LTSpice and Micro-Cap

[Yazoo]

I have been trying to simulate this circuit fragment from the Boss CE1:




I've tried this in both LTSpice and Micro-Cap. What I am trying to check are the voltages on the collectors of the four transistors. I breadboarded the circuit fragment using a 14V DC supply (the original circuit has a bipolar 14V+/14V- supply. I connected 14v to the points marked ground in the circuit fragment and GND to the point after R34. On the breadboard version, I measure around 7V, so -7V on the original.

I do not get this in either circuit simulator.  I just get 14V. I am new to using LTSpice and Micro-Cap and can't see what I'm doing wrong. I tried a simple voltage divider circuit and that does work.

[Rob Strand]

The original is powered from ground and -14V so the collectors should swing a little under 0 to -14V.

Your oscilloscope needs to be DC coupled to see that, you might get +/-7V if the scope is AC coupled.

The point "I" needs to be fed by a voltage.   You should include resistors R78, R79,  R63, VR13 (set to say 25k) with R78 connecting to +14V and the opamp side of R79 connected to ground.

You can get instances where the oscillator doesn't start-up in the simulator and you have to force initial conditions.   Also you might need to set-up an initial condition voltage on C22 so the simulation doesn't take ages to stabilize.

I have simulated this circuit and in the back of my mind there was some quirky behavior with the simulation.  Off hand it might of been something to do with the voltages on C22.

[Yazoo]

Thanks for your reply. I've tried, tried and tried again. I have had more luck in LTSpice. If I increase the capacitor sizes substantially, I do get a result - 4.7uf and 1uf. I cheated and just added a sine wave fed into point I.




Below those large capacitor values I just get a 14V line. Is it just that the frequency is too high for LTSpice?

[Rob Strand]

Thanks for your reply. I've tried, tried and tried again. I have had more luck in LTSpice. If I increase the capacitor sizes substantially, I do get a result - 4.7uf and 1uf. I cheated and just added a sine wave fed into point I.

Below those large capacitor values I just get a 14V line. Is it just that the frequency is too high for LTSpice?

A straight line could mean the oscillator isn't starting up and that can be due to initial cap voltage on the C22 capacitor.  Once it starts off on a bad foot it gets stuck there and the VCO doesn't oscillate.  I haven't confirmed this but there's a longs list of possible issue with getting oscillators to start.

Here's a few tips:
- Put the resistors between the LFO opamp into the simulation.
- Put an initial condition on the C22 cap (IC=1.6  will set the initial cap voltage to 1.6V)
  You need to edit the part to set it.
- Force the parameters on the .tran statement and enable uic "use initial conditions".
- To get things working make the LFO output a fixed DC voltage.

One problem with VCO + LFO simulations is you need 10ns to 100ns steps to get the
VCO to work but the LFO is operating at 1sec to 10sec sweeps.   That's a lot of
simulation points and simulation time.

For what I was doing at the time I reduced the value of C22 to 25n to speed-up the setting time.
I could get away with that because the LFO output was DC.  For a sine simulation you will need
to put back the 1uF and have long simulation times.

I used the transistor and diode models from here,
https://www.cordellaudio.com/book/spice_models.shtml

Not sure if I did that to get the simulation going or not.

FYI, there's no real speed limit in spice but if you don't force the time increments in the .tran statement sometimes the simulation goes wrong.



You can see everything here, but note I don't keep the same parts designations as the original schematic.
The output swing in my simulation is as expected 0 to -14V.