Is there a way to set zero rise and fall time in LTspice? I tried that but LTspice automatically uses a default value for <trise> and <tfall> if these parameters are set to zero.

 

It might be that the simulation blows up with derivatives of infinite magnitude. You are actually doing numerical integration of a system of linearized differential equations. If you could set those times to zero you would get meaningless results. Take your pick.

 

Yes, I am aware of this problem. But for some application, I want to use the option.

 

Can you set <trise> and <tfall> to very small times like 1 us or 1 ns? You might be able to find a time that suits your simulation purposes.

 

Can you set <trise> and <tfall> to very small times like 1 us or 1 ns? You might be able to find a time that suits your simulation purposes.

I tried one that is smaller than that above ( 1f (femto) second) but it seems that it still uses the default values.

 

I tried one that is smaller than that above ( 1f (femto) second) but it seems that it still uses the default values.

Femtoseconds must be too small for the simulator to recognize. Try something larger.

 

I tried one that is smaller than that above ( 1f (femto) second) but it seems that it still uses the default values.

You must have put the values in wrong.
As shown below, with the pulse rise and fall times set to 1fs in LTspice, 1fs is displayed in the transient plot.

 

Thank you. Here is the result of me:

 

You've got totally different time scales -- 1 fs rise and fall times but a 20 second period?

You've also got eight parameters to the PULSE model. How does that model handle eight parameters?

What happens if you simply use the settings that crutschow used?

 

You've got totally different time scales -- 1 fs rise and fall times but a 20 second period?

20 is the number of cycles which is plotted.
Period is 1 second.

You've also got eight parameters to the PULSE model. How does that model handle eight parameters?

Here is the model parameters:

What happens if you simply use the settings that crutschow used?

With this, I got the same result. However, with the same setting but change the stop time (run time) fro 4fs to 1m second, the result is totally different. Maybe my LTspice is having some problem.

 

Try subtracting TR+TF from Ton:

.param Ton=0.5-(1f+1f)

PULSE(0 1 0 1f 1f {Ton} 1 20)

 

The problem is your time scale. LTspice assumes that if you are doing seconds of time you don't need fs resolution (why would you?).
If you want to do seconds of simulation and display a 1fs rise-time then you need to set the maximum time-step in the transient setup to 1fs. But that will require many minutes (or even hours) of simulation time since for each second of simulation the computer now has to do at least a trillion calculations and each calculation likely requires many CPU cycles.

 

For pulses you leave the data, blank.

 

For pulses you leave the data, blank.

What data?
If you leave the rise and fall time values blank, the those times default to a fixed percentage of the pulse width.

 

20 is the number of cycles which is plotted.
Period is 1 second.

Here is the model parameters:
View attachment 102197


With this, I got the same result. However, with the same setting but change the stop time (run time) fro 4fs to 1m second, the result is totally different. Maybe my LTspice is having some problem.

View attachment 102200

You still aren't running the same settings that crutschow used. Look at your .tran statement. You are telling the simulator to run the sim for 5 milliseconds. That's 5,000,000,000,000 femtoseconds!

 

What data?
If you leave the rise and fall time values blank, the those times default to a fixed percentage of the pulse width.

What is that fixed percentage Carl? Where is it stated?

 

What is that fixed percentage Carl? Where is it stated?

Don't know if it's stated anywhere.
I've just observed that the default rise and fall times seem to be about 10% of the pulse width.

 

Yes, I am aware of this problem. But for some application, I want to use the option.

I can't imagine why you would want to do it and I suspect it won't let you do that for a very good reason. If you don't believe me, then why don't you shoot Mike Englehardt an email and ask him. I'm sure he'd be glad to educate you on the matter

 

You still aren't running the same settings that crutschow used. Look at your .tran statement. You are telling the simulator to run the sim for 5 milliseconds. That's 5,000,000,000,000 femtoseconds!

As I said above, with setting exactly as crutschow, I got the same result. However, I was wondering why run time (4fs, 5m) affects the rise or fall time. That seems strange to me.

 

I'm pretty sure that the actual simulator is not overriding you values with "defaults", but rather the schematic capture tool. You should be able to simulate a hand written circuit file (or a hand tweaked one) in which you force the values to zero. This may or may not simulate successfully as it may cause convergence problems.