Free electronics simulation software - Page 2

Do you have a question? Post it now! No Registration Necessary

Translate This Thread From English to

Threaded View
Re: Free electronics simulation software


Kevin,

I downloaded CircuitLogix last night and there is a VHDL function as well as
PCB export.  Look in the Help file and select "PCB export".  I have Multisim
8 (which I paid $600 for and it is garbage).  Someone was mentioning LTSpice
was better than CircuitLogix, which is quite hilarious.  LTSpice looks like
it was designed by high school kids.  I guess LTSpice is ok if you are
designing really simple circuits or if you don't know much about electronics.
CIrcuitLogix is the real deal.  How they are making money from it is a
mystery, since they give it away for free.  But I don't care.  Free is good.

Jerry

Kevin wrote:
Quoted text here. Click to load it


Re: Free electronics simulation software



snip

Quoted text here. Click to load it

Because they sell it for $249 Jerry.

Ian

Re: Free electronics simulation software


I downloaded the software and my wallet still has the same amount of money as
before I did the download, so I don't see how it cost me $249.  

I understand that there is a full version for $249 with even more bells and
whistles, but what I downloaded for free from the CircuitLogix site is better
than what I paid Multisim hundreds of dollars for last year.  The free
download is great.  Don't be a party-pooper, Ian.  The best things in life
are free.

Jerry

Ian Bell wrote:
Quoted text here. Click to load it


Re: Free electronics simulation software



Quoted text here. Click to load it

Because you downloaded the student edition with a restricted licence.


Quoted text here. Click to load it

I agree. LTSpice is full featured and completely free.

Ian


Re: Free electronics simulation software


Quoted text here. Click to load it

In one simple sentence, you have successfully proven that you know nothing
about simulators.

-Chuck

LTSpice is a slight variation on the spice used by the chip designers at
Linear Technology... one of the most highly regarded linear IC manufacturers
in the world.

Re: Free electronics simulation software


That's nice.  How's your job at Linear Technologies going.  Did they give you
a raise for your posting?



Chuck Harris wrote:
Quoted text here. Click to load it


Re: Free electronics simulation software


Quoted text here. Click to load it

Oh, you're the smart one!

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

-Chuck

Re: Free electronics simulation software


Quoted text here. Click to load it

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.


Re: Free electronics simulation software


Quoted text here. Click to load it

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

Re: Free electronics simulation software


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:
Quoted text here. Click to load it
you
Quoted text here. Click to load it


Re: Free electronics simulation software


Quoted text here. Click to load it

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



Re: Free electronics simulation software


Quoted text here. Click to load it

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
snipped-for-privacy@anasoft.co.uk
We've slightly trimmed the long signature. Click to see the full one.
Re: Free electronics simulation software



Quoted text here. Click to load it

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.


Re: Free electronics simulation software


Quoted text here. Click to load it


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.



Re: Free electronics simulation software


Quoted text here. Click to load it

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.

Quoted text here. Click to load it

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


Re: Free electronics simulation software


Quoted text here. Click to load it

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
snipped-for-privacy@kevinaylward.co.uk



Re: Free electronics simulation software


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


Re: Free electronics simulation software


Quoted text here. Click to load it


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: http://www.intusoft.com/models/MCNC.zip


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.



Re: Free electronics simulation software


Quoted text here. Click to load it

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


Quoted text here. Click to load it
 



Re: Free electronics simulation software


Quoted text here. Click to load it

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
snipped-for-privacy@kevinaylward.co.uk



Site Timeline