Helmut, OK. What's happening is that the '+' sign can be used to mean incremented from the previous value. It's a PSpice convention useful for time points as in V2 1 0 PWL (0 0 +1m 1 +1m 0 +1m 1 +1m 0 +1m 1) But I'll turn that off for the voltage in a future version, since I don't think it should do it for the voltage, just the time. --Mike __________________________________________________ Do you Yahoo!? Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop! http://platinum.yahoo.com

Hallo Helmut and Mike Engelhardt, thanks for finding and solving the +problem. My (LTspice-)World doesn't seem to collapse in the near future any more. Mr. Engelhardt, are you German? your Name is. Arnold

Quite apart from LTSpice, please accept a moral and ethical commendation. By living in another culture & learning its language you are promoting international understanding and respect for all persons. This is unusual even among educated professionals. When I was rushed to Mexico City after the earthquake, I learned that one of my co-workers believed ANYBODY could understand English if only it was spoken loudly and clearly enough. An old joke asks, "If somebody who speaks 3 languages is trilingual and somebody who speaks 2 languages is bilingual, what term describes somebody who speaks but one language?" The answer, of course, is "American". This situation is a symptom of a larger arrogance and self-centeredness which we never intended to cultivate and are certainly not proud of, but which often limits our ability to accept others as truly human and our equals. (Yes, I include myself in that indictment: with the minimal Spanish I learned in High School I could bumble through ordering from a menu, and possibly even ask for directions, but writing a coherent paragraph, reading a newspaper or even normal conversation are beyond me. ) Again, thanks for doing your part. I hope nobody recognizes that I carry a Scottish name and expects me to reply in Gaelic . . .

--- In LTspice@..., Message 141, Panama Mike <panamatex@y...> wrote: < snip > > > BTW, I'm thinking of introducing opamp models that > use a different modeling methodology, similar to > that used for LTspice's SMPS products. The result > would be computationally extremely lightweight and > robust models that model noise too(these PSpice- > style opamp models almost never get the noise > modeled). However, the opamps models would not > run in other SPICE simulators and non-LT opamp > models wouldn't be available. Would you folks be > interested in something like that? > > --Mike Mike, this sounds like something I'd like to dissuade you from. Part of the strength of the SPICE methodology is that the models are transmitted as "open source", simple text files. The most significant advantage is that we Mere Mortals can easily extend, improve, correct, or modify models as needed. The parent thread for this posting is a good example. Because almost everything about the model was in plain view, several minds were independently analyzing the problem and solving it. I cannot imagine the problem being resolved nearly as quickly if the model's topology and parameter values had been locked-up in a proprietary format readable only by a few people. The SPICE methodology permits individuals to customize models as needed. If, for instance, noise is a critical performance characteristic the necessary elements can be readily included to model it. Otherwise they may be omitted. Similarly, a small-signal stage where output limiting is not a concern can get by with a simplified output circuit in the model. Along the same line it is relatively easy to adjust model parameters to fit particular situations. The model can be customized to reflect the device's behavior at, say, a temperature extreme. Or an engineer can investigate the implications of using a device whose performance parameters (like offset voltage or slew rate) are near the data sheet limits. Likewise the need for parts specially selected for certain characteristics (such as low offset current) can be evaluated. Finally the current SPICE modeling methodology allows engineers to quickly create workable models for new or alternative components. I hope that whatever modeling methodology you choose will retain these features. Dale

Is there any way to limit the number of voltages and currents that are saved during a transient analysis? Over the weekend I ran a simulation of a poly-phase voltage regulator. The resulting data file was nearly 5G! It took about 20 minutes this morning just to load up 7 or 8 traces to view. I've noticed that the time to load a trace grows with the number of nodes, not just the simulation period, so I'm thinking that I could save a lot of time if I could be selective about what data I save. Also, is there a way to selectively export plot data? It would be really nice to be able to bring particular traces into Mathcad, for example, for more detailed analysis. It would also be very beneficial to be able to e-mail data to plot a few traces. Thanks, John

I just started using LTSPice a few weeks ago to model semi-insulating electro-optic devices as RC-mesh/networks. It works great... But I need to model the time dependence of theses devices as the temperature is ramped. Is there any way to specify a resistor value that is dependent on the simulation time. I know you can specify a voltage that is dependent on simulation time by using the PULSE command, or an behavioral voltage source using a mathmatical expression with the variable "time". Can you specify a resistor value that is a fuction of simulation time in a similar manner? If not, is there any other way to accomplish this?

First let me congratulate the author(s) and those that support this software. It is really useful and easy to use. My daughter, who is an engineeing sophmore, has even started to use LTSpice for some labs. I am looking for a way to either pass plot scales from a dot statement (.PLOT or .VIEW kind of thing) or at least to freeze the plot scales from run to run. It would be helpful when trying to visually compare the the results between runs if the the plot did not automatically rescale. It would also be nice to be able to have an alias type statement to save reentering things like V(out)/V(in) or V(N003, N006)/I(R7). Again, thank you for the software and thanks to Linear Tech for their part in this.

There's been some reorganization of the website that I use of SwCADIII/LTspice publication. Could you folks let me know if the menu item Tools=>Sync Release works for you. It should work from anywhere in the world and give you version 2.01s right now. Probably better to e-mail me at pmte@..., instead of posting to the users' group. --Mike __________________________________________________ Do you Yahoo!? Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop! http://platinum.yahoo.com

Hello, I'm new to this group and I don't have experience working with Spice models. Someone can please help me or point me to the right direction so I can make a TRIAC model? If there's some ready-to-go model, please let me know. Thank you very much, Brusque -- ----------------------------------------------------------------- Edson Brusque C.I.Tronics Lighting Designers Ltda Research and Development Blumenau - SC - Brazil Say NO to HTML mail www.citronics.com.br -----------------------------------------------------------------

parameter Preferably documentation There Yes, it's a good Idea to allow white background to the graphik Window, in order to save printing-color or some extra work for inverting it for other programs. The black background reminds me my analog oszilloscope, earlier used every day. But nowadays I'm almost afraid to touch it's knobs, because of the huge dust on it. Maybe a good Idea too, to allow some differnt styles of drawing lines like dotted, hatched .... for black and white coying machines. Adding the unit behind every number can make it difficult to read at high line-densities. The Windows could have a look similar to the picture below, I made with an early Version of Spice2 (years ago). . Thanks, Arnold

I'm trying to use the dflop part in a simple circuit and am having difficulty getting it to work. +-----------+ 0-6v square wave --------|>CLK Q |--- 1v solid out?? GND----| D Q'| +-----------+ Both the CLR and the PRE inputs are floating though I've tried tieing them up and down. There doesn't seem to be anywhere to attach power to the device? There is a common pin (COM?) on the corner, but leaving it open or tieing it to ground has the same effect. I'm looking for a 5-6v output. The 160 example has dflops in it and seems to work fine, which is beyond me. Any ideas? Thanks, David Pariseau.

I put up a version of LTspice today with a new feature. There's a new symbol attribute called ModelFile. This lets you specify a file to include as a library file whenever this symbol is included. However, the symbol is still edit-able. This let's you enter parameters to pass to the subcircuit. There's two example symbols of the use of these feature included, 1pole.asy and 2pole.asy in the opamp directory. These are somewhat ideal opamps with allow the following parameters to be entered to model a specific opamp: Avol open loop DC gain. GBW open loop gain-bandwidth product Slew slew rate Ilimit output current limit rail how close output can get to the rail Vos input offset voltage en equiv. input voltage noise enk equiv. input voltage noise corner freq in equiv. input current noise ink equiv. input current noise corner freq The model draws all current from the voltage supplies and has a signal internal node. Output stage emitter followers are set to 100 Ohms, but you can change that if you need a more ideal opamp. The 2pole version has two internal nodes and an additional parameter, phimargin, which specifies the 2nd pole in terms of the (approx -imate) phase margin in degrees. Input bias, input common mode range and PSRR are not modeled. Let me know if you find these things useful. --Mike __________________________________________________ Do you Yahoo!? Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop! http://platinum.yahoo.com

Various people are writing: Note that the background color is not printed. That is, you can set it to black in the color preferences dialog but it will still be white when you print it on white paper becuase it's the background and is not printed. So if you also what a bitmap that is on a white background, so a print preview and capture that bitmap with Alt-Print Screen. Hope this helps, --Mike __________________________________________________ Do you Yahoo!? Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop! http://platinum.yahoo.com

I've read through past messages, the SwCAD help and such and attempted to add a 3rd party model for the FDN304P. It seems to find the model fine now, but I get the error "Too few parameters for subcircuit type "fdn304p"". I basically dropped the model file into the &#92;sub directory, copied the pmos symbol file and changed it to specify the FDN304p model. Any thoughts? Dave Pariseau. Here are the files: FDN304p.asy ------------- Version 4 SymbolType CELL LINE Normal 48 48 48 96 LINE Normal 16 80 48 80 LINE Normal 16 48 24 48 LINE Normal 48 48 24 44 LINE Normal 48 48 24 52 LINE Normal 24 44 24 52 LINE Normal 16 8 16 24 LINE Normal 16 40 16 56 LINE Normal 16 72 16 88 LINE Normal 0 80 8 80 LINE Normal 8 16 8 80 LINE Normal 48 16 16 16 LINE Normal 48 0 48 16 WINDOW 0 56 32 Left 0 WINDOW 3 56 72 Left 0 SYMATTR Value FDN304P SYMATTR Prefix X SYMATTR SpiceModel FDN304P.mod SYMATTR Value2 FDN304P SYMATTR Description P-Channel MOSFET transistor PIN 48 0 NONE 0 PINATTR PinName D PINATTR SpiceOrder 1 PIN 0 80 NONE 0 PINATTR PinName G PINATTR SpiceOrder 2 PIN 48 96 NONE 0 PINATTR PinName S PINATTR SpiceOrder 3 FDN304p.mod --------------- *FDN304P at Temp. Electrical Model (T2) *------------------------------------- .SUBCKT FDN304p 20 10 30 50 *20=DRAIN 10=GATE 30=SOURCE 50=VTEMP Rg 10 11x 1 Rdu 12x 1 1u M1 2 1 4x 4x DMOS L=1u W=1u .MODEL DMOS PMOS(VTO=-0.87 KP=2.5E+1 +THETA=0.25 VMAX=8.5E5 LEVEL=3) Cgs 1 5x 1300p Rd 20 4 7E-3 Dds 4 5x DDS .MODEL DDS D(M=4.26E-1 VJ=3.39E-1 CJO=562p) Dbody 20 5x DBODY .MODEL DBODY D(IS=3.81E-10 N=1.145283 RS=0.00084 TT=14.5n) Ra 4 2 7E-3 Rs 5x 5 0.5m Ls 5 30 0.5n M2 1 8 6 6 INTER E2 8 6 4 1 2 .MODEL INTER PMOS(VTO=0 KP=10 LEVEL=1) Cgdmax 7 4 1050p Rcgd 7 4 10meg Dgd 4 6 DGD Rdgd 4 6 10meg .MODEL DGD D(M=3.2E-1 VJ=4.23E-3 CJO=1050p) M3 7 9 1 1 INTER E3 9 1 4 1 -2 *ZX SECTION EOUT 4x 6x poly(2) (1x,0) (3x,0) 0 0 0 0 1 FCOPY 0 3x VSENSE 1 RIN 1x 0 1G VSENSE 6x 5x 0 RREF 3x 0 10m *TEMP SECTION ED 101 0 VALUE {V(50,100)} VAMB 100 0 25 EKP 1x 0 101 0 .012 *VTO SECTION EVTO 102 0 101 0 .0007 EVT 11x 12x 102 0 1 *DIODE THERMO BREAKDOWN SECTION EBL VB1 VB2 101 0 0.8 VBLK VB2 0 20 D DB1 20 DBLK .MODEL DBLK D(IS=1E-14 CJO=.1p RS=.1) EDB 0 DB1 VB1 0 1 .ENDS FDN304p *FDN304P (Rev.A) 12/4/00 **ST

Hello, I'm trying to have a working TRIAC model on LTSpice. From www.teccor.com I got the following model that I saved to a file called triac.sub. I've put this file on lib&#92;sub folder. On the squematic I've put the ".INCLUDE triac.sub" Spice directive. *=========================* * TECCOR TRIACS * * Triac pinout: MT2 G MT1 * *=========================* ***** *SRC=Q8025R5;Q8025R5;TRIACS;TECCOR;800V 25A *SYM=TRIAC .SUBCKT Q8025R5 1 2 3 * TERMINALS: MT2 G MT1 QN1 5 4 3 NOUT OFF QN2 11 6 7 NOUT OFF QP1 6 11 3 POUT OFF QP2 4 5 7 POUT OFF DF 4 5 DZ OFF DR 6 11 DZ OFF RF 4 6 8MEG RT2 1 7 25.4M RH 7 6 5.25 RGP 8 3 12 RG 2 8 5.8 RS 8 4 1.2 DN 9 2 DIN OFF RN 9 3 6.12 GNN 6 7 9 3 0.554 GNP 4 5 9 3 0.705 DP 2 10 DIP OFF RP 10 3 3.56 GP 7 6 10 3 0.373 .MODEL DIN D (IS=764F) .MODEL DIP D (IS=764F N=1.19) .MODEL DZ D (IS=764F N=1.5 IBV=100U BV=800) .MODEL POUT PNP (IS=764F BF=5 CJE=1.12N TF=102U) .MODEL NOUT NPN (IS=764F BF=20 CJE=1.12N CJC=223P TF=6.8U) .ENDS ***** But everytime I try to start the simulation I got the message: SPICE Error Too many parameters for subcircuit type "q8025r5"(instance: xu1) On the "Component Attribute Editor" I have: Prefix X InstName U1 SpiceModel triac Value Q8025R5 Value2 <none> SpiceLine <none> SliceLine2 <none> Please, I need help. Thanks, Brusque -- ----------------------------------------------------------------- Edson Brusque C.I.Tronics Lighting Designers Ltda Research and Development Blumenau - SC - Brazil Say NO to HTML mail www.citronics.com.br -----------------------------------------------------------------

When I simulate the following circuit I end up with 60mv for VOUT when the circuit should be off? Any ideas why? Not sure where the voltage is coming from. 6v 47pf Batt BSS84 VOUT +----+---+------+----+ +-----------+--+ | + + + --- | | --- --- .-. V .-. | --- - | | | | |20K | | | 1M| | | 50K | | |-+ | === '-' | ___ '-' +->| | GND +-----+-|___|++ | | |-+ | | +-| + 47pf | |----+----------+ 2N7002 |<-+---+ | 2N7002 | +-| | | | | o | .-. | |=|> === | | --- VOff | o GND | | --- Mom.Switch | '-' | === 500K | | GND === === GND GND Dave Pariseau.

Thanks to Helmut for the hints to making model-libs and coverting plain Spice- Ascii text. I encounterd problems with the model of the vacuum tube 12AX7 below. Apart from being rather far from reality, this model seems to produce convergence problems. LTspice throws an abort "time intervall too small" whatever time invall I put in the .tran and also controlPanel. The shown waveform heavily varies. Winspice concludes computing. I earlier decided to develop Musician's Ampifiers, which imitate a tube- Amplifier together with it's output transformer using analog and switched circuits - not computing it, this had been done already. Guitarists love there sound, I do so too. I intend a switched output stage and supply to save power consumption and weight. There main features are: - huge dynamic range - nonlinearity depending on the signal's time domain - compression effects (and filtering) highly depending on the signal - some strange storage effects at medium and high levels I made lots of step-/puls-responses of this kind of amplifiers to get there behaviour. I is quit more than just nonlinearity. Are there special devices from LT for this purpose ? thanks, Arnold *************************************************************************** * ECC83_2.cir *************************************************************************** V1 1 0 DC 0 AC 1 PWL(0 0 1m 0 6m -5 16m 5 21m 0) R1 1 0 100K R3 3 0 2.2K R4 4 100 150K X1 4 1 3 NH12AX7 VP 100 0 DC 250 .TRAN 100u 50m 0 100u .PRINT TRAN V(4) *************************************************************************** * GENERIC: 12AX7 / ECC83 * MODEL: NH12AX7 * NOTES: *-------------------------------------------------------------------------- * Connections: Anode * | Grid * | | Cathode * | | | .SUBCKT NH12AX7 A G K * * ANODE MODEL BLIM LI 0 V=(URAMP(V(A)-V(K))^ 1.5 )* 1.6e-5 BGG GG 0 V=V(G)-V(K)--0.53056 BRP1 RP1 0 V=URAMP(-V(GG)* 0.076498 ) BRP2 RP2 0 V=V(RP1)-URAMP(V(RP1)-0.999) BRPF RP 0 V=(1-V(RP2)^ 1 )+URAMP(V(GG))* 0.18 BGR GR 0 V=URAMP(V(GG))-URAMP(-(V(GG)*(1+V(GG)*-0.013621 ))) BEM EM 0 V=URAMP(V(A)-V(K)+V(GR)* 87.302 ) BEP EP 0 V=(V(EM)^ 1.5 )*V(RP)* 1.11e-6 BEL1 EL1 0 V=URAMP(V(EP)) BEL EL 0 V=V(EL1)-URAMP(V(EL1)-V(LI)) BLD LD 0 V=URAMP(V(EP)-V(LI)) BAK A K I=V(EL) * * GRID MODEL BGF GF 0 V=(URAMP(V(G)-V(K)--0.2 )^1.5)* 1e-5 BG G K I=V(GF)+V(LD) * * CAPS CAK A K 0.7P CGK G K 2.4P CGA G A 3.9P * .ENDS *************************************************************************** .END

Not this time! '^' The behavioral source syntax is given in the help in LTspice=>Circuit Elements=>B. Arbitrary behavioral source. '^' means Boolean exclusive OR. '**' is exponentiation. SPICE3 doesn't have Boolean exclusive OR. PSpice uses '**' for exponentiation and it also implemented use behavioral sources before Berkeley, so here, PSpice is the standard, not Berkeley SPICE. --Mike __________________________________________________ Do you Yahoo!? Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop! http://platinum.yahoo.com

Hello Mike, sorry for my too fast judgement. I have overlooked the '^' XOR operator in the LTSPICE help page. Thanks for your reply, Helmut

Hello Helmut, thanks to you for this fine solution. Now it all works. best regards, Arnold