wow, crutschow, i am shocked of how easily you goi it going. I tried jump starting the oscilator with vpulse from orcad library (i hope i set it up just like you did), with the same values for the resistors (50k, 8 k), and even so, here's what i got:

Untitled11.png

Any idea why? I hoped i won't apear so dumb around here, but it looks like i'm completly stupid.
 

Thread Starter

Bserar79

Joined Oct 24, 2018
17
Jesus i'm so sorry, i was trying the jump start with a voltage source... Crutschow (and all of you, who helped) are incredible. I owe some beers . Thank you so so so much.

Edit: I know that in reality the circuit will start oscilating because of the small differences in the components values, but just to be on the safe side, should i place something like a potentiometer somewhere on the circuit so i can help it start in real life? Or is it jus not necessary?
 
Last edited:

crutschow

Joined Mar 14, 2008
28,207
i was trying the jump start with a voltage source..
Yes, you need to use a high-impedance source (such as a current-source) for the jump start, as a voltage-source is an AC and DC short to ground for any signals at that node.
just to be on the safe side, should i place something like a potentiometer somewhere on the circuit so i can help it start in real life? Or is it jus not necessary?
I think the real circuit will start up reliably when the power is applied and shouldn't need any extra help.
 
Last edited:

Thread Starter

Bserar79

Joined Oct 24, 2018
17
Yes, you need to use a high-impedance source (such as a current-source) for the jump start, as a voltage-source is an AC and DC short to ground for any signals at that node.
Yep, i realized it eventually, such a dumb mistake. Though i'm still puzzled, why does the oscillation start for my simulation without any help ( the one with 247K resistors and 33nF), but when i try increasing the frequency by lowering the values for the resistors it won't start. Is there something obvious that i'm missing? Can it just be rounding error, as i read on other forums which allow the oscillation to kick in?

Edit: I also found that if i skip the initial bias point calculation in the spice menu it will also start without help.
 
Last edited:

eetech00

Joined Jun 8, 2013
2,654
Yes, you need to use a high-impedance source (such as a current-source) for the jump start, as a voltage-source is an AC and DC short to ground for any signals at that node.
I think the real circuit will start up reliably when the power is applied and shouldn't need any extra help.
Not the best way to do that. A current source will pump the specified current through any device in the current path.
Its better to initialize the node(s) or device(s) to specific value(s) with a initial condition statement.
Example: .IC V(X)=5

eT
 

crutschow

Joined Mar 14, 2008
28,207
when i try increasing the frequency by lowering the values for the resistors it won't start. Is there something obvious that i'm missing?
Not particularly.
I think that when the resistor values are lowered there is more transistor base current, and the circuit more easily settles in a quasi-stable state with both transistors fully on.
 

crutschow

Joined Mar 14, 2008
28,207
a user who is unfamiliar with the way the simulation current source devices work will potentially get erroneous results with their circuit.
The current-source is only used to jump-start the oscillations and then it is effectively removed from the circuit (impedance is ideally infinite) so won't give any erroneous results in this case.
But using the .IC command is a little cleaner than using a current source.
 
Top