Re: Strange behavior for simple RC circuit
On Sat, 13 Jul 2013 23:01:59 -0400, Julio wrote: I am looking at simple RC circuit with a time constant of 1 sec and a 6 V
battery.
Doing a transient analysis, at t=0 the capacitor is already fully charged
at 6.0 volts!
I don't recall giving initial conditions for the cap, so if I did not
shouldn't the cap start
In a fully discharged state? Look at the .tran card (it's on the schematic.) Right click it and look near the bottom of the dialog box to find "skip initial operating point solution" and check it so that this step will be skipped. Then re-run the solution. Jon
|
Strange behavior for simple RC circuit
I am looking at simple RC circuit with a time constant of 1 sec and a 6 V
battery.
Doing a transient analysis, at t=0 the capacitor is already fully charged
at 6.0 volts!
I don't recall giving initial conditions for the cap, so if I did not
shouldn't the cap start
In a fully discharged state?
Sincerely,
Julio
|
Re: different resistance for .tran and .ac not working any more?
--- In LTspice@..., "haubmi1" <Michael.Haub@...> wrote:
--- In LTspice@..., "Helmut" <helmutsennewald@> wrote:
--- In LTspice@..., "haubmi1" <Michael.Haub@> wrote:
Hello,
there was a feature to have a resistor with different value for .ac and .tran .
e.g.:
R 1 2 1u AC 1Gig
That was a resistor that was 1uOhm in .TRAN and 1GOhm in .AC.
This does not work anymore?
That was a very handy feature to switch in a loop gain probe in .AC which is not fisible in .TRAN .
Was this feature removed by accident or is that intended?
Did the syntax change?
Or is it my error?
michael
Hello Michael,
It's still working. Trust me.
Please show me your example and I will repair your schematic.
Best regards,
Helmut
Hello Helmut,
i have uploaded Files>Temp>loopgain-probe-test.zip.
I don't know what was the exact problem as a similar spice desk at work did not run as expected. Here at home the loop-gain probe did run in the new spice desk i made, but only with the alternate solver.
If you like you can have a look at it and tell me why it needs the alternate solver for DC bias point.
I will check on Monday why it did not run correctly at work.
Cheers,
Michael
Hello Michael, You have used resistance values of 1f. That's a very bad idea. Change it to 1u and the simulation will run with the normal solver. Lesson from today: never use femto-Ohms. .subckt simple-openloopgain1 in out params: reakt=100Gig L1 in out {reakt} Rser=0 C1 2 1 {reakt} Rpar=0 R1 in 2 100G AC 1u R2 out in 1u AC 100G V1 1 0 0 AC 1 .ends simple-openloopgain1 Best regards, Helmut
|
Re: Help! How do I do find maximum signal easily!
hmmm...maybe I was too quick to dismiss this IF I use three 'different' text files, one for each analysis type, then bounce between them! Now if there is just some way to include the the command strings: 'file' 'export' select style of output, overwrite, yes is there a way to add command strings like this?? If so, you have REALLY automated this for me! --- dwh@... wrote: From: David Hawkins <dwh@...> To: LTspice@... Cc: Macy <macy@...> Subject: Re: [LTspice] Re: Help! How do I do find maximum signal easily! Date: Fri, 12 Jul 2013 16:07:44 -0700 [snip] and the .ac using specific values requires storing on the
schematic a list so long that it makes the schematic the size of a
postage stamp in auto size. perhaps a plus sign on the first of a few
lines will allow wordwrap - narrow width with long list. Why not put all the relevant text into file, and then .include it. It makes the schematic look nicer, and allows you to add header comments to the file along with relevant comments throughout the file. Cheers, Dave
|
Re: arbitrary solar cell model
--- In LTspice@..., "analogspiceman" <analogspiceman@...> wrote: There is no problem with LTspice. It is faithfully calculating
the original poster's extremely ill formed diode equations to Huh? It's just the standard diode equation, as taught in every elementary device course. It may not be the best way to do what the OP is trying to do, but it seems quite reasonable to me to expect that it should give a reasonable answer. After all, spice solves this exact equation in maybe a majority of the active circuit it simulates, maybe for a dozen elements at a time, why should one expect that it can't handle it in a dependent source? To call this "extremely ill-formed" seems quite hyperbolic. These sorts of content-free, bullying responses make me think the bully is trying to avoid intelligent discussion by intimidation. Sorry I don't react well to that, and I really expect better from this forum. [/rant] The trouble arises from taking the ratio of two exponential
expressions that both may grow to very large values. Not really, the exp() in the denominator is constant, and a reasonable value (e**21.7 is well in range of even single-precision floats), it just modifies the constant Visc multiplier to provide the correct open-circuit voltage. The case where things fail is when the input is negative so nothing should blow-up. The "very large" values occur with positive voltages where everything works fine. However you are certainly correct that LTspice seems to be launching itself off the end of its numerical range, ending up with a solution that is completely unrealistic yet the simulator does not recognize that this has happened. Look at the circuit when Vout is negative. The Bidiode source becomes a very low-value current source, with very low incremental conductance. It is in parallel with two high-conductance linear resistors. The Rs dominate what is happening in this regime, why on earth would spice feel the need to drive the voltage at that node so far negative that it wraps around? The circuit is very well-behaved in this range but somehow spice goes off the deep end. I'd have more sympathy if the sim failed at higher voltages when the B source had a significant dI/dV, not where the element is basically out of the circuit. Or if there were no resistors in the circuit so the dV/dI might blow up, but that's not the case either. As more proof that something odd is going on, why does this problem go away when the Voc voltage is changed from an expression of constant inputs to a pure constant? There is no reason the solver should be perturbing the constant inputs to that equation, but apparently it is. This also works fine in a transient analysis if one starts the independent sources at 0, but not otherwise. This raises the question: does LTspice try to solve things like this with some higher-level approach than an incremental analysis? Symbolic analysis? I'm at a loss. lead to numerical clipping, which LTspice handles well without crashing Nice that it doesn't crash, but it is wrong to claim a valid solution when this happens, and worse that it uses this bizarre state as the starting point for the next iteration. At the very least make a mention of this in the error log. I'd prefer it recognize that the clipping (wrap-around, I think) has occurred and at least flag that it can not find a solution, as it does in many other situations, or try a different approach like it does for a difficult operating-point. As an experiment I converted the exponential current source into a logarithmic voltage source. Spice had even more trouble solving that at low voltages (not terribly surprised) but at least it recognized that it could not find a solution and moved on to the next point. Once it found a real solution it was fine from there on. but the clipped value causes the ill formed equation to have two solutions I'd understand that if the equations had two solutions, stable or not, but they do not. What it reports is not a solution at all, KCL is not remotely satisfied at the reported "solution," there are a zillion Amps flowing out of that node from both the diode and the voltage source, and only 9 Amps flowing in. But somehow 73MAmps is within tolerance of 1.#INDA Amps, whatever that is. Latching onto the clipped solution can be avoided either by turning
the input source, V1, upside down so that the approach is from the
favorable direction, or by limiting the expression for BIdiode to
only positive values by wrapping its expression within a uramp()
function (or some other suitable limiter). The first option doesn't help the OP, but the second is a simple fix that seems to work well. I put the uramp() inside the exp() rather than outside and everyone's happy. Why this works when all it really does is add a discontinuity to the dI/dV is well beyond me. It is always best to use the built in devices whenever possible
because their internal expressions will always have be manipulated
to be as well formed as possible. I agree completely, and you'll see I still recommend that in my responses, but this bothers me anyway because I like to think of LTspice as a general-purpose nonlinear equation solver and here is a simple case of well-behaved equations yet it both fails misesrably and fails to recognize that it failed miserably (I have to think of the original Star Trek episode with "Nomad," once it realized it had made a mistake and, worse, failed to correct its mistake it had to self-destruct. I'm not advocating that behavior for LTspice). Cheers, sorry for the rambling, have a great weekend all, Fred
|
A couple of programs that were nodal analysis (net list only entry) on mainframe computers that were precursors to SPICE. Namely ICAP (IBM Circuit Analysis Program) and then PCAP (Princeton Circuit Analysis Program).
Regards, (9V1MI, WN8P) Larry
|
Re: arbitrary solar cell model
Hi Hamed,
I still recommend using the standard diode elements instead of writing your own, the only reason you would not be able to do that is if you need to change the Temperature -during- a transient simulation, e.g. I think everything else (irradiance/Isc) can be adjusted dynamically, and you can have multiple cells in any topology, all with different temperatures and Isc. Temperature can be swept for one/multiple/all devices in an Operating Point solution if that's what you need.
If you still think this does not meet your needs please state what you have to do that you can't do with the standard model and I can show you how to fix your equations so that it works. Whether it's reasonable or not LTspice can not handle your equations as you have written them, but it can be fixed.
-Fred
toggle quoted message
Show quoted text
--- In LTspice@..., "qrx3" <fredh@...> wrote:
Hello Hamed,
I had a chance to look at this a bit more closely, and I do think LTspice is having a problem with this circuit that it should not have. I have created a simpler version of your circuit, in schematic form, and placed it in the Temp directory. The file is "BadExp.asc." If you run it as-is the simulator fails to find a reasonable solution, voltages and currents that should be in the single-digits are in the 100ks or Megs, not where they should be. However if you change the simulation command to start the DC sweep at 0V instead of -1V it works fine. This is what I saw with your circuit too, I think having two cells in series might have caused the simulator, at some point in its search, to have a negative voltage on one of the cells, and everything blew up. It seems that LTspice tries to use the results of each iteration to start the next iteration, so once it's gone off the rails it stays there. But it really shouldn't be having any problem calculating the solution with negative input voltages.
Another way to 'fix' the problem is to force the B-source for Voc to a constant value of 0.564V. This is odd since even when the sim fails that B-source has that correct value on it, while the Bidiode source blows up.
I have sent this circuit and observation to Mike @ LT, I'll report back here when I hear from him.
--- In LTspice@..., "hamed" <l0st_l0rd@> wrote:
the reason that I use arbitrary model not a standard diode is that I cannot control temperature change for each solar cell in diode model. But as you've been told this is not true. You -can- control the temperature independently for each instance. What's more, the standard model will have the correct temperature dependence while you already know that your equations do not calculate Voc correctly over temperature.
--- In LTspice@..., "hamed" <l0st_l0rd@> wrote:
Furthermore, the reason that grounds are different is that two cells are in series. Yes, I understand why you want your model to float so you can connect them without reference to ground, but as I said you did not implement this correctly. Your formulas for Voc and Isc are referenced to the 'ref' node but then when you use those values in the subsequent calculations you are using their value relative to ground. This is wrong.
Actually I should say that I am not so good in schematics environment and I am used to netlists while I can control the nodes easier. You should give it a try, with very little practice I think you will find that it's actually much easier to keep track of what nodes are connected where by looking at the schematic than it is by reading a large netlist. I suggest again that you might not have made the errors with the signal references if you had used a schematic instead of a netlist.
Best,
Fred
--- In LTspice@..., "qrx3" <fredh@> wrote:
Hello Hamed,
While I would also advise you to use a standard diode model instead of building your own, I may be able to shed some light on your difficulty.
Note that your derived values for ISC and VOC are generated in relation to the reference input 'ref'. However when you use these values in your formulae you are using the value relative to ground:
log((v(isc)/{i0})+1)
The same is true when you use the input voltage:
(v(inp)*iscr)/1000)
I have not tried to run your circuit, but I strongly suspect this is why it would work for a single cell where ref = ground and not for a second cell where ref != ground.
I think the most sensible fix would be to reference eisc and evoc to ground instead of ref, so you can observe the values externally if you want and not have to subtract the ref voltage. Then change "v(inp)" for example to "v(inp,ref)" where needed.
I suggest that if you had drawn this as a circuit instead of writing a netlist these issues would have been quickly apparent, but maybe not.
Cheers,
Fred
--- In LTspice@..., "hamed" <l0st_l0rd@> wrote:
Dear friends
in the file below you can find an arbitrary solar cell.
When I put two cells in parallel the answer is correct and when I put them in
series I see a distortion.
I think the problem is related to the diode behavioral model.
I will be thankful if any of you could help me.
sincerely,
Hamed
|
Re: different resistance for .tran and .ac not working any more?
--- In LTspice@..., "Helmut" <helmutsennewald@...> wrote:
--- In LTspice@..., "haubmi1" <Michael.Haub@> wrote:
Hello,
there was a feature to have a resistor with different value for .ac and .tran .
e.g.:
R 1 2 1u AC 1Gig
That was a resistor that was 1uOhm in .TRAN and 1GOhm in .AC.
This does not work anymore?
That was a very handy feature to switch in a loop gain probe in .AC which is not fisible in .TRAN .
Was this feature removed by accident or is that intended?
Did the syntax change?
Or is it my error?
michael
Hello Michael,
It's still working. Trust me.
Please show me your example and I will repair your schematic.
Best regards,
Helmut
Hello Helmut, i have uploaded Files>Temp>loopgain-probe-test.zip. I don't know what was the exact problem as a similar spice desk at work did not run as expected. Here at home the loop-gain probe did run in the new spice desk i made, but only with the alternate solver. If you like you can have a look at it and tell me why it needs the alternate solver for DC bias point. I will check on Monday why it did not run correctly at work. Cheers, Michael
|
Re: Help! How do I do find maximum signal easily!
[snip] and the .ac using specific values requires storing on the
schematic a list so long that it makes the schematic the size of a
postage stamp in auto size. perhaps a plus sign on the first of a few
lines will allow wordwrap - narrow width with long list. Why not put all the relevant text into file, and then .include it. It makes the schematic look nicer, and allows you to add header comments to the file along with relevant comments throughout the file. Cheers, Dave
|
In message <krpvc7+8b3g@...>, dated Fri, 12 Jul 2013, Helmut <helmutsennewald@...> writes: The point isn't whether it's Fahrenheit or degree. It's about stealing knowhow. I know: I heard the story before, in a company seminar on NOT giving away know-how. Translating 830 degrees to the cooking oven scale was just another of my weak jokes. -- OOO - Own Opinions Only. See www.jmwa.demon.co.uk Why is the stapler always empty just when you want it? John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK
|
Hello John,
The point isn't whether it's Fahrenheit or degree. It's about
stealing knowhow.
Best regards,
Helmut
toggle quoted message
Show quoted text
--- In LTspice@..., John Woodgate <jmw@...> wrote:
In message <krpsf9+e62p@...>, dated Fri, 12 Jul 2013, Helmut
<helmutsennewald@...> writes:
And so I got on the phone and called down to Fab 3 over at Intel and I
said what temperature are the ovens at and they said 830 degrees. I guess that's Fahrenheit - Gas mark 23 (not in Germany, which has
bigger marks!).
--
OOO - Own Opinions Only. See www.jmwa.demon.co.uk
Why is the stapler always empty just when you want it?
John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK
|
In message <krpsf9+e62p@...>, dated Fri, 12 Jul 2013, Helmut <helmutsennewald@...> writes: And so I got on the phone and called down to Fab 3 over at Intel and I said what temperature are the ovens at and they said 830 degrees. I guess that's Fahrenheit - Gas mark 23 (not in Germany, which has bigger marks!). -- OOO - Own Opinions Only. See www.jmwa.demon.co.uk Why is the stapler always empty just when you want it? John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK
|
Re: Help! How do I do find maximum signal easily!
still requires a LOT of fussing around. bouncing between wide band .noise and 'regular' .ac analysis and the .ac using specific values requires storing on the schematic a list so long that it makes the schematic the size of a postage stamp in auto size. perhaps a plus sign on the first of a few lines will allow wordwrap - narrow width with long list. getting an output requires click file, export, then select real, imaginary ofrmat, and then YES overwrite existing *.txt file. Then run a script in octave to grab all the data, do the conversion to something meaningful and evaluate whether I did what I wanted to. But, other than all this mucking about, I CAN get my answers!! whew! it gets me there. --- Andrew.Ingraham@... wrote: From: Andy <Andrew.Ingraham@...> To: LTspice@... Subject: Re: [LTspice] Re: Help! How do I do find maximum signal easily! Date: Fri, 12 Jul 2013 12:35:43 -0400
Thanks! a lot of work, but it will get me by for awhile.
I'm puzzled, because this seems like exactly what you were looking for. Isn't it? I don't think it could be much simpler. You can probably avoid the "dB" by setting up your AC plot with a linear Y axis. Andy
|
Hello Howard,
I like especially this part of the story below.
... And she said well why don't you call Fab 3 over at Intel and
ask them what the temperature is. And so I got on the phone and
called down to Fab 3 over at Intel and I said what temperature
are the ovens at and they said 830 degrees. And I said thank you.
Best regards,
Helmut
toggle quoted message
Show quoted text
--- In LTspice@..., Howard Hansen <hrhan@...> wrote:
Thanks for posting the links. All were very interesting.
Howard
On 7/12/2013 2:51 PM, Helmut wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
"analogspiceman" <analogspiceman@> wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
"Helmut" <helmutsennewald@> wrote:
You will find the history of LTspice in the Slides.ppt
included in the World-Tour's zip-file. That is where I got what little information that I already have. Do
you have
more?
Regarding the LTspice code, yes it is all Mike's, but it is still very much
based on the SPICE methods in general.
Hello analogspiceman,
One of the links is about HSPICE.
Best regards,
Helmut
[Non-text portions of this message have been removed]
|
Thanks for posting the links. All were very interesting.
Howard
toggle quoted message
Show quoted text
On 7/12/2013 2:51 PM, Helmut wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
"analogspiceman" <analogspiceman@...> wrote:
--- In LTspice@... <mailto:LTspice%40yahoogroups.com>,
"Helmut" <helmutsennewald@> wrote:
You will find the history of LTspice in the Slides.ppt
included in the World-Tour's zip-file. That is where I got what little information that I already have. Do
you have
more?
Regarding the LTspice code, yes it is all Mike's, but it is still very much
based on the SPICE methods in general.
Hello analogspiceman,
One of the links is about HSPICE.
Best regards,
Helmut
|
Re: LTspice model for a 120V 4W LIGHT BULB in a Wien bridge oscillator ?
--- In LTspice@..., "ron.ck722" <ron.ck722@...> wrote:
For those interested in further simulations of low distortion Wein oscillators and Ultra-linear VCOs, here are 3 articles:
1) Anne Watson Swager, "DOS-based analog-simulation software" EDN, May 21, 1992.
2) LTC's late Jim Williams' "Max Wein, Mr. Hewlett and a Rainy Sunday Afternoon" somewhere in the Linear Technology archives. Good references to Max Wein, Bill Hewlett and Jim, himself.
3) Jim Williams' "The Zoo Circuit - History, Mistakes and Some Monkeys Design a Circuit" on Jim and his good buddy, Bob Pease's obsession with Ultra-Linear V/F converters. Also somewhere in the LTC archives.
My copies of 2) and 3) aren't dated. They may have been copied from
one of several Analog design books Jim and Bob did together.
Regards,
Ron
Hello, Please stop this thread. Best regards, Helmut I will delete further messages.
|
Re: LTspice model for a 120V 4W LIGHT BULB in a Wien bridge oscillator ?
For those interested in further simulations of low distortion Wein oscillators and Ultra-linear VCOs, here are 3 articles:
1) Anne Watson Swager, "DOS-based analog-simulation software" EDN, May 21, 1992.
2) LTC's late Jim Williams' "Max Wein, Mr. Hewlett and a Rainy Sunday Afternoon" somewhere in the Linear Technology archives. Good references to Max Wein, Bill Hewlett and Jim, himself.
3) Jim Williams' "The Zoo Circuit - History, Mistakes and Some Monkeys Design a Circuit" on Jim and his good buddy, Bob Pease's obsession with Ultra-Linear V/F converters. Also somewhere in the LTC archives.
My copies of 2) and 3) aren't dated. They may have been copied from
one of several Analog design books Jim and Bob did together.
Regards,
Ron
toggle quoted message
Show quoted text
--- In LTspice@..., "xe3po" <xe3po@...> wrote:
Hi AC2CL,
Thanks for your suggestion!
My concern is that regarding the double integrator state variable oscillator, how promising is it?
Mine oscillator gives me THD 0.03% (-70dB) while other people reportedly acheived <0.001% by simply using AD797 and a bulb.
Can the double integrator state variable oscillator get -100dB
without special tricks?
73,
xe3po
--- In LTspice@..., alzie <alzie@> wrote:
Hi Xe
The wein bridge has poor harmonic rejection.
Try the double integrator state variable oscillator.
Take the output from the 2nd integrator.
2 stages of integration Greatly attenuates harmonics.
Amplitude stability can be gotten with a Soft clipper in the summing
stage, or
you can use the usual jfet method.
Very stable / wide range.
Easy to get a decade with a stereo pot.
Switch ranges by changing capacitors.
On 05/22/2013 07:15 PM, xe3po wrote:
Thank you very much for your input!
120V 4W is the lowest rating I could find locally.
It worked, with a LM741 opamp, and yielded 6Vp-p 1000HZ
output while THD is lower than -70dB.
I just want to get a better THD result like -100dB. --
AC2CL
I do not think there is any thrill that
can go through the human heart like that felt by the inventor as
he sees some creation of the brain unfolding to success...
Such emotions make a man forget food, sleep, friends, love, everything.
- Nikola Tesla
|
--- In LTspice@..., "analogspiceman" <analogspiceman@...> wrote:
--- In LTspice@..., "Helmut" <helmutsennewald@> wrote:
You will find the history of LTspice in the Slides.ppt
included in the World-Tour's zip-file. That is where I got what little information that I already have. Do you have
more?
Regarding the LTspice code, yes it is all Mike's, but it is still very much
based on the SPICE methods in general.
Hello analogspiceman, One of the links is about HSPICE. Best regards, Helmut
|
And some of those intusoft newsletters still have some of the best model ideas for electromechanical and thermal problems.
Jim Wagner
Oregon Research Electronics
toggle quoted message
Show quoted text
----- Original Message ----- From: "Howard Hansen" <hrhan@...> To: LTspice@... Sent: Friday, July 12, 2013 12:08:26 PM Subject: Re: [LTspice] The road to LTspice On 7/12/2013 11:24 AM, analogspiceman wrote:
I am attempting to create a historical timeline of the history
of SPICE as it has grown in function, use and popularity in the
engineering community. This is to be in bullet point format and
I intended to include only those forms of SPICE that were most
ubiquitous in their time, i.e. the various Berkeley SPICEs, then
PSpice, and, of course, LTspice.
What I've got so far I will put at the end of this message. It has
errors and is not complete, especially the part about LTspice. I
am looking for corrections and input as to the major additions and
events regarding LTspice. (What additions over the years seem
especially noteworthy to you?).
I will fill in the historical dates from the Change Log and from
the group message archive. When the history is complete, I will
add it to group files as a PDF and also add it as a new section
over at the LTwiki (so there is no need to copy it just yet).
________________________________________________
THE HISTORY OF SPICE
1969 beginnings of CANCER (Computer Analysis of Nonlinear Circuits,
Excluding Radiation)
. CANCER began as a derivative of a program that was the class project
of a series of courses taught by Ron Rohrer with the approval and
encouragement of Professor Donald O. Pederson
. Larry Nagel wrote the netlist parser and the analysis core and was
student group leader
. Lynn Weber developed a noise analysis feature that utilized adjoint
network techniques
. Bob Berry wrote the sparse matrix LU decomposition package
. CANCER project's key features:
. o Was the first circuit simulator to utilize sparse matrix techniques
. o Used Newton-Raphson iteration method heuristically modified for
bipolar circuits
. o Utilized implicit integration to accommodate widely spread time
constants of an IC
. o Integrated DC operating point analysis, small-signal AC analysis
and transient analysis
. Project presented by Ron Rohrer at the 1971 ISSCC , but the code was
considered partially proprietary and was never publicly released
1971 SPICE 1 (Simulation Program with IC Emphasis) direct outgrowth of
CANCER
. Ron Rohrer leaves UC Berkeley and further development of CANCER
(renamed SPICE) became Larry Nagel's Masters project with Don Pederson
taking over as faculty advisor
. KEY EVENT: Don Pederson insisted that all further work be releasable
to the public domain
. SPICE 1 release's key features:
. o Models for bipolar transistors were changed to Gummel-Poon equations
. o JFET and Shichman-Hodges MOSFET devices added (for Dave Hodges'
MOSFET design class)
. o Fixed time step and strict Nodal Analysis (true voltage sources
and inductors not supported)
. o DC, AC, Transient, Noise, and Sensitivity Analyses in the same program
. o Built-in models for diodes, bipolar transistors, MOSFETs, and JFETs
. Was about 6k lines of FORTRAN at first informal limited public
release in late 1971
. Official public release was May 1972 with first formal paper
presented by Don Pederson at the 16th Midwest Symposium on Circuit
Theory, April 12, 1973
. SPICE 1 becomes industry standard simulation tool running on large
mainframe computers
1972 SPICE 2 begins
. First version of SPICE 2 was Larry Nagel's Ph.D. project under Don
Pederson
. Modified Nodal Analysis (MNA) added, enabling voltage sources and
inductors for the first time
. Ellis Cohen added dynamic memory allocation
. Adjustable time-step control added, greatly speeding most simulations
. MOSFET and bipolar models overhauled and extended
. Was about 8k lines of FORTRAN when first released to the public
domain in late 1974
. Larry Nagel departs for Bell Labs and his thesis becomes the SPICE 2
Users Guide
1975 journey to SPICE 2G6 (the pinnacle FORTRAN version)
. Ellis Cohen becomes primary contributor with later help from Andrei
Vladimirescu
. First of a series of public revision releases after Nagel's version
2B begin in 1978
. Along the way, sub circuits, poly sources and transmission lines are
added
. Version 2G6 ends up implementing three MOSFET models:
. o MOS 1 is a simplistic model described purely by ideal square-law
I-V characteristics
. o MOS 2 is an analytical model, MOS 3 is a semi-empirical model and
both include second-order effects such as channel length modulation,
sub threshold conduction, scattering limited velocity saturation,
small-size effects, and charge-controlled capacitances
. 2G6 released to public domain in April 1983 (and is still available
today from UC Berkeley)
. Many commercial simulators today are based on SPICE 2G6
1983 SPICE 3 begins
. Tom Quarles begins work, writing first version in RATFOR, a C-like
preprocessor for FORTRAN
. Was fully converted to C in 1985 with first early versions released
in March of that year
. Added models: MESFET, lossy transmission line and non-ideal switch
. Arbitrary behavioral voltage and current sources added
. Includes polynomial capacitors, inductors and voltage controlled sources
. Allowed the use of alphabetical node labels rather than only numbers
. Features a graphical interface for viewing results
. New version eliminates many convergence problems
. Added noise, distortion and pole-zero analysis, temperature
sweeping, Monte Carlo and Fourier analysis
. Not fully compatible with SPICE 2G6
. Was about 135,000 lines of C code at first public release in 1989
. Final version at Berkeley, SPICE 3F5, released to public in 1993
. XSPICE was developed at Georgia Tech as an extension to the SPICE
language to allow behavioral modeling of components
. o Drastically improve the speeds of mixed-mode and digital simulations
1984 PSpice (micro Processor SPICE)
. Developed by MicroSim to run on the first IBM PC, initially released
in January 1984
. Was the first commercial offspring of Berkeley SPICE to run directly
on the PC platform
. Was the first SPICE program to gain wide acceptance in both industry
and academia
. KEY EVENT: A zero cost (but node-limited) student version is
introduced in 1988 -- for the first time, SPICE becomes ubiquitous in
the electrical engineering community
. Evolved from Berkeley SPICE 2G, but added many proprietary enhancements
. Probe, a waveform viewer module, was added when PC VGA graphics
became available
. Schematics, a graphical front end, was added much later sometime in
the early 1990s
1999 LTspice/SwitcherCAD III first released to public
. 1981 Linear Technology Corporation founded
. 1991 DOS SwitcherCAD available (equation based)
. 1996 ?Power SwitcherCAD available(simulation based)
. 2008 LTspice IV
Some possible noteworthy events/additions:
Ver 2 Jan03: graphical symbol editor hierarchical schematics
Apr04: Chan inductor, undocumented behavioral inductor revealed
Your suggestions?
__
During the 1980s time frame when Micosim's PSPICE became popular Intusoft Spice program was competitive with Microsim and Electronics Workbench was a low cost Microsim competitor. I believe Intusoft is worth a mention because during the 1980s and 1990s time frame Intusoft published a large variety of simulation examples in their Newsletter. All of the the old Newsletters are still available on Intusoft's Web site. Howard [Non-text portions of this message have been removed] [Non-text portions of this message have been removed]
|
On 7/12/2013 11:24 AM, analogspiceman wrote:
I am attempting to create a historical timeline of the history
of SPICE as it has grown in function, use and popularity in the
engineering community. This is to be in bullet point format and
I intended to include only those forms of SPICE that were most
ubiquitous in their time, i.e. the various Berkeley SPICEs, then
PSpice, and, of course, LTspice.
What I've got so far I will put at the end of this message. It has
errors and is not complete, especially the part about LTspice. I
am looking for corrections and input as to the major additions and
events regarding LTspice. (What additions over the years seem
especially noteworthy to you?).
I will fill in the historical dates from the Change Log and from
the group message archive. When the history is complete, I will
add it to group files as a PDF and also add it as a new section
over at the LTwiki (so there is no need to copy it just yet).
________________________________________________
THE HISTORY OF SPICE
1969 beginnings of CANCER (Computer Analysis of Nonlinear Circuits,
Excluding Radiation)
. CANCER began as a derivative of a program that was the class project
of a series of courses taught by Ron Rohrer with the approval and
encouragement of Professor Donald O. Pederson
. Larry Nagel wrote the netlist parser and the analysis core and was
student group leader
. Lynn Weber developed a noise analysis feature that utilized adjoint
network techniques
. Bob Berry wrote the sparse matrix LU decomposition package
. CANCER project's key features:
. o Was the first circuit simulator to utilize sparse matrix techniques
. o Used Newton-Raphson iteration method heuristically modified for
bipolar circuits
. o Utilized implicit integration to accommodate widely spread time
constants of an IC
. o Integrated DC operating point analysis, small-signal AC analysis
and transient analysis
. Project presented by Ron Rohrer at the 1971 ISSCC , but the code was
considered partially proprietary and was never publicly released
1971 SPICE 1 (Simulation Program with IC Emphasis) direct outgrowth of
CANCER
. Ron Rohrer leaves UC Berkeley and further development of CANCER
(renamed SPICE) became Larry Nagel's Masters project with Don Pederson
taking over as faculty advisor
. KEY EVENT: Don Pederson insisted that all further work be releasable
to the public domain
. SPICE 1 release's key features:
. o Models for bipolar transistors were changed to Gummel-Poon equations
. o JFET and Shichman-Hodges MOSFET devices added (for Dave Hodges'
MOSFET design class)
. o Fixed time step and strict Nodal Analysis (true voltage sources
and inductors not supported)
. o DC, AC, Transient, Noise, and Sensitivity Analyses in the same program
. o Built-in models for diodes, bipolar transistors, MOSFETs, and JFETs
. Was about 6k lines of FORTRAN at first informal limited public
release in late 1971
. Official public release was May 1972 with first formal paper
presented by Don Pederson at the 16th Midwest Symposium on Circuit
Theory, April 12, 1973
. SPICE 1 becomes industry standard simulation tool running on large
mainframe computers
1972 SPICE 2 begins
. First version of SPICE 2 was Larry Nagel's Ph.D. project under Don
Pederson
. Modified Nodal Analysis (MNA) added, enabling voltage sources and
inductors for the first time
. Ellis Cohen added dynamic memory allocation
. Adjustable time-step control added, greatly speeding most simulations
. MOSFET and bipolar models overhauled and extended
. Was about 8k lines of FORTRAN when first released to the public
domain in late 1974
. Larry Nagel departs for Bell Labs and his thesis becomes the SPICE 2
Users Guide
1975 journey to SPICE 2G6 (the pinnacle FORTRAN version)
. Ellis Cohen becomes primary contributor with later help from Andrei
Vladimirescu
. First of a series of public revision releases after Nagel's version
2B begin in 1978
. Along the way, sub circuits, poly sources and transmission lines are
added
. Version 2G6 ends up implementing three MOSFET models:
. o MOS 1 is a simplistic model described purely by ideal square-law
I-V characteristics
. o MOS 2 is an analytical model, MOS 3 is a semi-empirical model and
both include second-order effects such as channel length modulation,
sub threshold conduction, scattering limited velocity saturation,
small-size effects, and charge-controlled capacitances
. 2G6 released to public domain in April 1983 (and is still available
today from UC Berkeley)
. Many commercial simulators today are based on SPICE 2G6
1983 SPICE 3 begins
. Tom Quarles begins work, writing first version in RATFOR, a C-like
preprocessor for FORTRAN
. Was fully converted to C in 1985 with first early versions released
in March of that year
. Added models: MESFET, lossy transmission line and non-ideal switch
. Arbitrary behavioral voltage and current sources added
. Includes polynomial capacitors, inductors and voltage controlled sources
. Allowed the use of alphabetical node labels rather than only numbers
. Features a graphical interface for viewing results
. New version eliminates many convergence problems
. Added noise, distortion and pole-zero analysis, temperature
sweeping, Monte Carlo and Fourier analysis
. Not fully compatible with SPICE 2G6
. Was about 135,000 lines of C code at first public release in 1989
. Final version at Berkeley, SPICE 3F5, released to public in 1993
. XSPICE was developed at Georgia Tech as an extension to the SPICE
language to allow behavioral modeling of components
. o Drastically improve the speeds of mixed-mode and digital simulations
1984 PSpice (micro Processor SPICE)
. Developed by MicroSim to run on the first IBM PC, initially released
in January 1984
. Was the first commercial offspring of Berkeley SPICE to run directly
on the PC platform
. Was the first SPICE program to gain wide acceptance in both industry
and academia
. KEY EVENT: A zero cost (but node-limited) student version is
introduced in 1988 -- for the first time, SPICE becomes ubiquitous in
the electrical engineering community
. Evolved from Berkeley SPICE 2G, but added many proprietary enhancements
. Probe, a waveform viewer module, was added when PC VGA graphics
became available
. Schematics, a graphical front end, was added much later sometime in
the early 1990s
1999 LTspice/SwitcherCAD III first released to public
. 1981 Linear Technology Corporation founded
. 1991 DOS SwitcherCAD available (equation based)
. 1996 ?Power SwitcherCAD available(simulation based)
. 2008 LTspice IV
Some possible noteworthy events/additions:
Ver 2 Jan03: graphical symbol editor hierarchical schematics
Apr04: Chan inductor, undocumented behavioral inductor revealed
Your suggestions?
__
During the 1980s time frame when Micosim's PSPICE became popular Intusoft Spice program was competitive with Microsim and Electronics Workbench was a low cost Microsim competitor. I believe Intusoft is worth a mention because during the 1980s and 1990s time frame Intusoft published a large variety of simulation examples in their Newsletter. All of the the old Newsletters are still available on Intusoft's Web site. Howard
|
