Hi Arthur,
No, I haven't tried any of the non-freeware simulators in quite some time, as most of the ones I have seen are very expensive. I have had numerous problems with convergence using LTspice. It seems the power amp designs that result in very low distortion also result in poor convergence (or complete lack of it).
I generally have to resort to the trick of determining the operating point using a transient analysis, setting the power supplies with a PULSE statement and using .SAVEBIAS and .LOADBIAS to save and load files containing .NODESET specs.
No, I haven't tried any of the non-freeware simulators in quite some time, as most of the ones I have seen are very expensive. I have had numerous problems with convergence using LTspice. It seems the power amp designs that result in very low distortion also result in poor convergence (or complete lack of it).
I generally have to resort to the trick of determining the operating point using a transient analysis, setting the power supplies with a PULSE statement and using .SAVEBIAS and .LOADBIAS to save and load files containing .NODESET specs.
I have been haveing a go at microcap the last two weeks or so... now starting to grasp the basics... very usefull for PCB design, but not useing funcitonality not available in LTspice etc...
The truth is, I am still learning... but it is fun to be able to put the simulator to actual use for something, even if it was just to calculate dissipation...
I still have to learn how to see what the in and output impendance of my regulator is, or even things like how much noise it rejects etc... or even if those things are at all possible...
But my vote goes to Micro Cap out of all the spice tools I have played with recently
The truth is, I am still learning... but it is fun to be able to put the simulator to actual use for something, even if it was just to calculate dissipation...
I still have to learn how to see what the in and output impendance of my regulator is, or even things like how much noise it rejects etc... or even if those things are at all possible...
But my vote goes to Micro Cap out of all the spice tools I have played with recently
Re: Convergence
I have not. I was going to, but I read in the LTSpice forum from people who have repeatedly proved they know what they're talking about when it comes to circuit simulation that the convergence capabilities of LTSpice are superior.
LTSpice has two different solvers. I have had problems with some circuits, but switching the engine has been faster than playing with GMIN, etc. Truth to tell, I don't recall a problem using the 'alternate' solver in the past year or more.
Regards,
Jeff
PHEONIX said:
I have not. I was going to, but I read in the LTSpice forum from people who have repeatedly proved they know what they're talking about when it comes to circuit simulation that the convergence capabilities of LTSpice are superior.
LTSpice has two different solvers. I have had problems with some circuits, but switching the engine has been faster than playing with GMIN, etc. Truth to tell, I don't recall a problem using the 'alternate' solver in the past year or more.
Regards,
Jeff
Re: Re: Convergence
- Klaus
I also run the alternate solver and don't have much convergence issues. And if, I could always help with either an .OPTION GSHUNT or with the "last resort" of ramping up the supplies and save the bias with .SAVEBIAS at a time when the circuit has settled, just like andy_c has pointed out.Jeffin90620 said:
- Klaus
1) attach a AC current source (set it to "AC 1") at the ouput so that the current from it flows into the circuit, and run a AC simulation run. Then plot voltage accross that AC source, this corresponds to the output impedance in ohms (in a mag/phase plot).Nordic said:
2) place a 1V AC voltage source in series with the input (the DC input source should have zero impedance) and plot 1/input_current, this gives input impedance. Or look at the output, there you will see the input noise rejection.
This was all in the small signal AC domain, at a fixed DC operating point with microscopic AC voltages/current ("AC 1V" sets only a scale factor for the plots but it doesn't apply 1V to the circuit). So you can set different operating points (say, different resistive loads) and usually you'll see a slight change in the response
To check stability, line and load regulation it is also useful to do a transient run with a real AC source, applying a small squaurewave signal and look at the waveforms directly, again with different operating points (or using a low freq sine or ramp to shift operating points continously).
- Klaus
i've used various versions of SPICE, and although LTSpice doesn't have some of the "whistles and bells" some of the other SPICE software (such as the "real time" oscilloscope in TINA), LTSpice has a good level of universality (you can directly import most text based models and libraries, often without modification) as well as a more stable set of solvers (often other spice software would dump during a simulation with only vague clues of the reason).
also simulating saves a lot of time with selecting a good starting point for parts values for a circuit. instead of building an oscillator and rummaging through a box of capacitors, i can just try different capacitances by typing them in and watching the results. once i get the proper capacitor in SPICE, i only have to rummage for one cap. SPICE will also measure device currents without the hassle of connecting an inline milliameter or expensive oscope current probe, so i can see how a particular current source or current mirror will behave. SPICE may not have 100% accurate results all of the time, but usually the results will be close enough to know whether a circuit is going to work or not, and be at least in the ballpark of how well it will work.
also simulating saves a lot of time with selecting a good starting point for parts values for a circuit. instead of building an oscillator and rummaging through a box of capacitors, i can just try different capacitances by typing them in and watching the results. once i get the proper capacitor in SPICE, i only have to rummage for one cap. SPICE will also measure device currents without the hassle of connecting an inline milliameter or expensive oscope current probe, so i can see how a particular current source or current mirror will behave. SPICE may not have 100% accurate results all of the time, but usually the results will be close enough to know whether a circuit is going to work or not, and be at least in the ballpark of how well it will work.
unclejed613 said:
Exactly my opinion to.
Very good summary, unclejed.
In most any other area virtual simulations are used.
Be it weather forecast or Aeropilot training flight simulators.
Or aestronaut educations.
We wouldn't want to send those pilots out for initial training in real aeroplanes/space shuttles,
would we?
He who can not accept good tools to model reality
should not post here using virtual communication via internet.
( this should not be confused with REAL SPEAKING to EACHOTHER )
If you are 'old-fashion' and only accepting REAL THING:
Call me up via telephone ( another virtual!!! way to communicate )
and we settle some place and time to meet in person.
Regars, Lineup
unclejed613 said:
You have hit the nail on the head regarding the greatest value-added of performing SPICE simulation. In particular, I just love to be able to probe around a circuit effortlessly (and without disturbing the circuit) to see exactly what is going on. Not just currents flowing through elements, but also probing differential voltages effortlessly.
Cheers,
Bob
I have said this many times before, but don't get fooled that Spice is only useful for predicting the behaviour of actual cirucuits to be built. If you think so, you have a lack of imagination. It can be very useful to study circuits with more or less ideal models to pinpoint certain effects. For instance, one might start with the basic NPN model, which is just the basic transfer function. Then one can add various effects and study separately. For instance, add Cob and see how that affects distorsion. Then remove it and add the Early voltage, etc. And those are just straightforward simple ideas. You can do much more interesting things. Partially ideal models can tell a lot of interesting things about a circuit by factoring out various contributions in a way that is impossible to test in a real circuit. Then of course, those factors will interact both in reality and in the sim, when you throw them all in, but you might get a better idea of what causes what, and what factors are most important.
Spice is also a great tool for learning. If you try to understand theory by deriving formulas yourself (which I find a much better way to understan than just read them in a book), then you can do some Spice simulations to see if what you derived seems to be correct.
This is still no argument that John and others with very long experience in managing without Spice should necessarily start using it now. On the other hand, if trying to get outsde the mental block about how to use Spice that I point to here, they might be surprised, perhaps.
Spice is also a great tool for learning. If you try to understand theory by deriving formulas yourself (which I find a much better way to understan than just read them in a book), then you can do some Spice simulations to see if what you derived seems to be correct.
This is still no argument that John and others with very long experience in managing without Spice should necessarily start using it now. On the other hand, if trying to get outsde the mental block about how to use Spice that I point to here, they might be surprised, perhaps.
john curl said:
Still using a Mac, are you? I don't think you should find much of a problem to get LTSpice running on a PC. Then, adding new models might perhaps be a bit tricky if you are not friendly with computers, but it is not so difficult if somebody shows you how.
LTSpice also seems to run fine under Linux, if installing Wine first, which I think works also for the MacOSX. I tried it under Linux and it worked without any fuzz, except possibly som ugly rescaling of text fonts sometimes.
Do you have any friendly forum members nearby who could give you a crash course?
john curl said:
John:
I'll give you a crash course (which probably will be all I know) to get you up the next time I'm nearby. Assuming you have the computer.
Getting models and making them work is the bigger pain. We all need sources for models for Jfets, MosFets and who knows what else that aren't in the default LTspice libraries. And a quick writeup on how to include them (I have to search the web every time I do that).
I personally don't think Spice is the way to -130 dB distortion products. Its a start but the devices themselves vary too much for the models to have that much accuracy. For the incredibly low distortion numbers to be real it needs to be built and verified. Its great for Monte Carlo analysis to see if you can make more than one of something. Its also great to test an off the wall idea to see if it will work.
-Demian
Thanks Demian, it was good meeting up with you today. I do need to talk to you also about the QT, as 10Hz is 10db too low for some reason, maybe a setting. Let's talk tomorrow.
Spicewise, I am trying to get PMA's circuit sims into Microcap 9, and can't quite do it. That is my biggest hassle at the moment.
Spicewise, I am trying to get PMA's circuit sims into Microcap 9, and can't quite do it. That is my biggest hassle at the moment.
1audio said:
High Demian,
Although I agree with most of your comments, I don't see a really good reason why you put the limit on -130dB. Sounds rather arbitrary. A good amplifier design is (more or less) insensitive to the tolerances of the active components. So the accuracy or inaccuracy of the models doesn't matter that much, that is, as long as the sources of distortion are quantitatively modeled between reasonable limits.
Cheers,
Edmond.