Free electronics simulation software

Oh, you're the smart one!

I have never worked for LT, but I do use LT's parts, and LTSpice.

-Chuck

Reply to
Chuck Harris
Loading thread data ...

Then you should understand that LTSpice only does analog simulation. A real simulator does mixed-mode (digital and analog). Have fun with your toy simulator.

Reply to
Kevin

A real simulator? Spices are analog simulators by nature.

I'm having difficulty understanding why you would want to throw digital in with an analog simulation.

Do tell!

-Chuck

Reply to
Chuck Harris

Unlike SPICE, which is designed mainly for analog simulation, mixed-mode simulators such as Multisim and CircuitLogix include both analog and event- driven digital simulation capabilities in the same executable. This means that any simulation may contain components that are analog, event driven (digital or sampled-data), or a combination of both. An entire mixed signal analysis can be driven from one integrated schematic. All the digital models in mixed-mode simulators provide accurate specification of propagation time and rise/fall time delays.

The event driven algorithm provided by mixed-mode simulators is general purpose and supports non-digital types of data. For example, elements can use real or integer values to simulate DSP functions or sampled data filters. Because the event driven algorithm is faster than the standard SPICE matrix solution simulation time is greatly reduced for circuits that use event driven models in place of analog models.

Mixed-mode simulation is handled on three levels; (a) with primitive digital elements that use timing models and the built-in 12 or 16 state digital logic simulator, (b) with subcircuit models that use the actual transistor topology of the integrated circuit, and finally, (c) with In-line Boolean logic expressions.

Exact representations are used mainly in the analysis of transmission line and signal integrity problems where a close inspection of an IC?s I/O characteristics is needed. Boolean logic expressions are delay-less functions that are used to provide efficient logic signal processing in an analog environment. These two modeling techniques use SPICE to solve a problem while the third method, digital primitives, use mixed mode capability. Each of these methods has its merits and target applications. In fact, many simulations (particularly those which use A/D technology) call for the combination of all three approaches. No one approach alone is sufficient.

Chuck Harris wrote:

you

Reply to
Kevin

FYI, just as many (perhaps even most, albeit with LTSpice as one significant exception) commercial SPICEs are based on the original Berkeley source code, many mixed analog/digital simulator (including your Multisim, Kevin Aylward's SuperSPICE, etc.) are based on the XSPICE source code from Georgia Tech. And just as there are plenty of free "analog" SPICEs around, there are also plenty of free XSPICEs around as well.

However, I would grant you that the commercial simulator industry was already very much alive and kicking by the time XSPICE was released, and there are a lot more "nicely polished" analog SPICEs that happen to be free than there are nicely polished mixed-signal SPICEs.

Of course there are plenty of other ways to do mixed signal simulation as well...VHDL-A has significant support commercially.

---Joel

Reply to
Joel Kolstad

This all depends on what you want to do with the simulator. There are markets for both mixed-mode and a better pure analogue.

Although I agree that LTSpice's GUI, is a bit lacking, well a lot lacking actually, it has features that for quite a few applications, make it a number one choice. I say this, despite flogging my own mixed-mode bit of kit.

LTSpice is probably about the best converging spice on the market, and runs around 3 times as fast. In my day job, I routinely run very long simulations on high transistor count designs, and having something done in 1/2 day verses two days would be a great bonus.

As far as "real" mixed-mode simulator goes, unless it integrates with the Cadence suite, its pretty much useless. I don't see much of a professional market for mixed-mode design outside of SoC i.c. design.

--
Kevin Aylward
ka@anasoft.co.uk
 Click to see the full signature
Reply to
Kevin Aylward

JerryG wrote: : Eagle, LTSpice, and TINA? What is this......Losers anonymous? Those are the : three worst simulators that have ever been built. At least LTSpice has the : excuse that they are not really a simulation product since they sell hardware. : But LTSpice and TINA? Give me a break. Why even post messages when you have : no clue about simulation software. Stay in school for a few more years and : then get a job and then post messages. Until then you are just taking up : valuable space.

*chuckle*

I'll be interested in your ranting when you post some benchmark results comparing CircuitL*gix run times to LTSpice's. Also, please post some *reasons* about why CircuitL*gix is better than LTSpice -- besides the purported VHDL ability, which doesn't even appear on their website as far as I could tell.

Otherwise, you're just another CircuitL*gix shill, and a cranky one at that.

Meanwhile, for educators looking for simulation software: consider the full range of freeware and open-source options, including CircuitL*gix. But remember why the different closed-source freeware simulators are out there: most of them are some attempt at vendor lock-in.

I'll now leave this thread unless one of you CircuitL*gix guys has something quantifiable to say.

Stuart

Reply to
Stuart Brorson

The only shill in this discussion is you, Stuart. You seem to have some weird obsession with LTSpice, which is a nice little simulator if all you want to do is analog simulation. At least CircuitLogix and Multisim provide mixed-mode simulation, which is what real designers require. Why you are afraid of a free simulation product is strange, to say the least.

--
Message posted via ElectronicsKB.com
http://www.electronicskb.com/Uwe/Forums.aspx/cad/200704/1
Reply to
JerryG via ElectronicsKB.com

Because you downloaded the student edition with a restricted licence.

I agree. LTSpice is full featured and completely free.

Ian

Reply to
Ian Bell

Wow. I had no idea I wasn't a real designer.... Thanks for clearing that up

Steve

Reply to
Steve

In testing simulators, we ran some SPICE netlist tests on LTSpice, PSpice and Microcap. We had heard all the hype about LTSpice but the simulation speeds in most of the netlists was a good deal slower than both PSpice and Microcap. We were not running simulations with their enhanced Linear models but just a few general circuit files though. Perhaps if you use the SMPS capability with the Linear models, then it is a fast simulator, or we just fluked into a few circuits that LTSpice has problems with. Was not impressive though. Great price however.

Reply to
engr4fun

"engr4fun" schrieb im Newsbeitrag news: snipped-for-privacy@r35g2000prh.googlegroups.com...

Hello eng4fun,

Have you considered the number of steps caculated in ".tran" and the default settings about accuracy?

I am interested in your test circuits to for my own benchmarking. Can you send me one of your test cases?

Best regards, Helmut

PS: I am not an employee of LTC if that matters.

Reply to
Helmut Sennewald

This is at odds with pretty much all prior benchmarks reported in this NG and my own test runs, so I am major sceptical.

So... for example, did you manually try and set LT minimum time steps? Doing so is not recommended. It will usually slow it down significantly. LT wants to be run on automatic settings.

--
Kevin Aylward
ka@kevinaylward.co.uk
Reply to
Kevin Aylward

Unfortunately, I think we were testing proprietary circuits since we of course wanted to see how these simulators acted with our types of circuits. They may have also tested some other netlists as well. I'll check with the guy who ran all of these.

We kept all of the simulators on their default settings. The Maximum Time Step was typically set in the .tran statement.

Reply to
engr4fun

The point here is that you don't want to do that in LTSpice. It makes a BIG difference to the speed. .tran for LT should just be how long you want it to run for. If you specify a default time step as well it will override LT's algorithm. Considering that halving the number of points will half the simulation time, a good time step algorithm is crucial.

--
Kevin Aylward
ka@kevinaylward.co.uk
Reply to
Kevin Aylward

Helmut,

I tried to post this information previously but it doesn't seem to have taken. My coworker tried one more circuit from the list since then.

We can't provide the original circuits we used, but we found some on the web called MCNC which are supposed to be SPICE benchmark circuits. The three simulators tested were PSpice Ver 9, Micro-Cap 9, and LTSpice 2.20k. I know PSpice is an older version but the guys who use it love it and don't want to upgrade to the creature that Cadence has created. Both PSpice and Micro-Cap are professional versions not student versions. For the system we did this on, both Micro-Cap and LTSpice were fresh installs so everything was defaulted. We set PSpice back to its default conditions as best we could. We chose circuits randomly from the set while ignoring the huge ones since we can't put too much time into this. In each simulator, we just loaded the circuit and simulated. That's all. The results were:

SQRT.CIR PSpice - 100.98s Micro-Cap - 99.06s LTSpice - 207.046s

AROM.CIR PSpice - 8.11s Micro-Cap - 4.41s LTSpice - 10.25s

ADD32.CIR PSpice - 609.53s Micro-Cap - 868.70s LTSpice - 1917.749s

MUX8.CIR PSpice - 15.06s Micro-Cap - 7.52s LTSpice - 15.25s

I must be missing some setting to change in LTSpice but this is how it installs.

Alex

Reply to
engr4fun

"engr4fun" schrieb im Newsbeitrag news: snipped-for-privacy@r3g2000prh.googlegroups.com...

Hello Alex,

There is a default setting of trtol=7 for PSPICE and Micro-Cap. LTspice has the more precise default setting trtol=1. LTspice will run about two times faster if trtol is rised from 1 to 7. If I divide your numbers by this factor, LTspice looks as fast as PSPICE and Micro-Cap

Please add the following SPICE-line to the netlists for a comparable result.

.options trtol=7

I tried the same netlists on my PC with LTspice. AMD64-4000+(2.4GHz), 2GB Benchmark files:

formatting link

SQRT.sp trtol=1 142.3sec trtol=7 70.2sec

AROM.sp trtol=1 4.8sec trtol=7 2.1sec

ADD32.sp trtol=1 1110sec trtol=7 768sec trtol=6 706sec trtol=5 720sec

MUX8.sp trtol=1 7.3sec trtol=7 3.7sec

Best regards, Helmut

PS: I don't expect it would be faster with a 2.4GHz Core-2 Duo.

Reply to
Helmut Sennewald

"Helmut Sennewald" schrieb im Newsbeitrag news:f0u0p2$9a0$01$ snipped-for-privacy@news.t-online.com...

Hello again,

An additional cshunt-capacitance avoids numerical problems with hyper-fast unreralistic transitions. Just think of it as a fraction of the wiring capacitance. trtol=7 cshunrt=1f

-> 605sec

Now we are back at about this factor 2 in speed compared to trtol=7.

Best regarsd, Helmut

Reply to
Helmut Sennewald

There is a reason for trtol=1 not 7! I get the same sort of speed up in my XPSpice with trtol=7, however, I have found that this setting just does not guarantee correct results in some circuits, especially my switching power supply examples in SuperSpice, so I also have it defaulted to trtol=1. Its not just an inaccuracy, its can give fundermenatlly wrong results. Even trtol=2 is not enough for some circuits.

I would like to see the benchmarks run with trtol=1 for all simulators see what the results are.

--
Kevin Aylward
ka@kevinaylward.co.uk
Reply to
Kevin Aylward

Hello Kevin,

I tried today in the office three of the benchmarks with PSPICE on a C2-PC. benchmarks:

formatting link

TRTOL PSPICE-C2 LTspice-C2 LTspice-AMD64 AROM 7 3.84 2.53 2.1 AROM 1 10.26 5.84 4.8 MUX8 7 6.83 4.67 3.7 MUX8 1 14.36 9.27 7.3 SQRT 7 49.08 53.67 70.2 SQRT 1 118.53 108.22 142.3

C2: Intel Core2-Duo 2.33GHz (Xeon) AMD64: 4000+, socket 939

PSPICE 10.2 LTspice 2.20k

My conclusion is that LTspice is at least as fast as PSPICE and MC-SPICE. I expect each of the three simulators will win in a few benchmarks and overall LTspice will reach a good position in this race.

Best regards, Helmut

PS: It's necessary for PSPICE to remove the character # in the names used in the circuit files and to change the file names to ".cir". LTspice doesn't require any change.

formatting link

Reply to
Helmut Sennewald

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.