weird LT Spice

What did you expect for FREE ?

Cheers

Heck, expensive software is buggy too. I prefer free bugs!

The 1V supply fixed it, but adding a diode broke it again.

Setting the transient response option "skip initial operating point solution" is ugly but does fix it.

I've had a few weird things happen which get fixed after saving, closing and restarting. I think LTspice XVII is buggier than the older versions, but still very good value.

Cheers

One should never underestimate one's capablity for screwing up a simulation by hitting the wrong key or selecting the wrong option.

That kind of error can be very hard to find, and excruciatingly embarrassing when you do find it, or somebody else finds it for you (which is usually the quickest option, if you can survive looking like an idiot).

I have seen LTspice circuits not converge until I added something weird, for example, I got it to work once by adding just ONE end of a resistor to the circuit. Later versions did not need it.

Also, sometimes you need to add a high value (several MegOhms) resistor from a floating node to a grounded node to get it to converge.

But your circuit converges right ? It just comes up with a blank trace ? That I haven't seen before as far as I remember.

I will assume that future versions of LTspice won't require that weird battery connection.

You have GND missing somewhere whether it's used in the actual circuit or not, you need to rig it. Probe needs a reference.

The circuit is fairly simple and visually correct. It does use some EPC GaN fets, with an included library, but I've used that many times before and the .lib file looks OK.

Spice doesn't complain about convergence or take long to run the sim. It's just as though all nodes except the single pulse generator simply don't exist, and don't show a plot line if probed. Not even the +12 volt power supply.

And it's erratic; adding a part might fix it or break it.

Am 07.02.19 um 17:31 schrieb boB:

There is no such thing as a floating node in Spice. Everything has to have some connection to node 0 (gnd). The first thing that spice does to your circuit is constructing a conductance matrix and zero or not-completely-0-but-nearly entries mess up the algorithms that follow. Just imagine computing a voltage difference between 2 nodes from current and NO conductance. i/0.

To avoid that, Spice normally adds huge resistors to nodes that are not connected "enough". The size of these resistors is hard to determine. Make them too large and the equation system will not converge, make them too small and the user will complain that the results are not accurate. And resistances/conductance may change wildly during simulation.

So you don't add just one end of a resistor to the circuit. The other end is connected also via the invisible large R.

And WRT LTspice support: If you feed your problem into the provided channels, it will be fixed pretty soon. Last week I heard of a case where writing sound files did not work for resolutions other than 16 bits. That was fixed within hours.

regards, Gerhard

Which version? If it is XVII, that may be the problem. Try it with version IV.

The LTSpice UI is not particularly well-known for its quality. I hate when it ignores manually changed .param values and sticks to the old ones. Only one change per 3 or 4 take the desired effect. The way it looks like on a 4k display is another "feature"...

Best regards, Piotr

XVII, which is otherwise pretty good. IV isn't supported any more.

I think the problem is that I have some optional peaking inductors in series with some fet gates. If I set the values small, around expected circuit parasitics, the equivalent time constants or resonant frequencies get crazy and the initial conditions solution doesn't converge. But there is no warning, the sim runs, and the symptom becomes this invisible node thing.

Removing the inductors, or skipping the initial condition solution, either one fixes it.

Does it even work at DC? That's usually easiest to debug. It's probably your fet models.

Check to see if you have an undriven node lurking somewhere. Spice doesn't like those and may or may not throw a fit.

Rick C.

A grounded +1V DC power supply, connected to nothing in the circuit, probes as "no line."

I should look at the .RAW file. Probably mostly empty.

Something's wrong with that power supply. They have provisions for a label and then another provision for naming a net. Either you or LTS has the net unspecified.

No, it's an initial conditions convergence problem. With no warning.

No, wrong again. It now seems like the EPC2038 model breaks LT Spice.

But skipping the initial operating point solution does work.

I know nothing, but there is a yahoo LTspice group/thing I've found useful.

George H.

My particular circuit did not need a large value to any other node as I remember. I know you can choose some of those values. But LTspice doesn't converge well sometimes. Requires some playing around with adding extra conductance sometimes. I believe that Mike Englehart (and others?) have done a lot of work..

John's battery I think he said wasn't connected to anything. Might be default be connected to ground by some high value. Not sure why that would help anything though.