LTspice vs ngspice: Why Do I Get Different Results With the Same Netlist?

Hi Everybody.
I'm trying to do a comparison about two different simulations softwares: LTSPice and ngspice, both free.
The main problme is that I was able to make a compatible file that works on both the systems, but I got pretty different results form the simulation. Note that the simulation specifications are inside the file.
Here is the file used:
[code]
*** Component Net List Start ***
*Q_Q1 Net_0 Net_1 Net_6 2N4401 1 IC=0, 0 Temp=25
*Q_Q2 Net_2 Net_3 Net_4 2N4401 1 IC=0, 0 Temp=25
Q_Q1 Net_0 Net_1 Net_6 2N3904 1 IC=0, 0 Temp=25
Q_Q2 Net_2 Net_3 Net_4 2N3904 1 IC=0, 0 Temp=25
R_R1 Net_1 Net_5 47K
R_R2 Net_0 Net_5 47K
R_R3 Net_2 Net_5 1K
R_R4 Net_3 Net_5 47K
C_C1 Net_0 Net_3 22uF IC=0
C_C2 Net_2 Net_1 22uF IC=0
V_B1 Net_5 0 DC=5 AC=0 0
D_LED1 Net_6 0 D1N4148 1 IC=0 Temp=25
D_LED2 Net_4 0 D1N4148 1 IC=0 Temp=25
.model 2N4401 NPN(Is=26.03f Xti=3 Eg=1.11 Vaf=90.7 Bf=4.292K Ne=1.244
+ Ise=26.03f Ikf=.2061 Xtb=1.5 Br=1.01 Nc=2 Isc=0 Ikr=0 Rc=.5
+ Cjc=11.01p Mjc=.3763 Vjc=.75 Fc=.5 Cje=24.07p Mje=.3641
+ Vje=.75 Tr=233.7n Tf=466.5p Itf=0 Vtf=0 Xtf=0 Rb=10)
.model 2N3904 NPN(Is=6.734f Xti=3 Eg=1.11 Vaf=74.03 Bf=416.4 Ne=1.259
+ Ise=6.734f Ikf=66.78m Xtb=1.5 Br=.7371 Nc=2 Isc=0 Ikr=0 Rc=1
+ Cjc=3.638p Mjc=.3085 Vjc=.75 Fc=.5 Cje=4.493p Mje=.2593
+ Vje=.75 Tr=239.5n Tf=301.2p Itf=.4 Vtf=4 Xtf=2 Rb=10)
.MODEL D1N4148 D(IS=0.1P RS=16 CJO=2P TT=12N BV=100 IBV=3.867E-10)
*.TRAN 0s 100s 0.1s
.TRAN 0.1s 50s
[/code]
I attached the two simulated results , both on net_0. I'm pretty new to this kind of simulations, so I'm asking advices here about why this different results, thanks in advance!

Too Bad Bob Pease is not around to coach you on this. Read the EDN archives for his opinion on SPICE.

Many thanks for the advice! I, I totally think that Pease was right in his true diffidence about the numerical simlations... still... I'm puzzled by the big difference I have from two simulators... this add a third option to the two already on the board... first right, second right.... both wrong... not a bad way to proceed.

When you say totally different results, you don't show the results, please see what you can do for that.

Here is possible root cause and you will find this with same netlist on same simulator, is the simulator options. For instance reltol, max step time, nin step time, these are just a few but can have dramatic differing results depending on the circuit.

You must compare those. Also these propritory simulators have done things to the mathematical algorithms to get them to converge. I have not seen one easily converge attempt get the best accuracy so they are willing to sacrifice accuracy for convergence, which would send you on to the competion's simulator out of frustration (this is serious , but it's a market driven simulator requirement)

After all these simulators are't putting rovers on Mars, serious expensive simulators are, You get what you pay for,

I know the guy from LT who developed LTSpice, not that it make me the expert, and it's good stuff for free stuff. Get youself a free Berekely compliant simulator no bells & whistles, but accurate.

Thanks for your reply and good suggestion... since I never used these simulators I'm still on my way learning them and yes, I think that may e right....
For the result part, I have attached in the first post the plots I get from the simulation. Should I add the raw generated results too?
right now I'm more propense in beleaving that LTSpice is the "right one", but still, I would like to perfor digital and mixed simulations, and as far as I know that part is almost totally idealized on LT side.

I'm no expert, but in my attempts to run simulations, it because clear that there's a trade-off between accuracy and speed. The sample rate (step vs interval) needs to be faster than the frequency of detail you want to see, otherwise what you get is aliasing patterns and the like. You have to be at, at least, twice the highest frequency and I would suggest at least 5 to 10x..

One way to compensate for the extra processing time, is to limit the simulation duration to the minimum needed to get a meaningful result -- in the first of your diagrams, there is considerable repetition. By running the simulation for say 3 seconds instead of 50s, you will speed it up considerably (or get finer resolution for the same time cost).

Yes but simplistic. First you must be past the initial transient if you want say steady state. The you choose to start taking data and then only say 10 cycles if this is a switched event.

This allows you to drill down to nano second events. You also limit probes, probe data takes time to write as. But again you can only do this if you already looked at the sim over the complete transient otherwise you are just guessing on where to drill down.

If you are interested in the complete transient then you should up reltol to say 0.01, something like that. Then you have to choose max step time and min step time. Having done this you loose granularity but you can get a reasonable idea of overall transient.

Remember steady state is only a snap shot in the transient space so that is where you want granularity & accuracy.

Like I commented on, same net list, same simulator can yield very different results depending on sim options, loose vs tight.

Which one to choose? You have to virtually know the answer before you start. But once you have baselined it, then you have a point of reference.

Sorry but this is the nature of simulations. You must validate the results and explain any deviations from real world results.

Thanks for the suggestion. To be honest I have to admit that wht you point out was my fault. I mean, I forgot to specify in the main thread that I indeed performed the same analysis on both the software (same file with the simulation parameters inside), but then I presented here only the zoomed version to shwon the behavior of LT spice respect to the oneshwon by ngspice, Still you are right on your point, but I was unable to get comparable results also looking for that kind of parameters....

Here is what you miss perhaps. Just because you see tolerance and sim options appear the same doesn't mean everything that represent these are the same in the sense the mathematical algorithm are the same, they are not.

If both simulators were exact in how they got the answer and both were given the same netlist, then the results would be the same, that simple.

You are beating your head against the wall when all you need to do is figure out which one is accurate and forget the other one.

This is why I suggest get hold of a free SPICE simulator that is compliant with the latest Berkeley SPICE and use that as the bench mark. Then deal with this is that free Berkeley version usually are text driven and likely have no GUI, but your netlist is so simple that shouldn't be an issue.

Again use a Berkeley compliant simulator and see which of the others has the best match, and forget why there is a difference. I have explained why they have inaccuracies.

Good luck!

Well, I think I start to get something. The circuit I presented here should not work, clearly. In Its theory of operation, R2 and R3 shoyuld be the same. I sude the simulation trick to see what happen if that condition is not met. Configuring thetwo values to be the same, I got "comparable results" on both the simulation enviroments, still some differences on the initial transient. Now at least I know that in "good conditions" the simulators produce comparable results. Now, on the why the simualtions for the wrong operation modes are different, well, that is another story... For that I suspect the reasong are quite different mathematical approach to the solving mechanism .
By the way, NGspice is a spoice3f5 compliant simulator.

Thanks for your kind support, if I should have some news I'll post them here.
Thanks again everybody