So there is this one circuit that uses only 1 transistor to make a simple LED flasher. The schematic is from this website http://tefatronix.g6.cz/display.php?page=dflasher&lang=en

I entered it into LTspice, and for the life of me I cannot get it to simulate; particularly I do not see any RC charging/discharging going on. I tried expanding the simulation time super long (1500 seconds), and I see some minor variation in the LED current, but only a fraction of a pico Amp. I tried smaller resistor and cap values, but nothing seems to change.

I was able to get a different LED flasher (2-transistors, 8 parts) circuit to simulate, but this simpler circuit has me stumped.

LT spice file attached

 

hi,
Add Startup =0 in the tran window.
You will see the exponential charge, but no oscillations.
Read the warning notes in the link regarding it may not work.
E

 

Welcome to AAC!
The circuit operation is dependent on negative resistance due to transistor junction breakdown, which is not modelled in the BC337 model. Try a diac instead of the transistor.

 

Welcome to AAC!
The circuit operation is dependent on negative resistance due to transistor junction breakdown, which is not modelled in the BC337 model. Try a diac instead of the transistor.

Thanks! I thought I was losing my mind.

I'm new to LTspice so I just ASSUMED transistor junction breakdown would be modelled. Considering it can model 100s of Linear Tech chips, I figured a 3pin transistor would be no biggie. Kind of disappointed to say the least.

 

Look at how assume is spelled. ass-u-me

Assuming a simulator knows more than you or is making the right assumptions is just that, an assumption. Unless you delve into the models and understand the assumptions LTspice is making, you don't know what it's doing.

 

See

My models:
http://bordodynov.ltwiki.org/

 

Look at how assume is spelled. ass-u-me

Assuming a simulator knows more than you or is making the right assumptions is just that, an assumption. Unless you delve into the models and understand the assumptions LTspice is making, you don't know what it's doing.

I thought it was a very safe assumption since it is simply a 3 pin discrete device that has been around for decades. After all, isn't the role of a simulation tool to 'simulate'? When you see titles for example circuits that LTspice can simulate like ;LTC7851/LTC4449 Demo Circuit - High Current, Quad Output Synchronous Buck Converter with Discrete Gate Drivers and MOSFETs (7-14V to 1.8V, 1.5V, 1.2V, 1.0V @ 30A)", you would think a simple transistor would be a walk in the park for LTspice.

 

After all, isn't the role of a simulation tool to 'simulate'?

It has to make assumptions. Some of those assumptions may not be appropriate. If you want to simulate real conditions, you need to change the models to account for parameter variations.

I've simulated several circuits in LTspice and couldn't get the simulator to work. In my case, I knew the circuit worked and didn't bother learning enough about LTspice to make it work. I just breadboarded and confirmed that the design worked as expected and moved on.

 

In LTspice, it is possible to specify breakdown voltages for bipolar transistors. Adding these parameters increases the counting time of the circuit. What you see in this relaxation scheme uses the ad-hoc modes of the transistor. I'm interested in non-standard oscillators that use avalanche breakdown. So I made some transistor models. The parameters of the light pulses can vary widely with the transistor instance. It is necessary to select resistors, capacitors and supply voltages.

 

See
View attachment 158570
My models:
http://bordodynov.ltwiki.org/

Thank you so much! I will definitely be using your models.