QUCS-S issues help needed for LED blinker

[edy]

Hi everyone,

I didn't see a specific simulator section on the forum, so I thought I'd ask here. I'm just starting to get back into circuit simulation, building basic prototypes. I'm now using QUCS-S after having dabbled in LTspice years ago in Windows. I'm now on Linux Ubuntu 22.04 so I installed a QUCS-S 25.2.0 build from ra3xdh. I've attached the schematic and other related files as a ZIP for a simple "LED Blinker" astable multivibrator, with the following schematic:



My simulation shows the first 1 second, basically one complete cycle and then errors out. No matter how long I set my transient simulation the cartesian graph goes for 20 seconds but it should be automatic (ending the length of the simulation). I've tried various suggested changes on Google search but no matter what I do it always ends. I tried loading up one capacitor charge at max and other at 0V. I've tried changing the values of resistors and caps and the timing is still the same... I'm not able to speed up or slow down the blinkers.

Can someone please look at my files and let me know what I'm doing wrong. Thanks.

[Whales]

Your circuit is working, you just can't see it.

1. Increase the number of simulation steps (10 steps over 10 seconds is far too few).

2. Check the variables used in your graph.  They appear to be old (qucscator) simulator outputs from some simulation you ran a long time ago, not the new (ngspice) simulator outputs that you are generating in QUCS-S.  You graph will never change because it's looking at old data.  If you add a new graph then you can select the new names easily.

Both changes shown here.  Your graph of old unchanging data at the top, my graph of new data below.

(And yes, this is all completely non-obvious.  Even worse is when you have to learn the ngspice names for current probes, that throws your head into a twist.  QUC-S is amazing, but it sadly adds a lot of new traps with its transition from qucscator to ngspice)

[edy]

Thank you, I changed the simulator to Ngspice (Qucsator was giving me problems). After that I added another graph and chose to plot the tran.v(led1) and tran.v(led2) (which appeared as new parameters I never saw before) and was able to reproduce the lower graph showing the oscillations! Thanks! I still don't understand what is going on then in my upper graph... unless it shows the old data... Also if I try to edit that old graph, the variables previously available under Qucsator (Led1.Vt and Led2.Vt) are no longer listed. I guess I'll have to mess around with it more and try it on some other circuits I've been trying to simulate (like an oscillator using a pair of OpAmps which was also giving me trouble). Thanks for the advice! I thought maybe over the years of development they would have made it more idiot proof for users like myself. However it looks like a lot of fun to learn on and develop and play around on!

[Whales]

> hanks! I still don't understand what is going on then in my upper graph... unless it shows the old data.

Correct.  It's showing old data from when you used Qucscator.  The giveaway to me was that its horizontal axis went to 20 seconds, whilst your simulation was only supposed to go to 10.


> I thought maybe over the years of development they would have made it more idiot proof for users like myself.

The original QUCS was reasonably polished in this regard.  Sadly the spice solver (qucscator) was annoying as all hell for transient analysis, it would get itself stuck ("jacobian error!") all the time and the oddest circuit tweaks would fix it or break it.  I spent many afternoons puzzled as to whether my circuit was bad or if I just needed to work out the right offering to the gods.  For non-transient simulation modes it was great, however, and I truly enjoyed using it for that.

QUCS-S is a project that grafts in ngspice (which is tremendously better and more reliable for transient sims) but it also does not want to break compatibility with qucscator.  Unfortunately the two solvers have quite a few fundamental differences, so chunks of the UI don't make as much sense any more or have to be duplicated for each.  It's messy.

Another layer of confusion to be wary of: there is a "compatibility mode" option in the settings that lets you using pspice models et al.  Many of the in-built models (in the libraries sidetab) assume you have this set a certain way.


> (like an oscillator using a pair of OpAmps which was also giving me trouble)

Feel free to share, I might be able to help 

[edy]

I'm working to model the following starter kit board. I found a dual OpAmp LM358 LED flasher circuit which seems to have the same number and type of components, so I am assuming it basically follows this. There are 6 resistors, a transistor, and a capacitor along with the LM358 providing the 2 OpAmps. I also noticed "UR1" which seems to be some trimmer next to the main capacitor... I'm assuming this is to adjust the value of the cap to change the blinking frequency? I am going to try putting together that schematic and seeing what it does with the values as printed on the PCB. I don't have the board so I can't verify that it is laid out the same way but will confirm once I get it. I'll post my progress here shortly.

[EDIT1:.... I've attached the QUCS-S file and log. I have tried the LM358 provided in the library, I tried standard OpAmps, I've tried the values on the PCB as well as those in the actual schematic diagram. I have played around with various values but nothing seems to want to simulate. I've tried different time durations, time steps, etc... I'm stuck and I don't know why].

[EDIT2:  I'm also a bit confused as to why the OpAmps are "flipper" upside down with the "-" being on top, and the "+" being on the bottom... and the power Vcc and Vee to the op-amp in the diagram also seems flipped, because in QUCS the Vcc is on the side of the "+" input, and vee is on the side of the "-" input. In my QUCS drawing I flipped my OpAmps to put the "-" on the top and "+" on the buttom but I realized I need to flip the Vcc and Vee to the proper rails... I tried both ways and still ran into same problems.]

[EDIT3:  I've attached a simple one op-amp square wave generation which should also work, which I found online. The simulator runs, it does not crash, but my output is flat... can't figure out what's going on].

[RoGeorge]

I'm now on Linux Ubuntu 22.04 so I installed a QUCS-S 25.2.0

Just so you know, LTspice (for Windows) installs and works just fine under Linux, too. 

You have to install WINE first (WineHQ for Linux, usually this is a single line from terminal 'sudo apt install wine', don't use the GUI installers from Ubuntu), then download LTspice for Windows, and double click the LTspice exe installer, as if you would do on Windows.

[golden_labels]

Regarding blinker circuit:

It is a two op-amp triangular wave oscillator. IC2 is a Schmitt trigger, with the 10 kΩ and 20 kΩ resistors setting its switching point. It’s fed from oscillator output. IC1 is an integrator, together with the 1 MΩ resistor and 1 µF capacitor. The two 4.3 kΩ resistors set the virtual ground.

At least it’s meant to be one. The capacitor used is wrong. The circuit requires an unpolarized capacitor. While not required for simulation (usually) and understanding the operating principle, you may need an additional, high-value resistor across that capacitor too. This is to provide a DC path for the feedback and avoid offset slowly accumulating on this capacitor.

Regarding “op-amp-osci.zip”:

Remember that an electronic simulator is nothing more than an advanced, specialized calculator. It may come with a fancy GUI to make entering numbers more convenient. But in the end it’s just you putting numbers into equations, equations you want to solve. The program just does the tedious part of crunching numbers.

I underline “equations” and “you.” You’re the tool operator and to operate the tool effectively you need to know what you want to calculate and how. The simulator isn’t going to do it for you.

In “op-amp-osci” you asked it to multiply everything by 0. The calculator obediently did a few millions of multiplications by zero, as asked. Consider, what equations this model represents, and if it can ever spit out anything other than 0. Capacitor placed across 0 V will not charge, difference between 0 V and 0 V on inputs is 0, and 0 multiplied by arbitrarily huge factor remains 0.

Regarding “heart.zip”:

Be happy mathematical models do not produce smoke. Your op-amps have positive and negative power supplies swapped (VCC, VEE).

And, in general, circling back to what I earlier said: it’s just a calculator. The simpler equations you use, the better. Both for the calculator and for you. There is hardly any reason to simulate all the details of LM358 or BC548 behavior, or a dozen diodes in parallel, to approximate the behavior of this circuit. You may stick to more generic components. And even split that into functional blocks and consider them separately.

After fixing power supply lines, this circuit works as expected. But many other will give you pain: dozens of (hidden in this case) non-linear components and huge range of values are making the landscape very hostile for any solver.

[edy]

I'm now on Linux Ubuntu 22.04 so I installed a QUCS-S 25.2.0

Just so you know, LTspice (for Windows) installs and works just fine under Linux, too. 

You have to install WINE first (WineHQ for Linux, usually this is a single line from terminal 'sudo apt install wine', don't use the GUI installers from Ubuntu), then download LTspice for Windows, and double click the LTspice exe installer, as if you would do on Windows.

Yes thanks I did use an old LTspice under WINE in the past. I thought that I've try out the new QUCS-S on Ubuntu and see how it works. I have Windows at work and so while I have a free moment I'll install and play around with LTspice Version 26.0.1 and see how that differs. I noticed there are lots of tutorials on the AD website as well. Note that I also have a Win10 VM running on my Ubuntu machine so I could just as easily install the latest LTspice there also, so lots of options. Main thing is to go through tutorials and understand how to build useful circuits that do what I want and learn some of the basic building blocks before actually trying real-world builds.

[edy]

Regarding blinker circuit:

It is a two op-amp triangular wave oscillator. IC2 is a Schmitt trigger, with the 10 kΩ and 20 kΩ resistors setting its switching point. It’s fed from oscillator output. IC1 is an integrator, together with the 1 MΩ resistor and 1 µF capacitor. The two 4.3 kΩ resistors set the virtual ground.

At least it’s meant to be one. The capacitor used is wrong. The circuit requires an unpolarized capacitor. While not required for simulation (usually) and understanding the operating principle, you may need an additional, high-value resistor across that capacitor too. This is to provide a DC path for the feedback and avoid offset slowly accumulating on this capacitor.

Regarding “op-amp-osci.zip”:

Remember that an electronic simulator is nothing more than an advanced, specialized calculator. It may come with a fancy GUI to make entering numbers more convenient. But in the end it’s just you putting numbers into equations, equations you want to solve. The program just does the tedious part of crunching numbers.

I underline “equations” and “you.” You’re the tool operator and to operate the tool effectively you need to know what you want to calculate and how. The simulator isn’t going to do it for you.

In “op-amp-osci” you asked it to multiply everything by 0. The calculator obediently did a few millions of multiplications by zero, as asked. Consider, what equations this model represents, and if it can ever spit out anything other than 0. Capacitor placed across 0 V will not charge, difference between 0 V and 0 V on inputs is 0, and 0 multiplied by arbitrarily huge factor remains 0.

Regarding “heart.zip”:

Be happy mathematical models do not produce smoke. Your op-amps have positive and negative power supplies swapped (VCC, VEE).

And, in general, circling back to what I earlier said: it’s just a calculator. The simpler equations you use, the better. Both for the calculator and for you. There is hardly any reason to simulate all the details of LM358 or BC548 behavior, or a dozen diodes in parallel, to approximate the behavior of this circuit. You may stick to more generic components. And even split that into functional blocks and consider them separately.

After fixing power supply lines, this circuit works as expected. But many other will give you pain: dozens of (hidden in this case) non-linear components and huge range of values are making the landscape very hostile for any solver.

Thank you, I'll have a look and put the components you suggested into the circuit and simplify everything (like reduce down to one LED) and swap the OpAmp polarity. I'm going to keep this in mind with future circuit builds and try not to over-complicate things and try to look for traps as you said where things are being calculated by 0 or infinity. I'm happy that the circuit simulator doesn't produce smoke (or kill my computer) but that would be a fun addition to the simulation... virtual smoke coming from some component(s) to let me know where I screwed up.  Thank you again for all the advice! 

[edy]

Ok I installed LTSpice at work and was able to simulate the astable multivibrator from the first photo (see attached screenshot)! It is a little different UI than QUCS-S but after looking at the tutorials I figured it out. I was looking for how to "label" my wires as in QUCS-S and then saw that you can just click on the wires after the simulation and it will graph it. Next I will try to simulate the Op-Amp version and see if I get better success on LTspice and try the same on QUCS-S when I have a chance.

[edy]

I was able to model also the single opAmp oscillator from the previous example, I had to use "UniversalOmpAmp2" which was suggested on other pages. The first few opamps didn't work as expected but this one did manage to create an oscillator and I was able to change the frequency by playing around with the capacitor value. I'm going to work on the dual OpAmp example using the LM358 next and see what happens... may have to use the OP200 as equivalent or just split it into separate op-amps.

[Zero999]

It makes it easier to interpret the plots if you add net names.

Setting the ic (initial condition) to something like 1V, on one of the capacitors, helps to make the simulation start, because it introduces asymmetry.

Finally, the base voltage goes negative, when the opposite transistor turns on. At higher voltages, this can be a problem for the transistors, because the reverse base-emitter voltage rating of most transistors is typically 5V to 7V. Adding diodes in series will mitigate against this. Operation at 9V is marginal, without them.

[edy]

Thanks everyone for the help. I've managed to experiment a bit more with QUCS-S and installed LTSPICE on both a Windows machine at work and now I have it running on my Linux laptop at home in a Win10 VM. Here's where I am so far and have some questions. First, I've attached some screenshots from a video that shows a similar board someone posted on YouTube. I looked at the traces and tried to reverse-engineer the schematic, which I put into BOTH LTSPICE and QUCS-S. For some reason QUCS-S gave me a flat line. LTSPICE at least shows some oscillations but the current across the diode seems to not vary much... it goes up and down but by only a little. I've attached all the relevant files here.

Here is the YouTube video:



I've attached a screenshot and all the LTSPICE files and QUCS-S files below. I'll be getting this board soon and want to make a video on it, but I think it would help to learn more about it than just soldering, which is fun in and of itself... but the viewers may want more understanding of what is going on, and so do I. I'm trying to figure out how the opamps play off each other. The schematic does look very much like the Lamp pulser circuit diagram.... although it looks like I reversed the order of the op-amps (that is, the one on the RIGHT in my schematic is the LEFT one in the Lamp Pulser circuit diagram, and vice-versa). That's because I didn't look at anything while I was following the traces and drawing and trying to figure things out... I'm glad though that I got at least something close at the end of it! 

Unfortunately, I only got oscillations on my LTspice model and even then it doesn't vary as much as I thought to make the LED dim. I would have thought I'd see a bigger difference in the current across D1 in my charts. Can anyone tell me why? Also QUCS-S shows one dip then rise (after I have the "Switch" set to turn on at 0.5s) and then flat-lines with no oscillations.

One other confusing bit was the potentiometer. I didn't understand why one end was connected to both VCC and output, and the other to GND. From what I understand now, the VCC connection is pointless because if connected also to "OUTPUT" it really turns it into an INPUT... and the really the pot resistance is the distance from the middle "INPUT/OUTPUT" and the GND end. If the pot is turned all the way over to the VCC, the entire pot resistance 50k is felt. If the pot is turned all the way over to the GND end it because almost a short.

One thing I may do is take my schematic and flip the op-amps around and see how close it looks like to the lamp pulser diagram as that can also help me understand better.

[golden_labels]

We’d need to see the values set. I built it in Qucs-c and it oscillates (see the attachment). I removed the switch, since it serves no purpose in the simulation, while adding complexity to calculations. But perhaps you’re actually setting it to turn off power instantly after start? I also had to increase timespan, since this is a very slow oscillator. With the 60 second run time that meant 600,000 steps (100 µs) to calculate, which again is very excessive in general.

With the diode model I assume is used there,⁽¹⁾ this circuit goes up and down between 14 mA and below 1 mA. Half of a cycle the current is too low for light to be noticeable.

The LTspice version misses the resistance introduced by the potentiometer. It’s not necessarily wrong. But it works as if the taper was on the extreme end, bypassing the entire length of the potentiometer. Not sure if that was the intention.

However, after stripping the circuit of irrelevant elements and rearranging it to a more common form, we get what the picture below shows. A triangle wave oscillator, but the Schmitt trigger feedback is wrong. At first I thought it’s your mistake in reverse engineering. But no, it seems you did it right. I’ll recheck later, when my brain resets. Just to make sure I don’t see things that aren’t there.



Assuming the reverse engineering is correct, I can explain it only in two ways. First is that somebody misplaced a resistor in design. But since it still does some oscillation (at least with LM358), it went unnoticed. Not the authors of this kit, as the design appears to be widely circulated way beyond this product. Second is that a long time ago somebody made that mistake, noticed it produces a more desirable effect, and shared it. But I can’t recall seeing that myself⁽²⁾ in the past. On the other hand I’d probably also not pay attention, until you asked now.

⁽¹⁾ 2 V @ 20 mA, noticeable conduction at a bit over 1.5 V, which matches many red LEDs. See the second image this post for the charts of what diode “LED” models Qucs-c ships with.
⁽²⁾ Which does not mean I did not. I might have seen that a dozen times, perhaps even soldered it myself. Brains are just very bad at memory.

[edy]

Thank you for the amazing help! I have looked again and again at my reverse-engineered schematic and after I flipped around my 2 op-amps I believe I found my mistake! The resistor which you have as "R11" (which on the board is labelled R3) may actually be somewhere on the vertical wire between the resistors you have labelled as "R7" and "R12"..... That is where you put your ? question mark ? and arrows ... YOU ARE CORRECT TO QUESTION THE PLACEMENT! My schematic was wrong!!!! It is actually on the vertical, and it exactly matches the "lamp-pulser-circuit" schematic picture that I included before (once the op-amps are switched!). The values are quite different on the "Lamp-Pulser-Circuit" diagram and I wasn't able to get it to work... either because of something I did wrong wiring and drawing it up, or the components I used (not all Opamps behave well in the simulation) or because the values didn't give it a good oscillation. But after checking the board traces a dozen more times to confirm the way R3 and R4 are connected, and indeed redrawing it from scratch again properly, I got it to works in QUCS-S and LTSpice!!!!     (see "heart4-qucs.zip" and "heart4-ltspice.zip" attached).

Here it is:



As Dave would say.... winner winner chicken dinner!

I attached a current probe at the LED, I'm sure there is a better way to do this by creating a variable for the current at D1 but I just don't know how to do that yet, so I stuck the probe in there and plotted it on one axis, and voltage on the other. I'm getting a nice up and down movement of voltage on the LED...  I have my "switch" to turn on at 500 ms, and I have set my "POT1" to actually be around 60/240 rotation, which is 25%...  which because of the way it's wired up is actually reversed... 25% would actually be 75% of the 50k resistance. When the POT1 is at 0% it actually is at the full 50k since the middle arrow is closer to one end. I believe when I have my POT1 set to 100% it gets closer to 0k.

When I increase my POT1 to higher and higher percent of "rotation" this actually reduces the resistance and my pulses get closer and closer together. I assume it's because it allows the capacitor to drain faster through it. When I set the rotation to the MINIMUM it makes the pulses longer and longer, as it seems to be increasing the resistance more and more, causing the capacitor to drain more slowly. When I increase R6 it also slows down the rate of pulses... so the combination of the POT1 and R6 is what sets the pulse rate and the higher it is, the slower it goes.

[EDIT:  Ok I've managed to also simulate it in LTspice once I fixed the schematic and attached both screenshots (below) and the actual ZIP of the schematics as well and it behaves similarly]

[golden_labels]

I rechecked the circuit with a fresh brain. Indeed there was a mistake in reverse-engineering. The output of op-amp goes both to the 100 kΩ and 4.7 kΩ resistors seaprately.

So this is a standard triangle wave generator, as mentioned in my first reply.