Keyboard Shortcuts
ctrl + shift + ? :
Show all keyboard shortcuts
ctrl + g :
Navigate to a group
ctrl + shift + f :
Find
ctrl + / :
Quick actions
esc to dismiss
Likes
- LTspice
- Messages
Search
|
Vacuum tube models in LTspice?
Bill Lewis <[email protected]>
Has anyone migrated any of the vacuum tube models floating
around on the 'net to LTspice? Bill |
|
Re: S-parameters for Helmut
Hello Helmut,
S-parameters are a very useful representation of a given network. For a 1-port, they correspond to the voltage reflection coefficient, and they can therefore be displayed on the Smith Chart. For an n-port, they provide the various voltage gains across different ports. S-parameters are another way to represent the H/Y/Z (or ABCD) parameters of a network. They are particularly useful at high (RF and higher) frequencies for which SHORTS and OPEN circuits are difficult to define accurately because networks become distributed when they reach about 0.1(lambda) in size. When this happens, it becomes convenient to think of forward and reflected voltage and power waves. See this link for more info on the Scattering Parameters: << >> For a two-port, for example, S11 and S22 represent the input and reflection coefficients, and S21 and S12 are proportional to the forward and reverse voltage gains. Circuit theory textbooks will provide conversion tables between S/Y/H/Z parameters, so one can always convert into more "physical" units. Once you get used to the S-parameters, there is no need to anymore. To see how the Smith Chart works, see << SpecAn9.shtml#schart >> Cheers! "Bolo" --- In LTspice@..., "Helmut Sennewald < helmutsennewald@y...>" <helmutsennewald@y...> wrote: --- In LTspice@..., "bolocolombo <colombobolo@h...>" |
|
Re: S-parameters for Helmut
--- In LTspice@..., "bolocolombo <colombobolo@h...>"
<colombobolo@h...> wrote: netlist that shows how to measure S11 and S21 for a simple two-portHello "bolocolombo", thanks for the S-parameter example. I tried it immediately and it seems to work. I have to admit that I have only a small idea about the S-parameter concept. Best Regards Helmut |
|
S-parameters for Helmut
Hello Helmut.
Thank you for your advice. I was able to modify the transistor models from the SPICE directive, or even better, by editing the model files for the NPNs. The .STEP is a good suggestion when you wish to play with a single parameter. As for you question regarding S-parameters, I have included a netlist that shows how to measure S11 and S21 for a simple two-port (consisting of a single shunt resistor Rtest2port) which you can substitute by your circuit. Then, you duplicate the circuit and switch the sources from the input to the output to "measure"S22 and S12. Then you plot Vs11, Vs22, etc, which correspond to S11, S22¡ Once that is done you can go to the plot window, and plot various quantities like the Unilateral power gain by clicking ADD TRACE and then paste the expression for U in the window as (((MAG(V(s21)/V(s12)-1))**2)/2/(((1-(MAG(V(s11)))**2-(MAG(V(s22)))**2+ (MAG(V(s11)*V(s22)-V(s12)*V(s21)))**2)/2/MAG(V(s12)*V(s21)))*MAG(V(s21 )/V(s12)) - Re(V(s21)/V(s12))))**0.5 (note that the square root is needed because LTSPICE takes 20log of everything in the dB scale) NETLIST TO MEASURE S11 and S21 ================================================================== * C:\Program Files\LTC\SwCADIII\CB_Files\FET_model.asc V1 N001 0 0 AC 1 0 Rser=0 Cpar=0 R6 N002 N001 50 E1 N003 0 N002 0 2 R8 S11 0 1G V2 N003 S11 0 AC 1 0 Rser=0 Cpar=0 R7 N002 0 50 E2 S21 0 N002 0 2 R9 S21 0 1G Rtest2port N002 0 100 .ac dec 99 1G 300G .backanno .end |
|
Re: Can't open library file.
Helmut you saved me again, thank you. Part of the confusion that I had
was that I don't really know what the syntax should be. What I did was cut and pasted the example in the help file to my library and renamed it. What I didn't realize was that the command didn't include everything below the 'Example:'. After looking at your example the help file made more sense. This got me thinking. What would be helpful would be actual working examples (similar to what you did for me) using the circuit elements and commands in a single file. Also what would be useful would be an explanation of the error codes (I figured out that multiple instances of W1 was a result of having more than one library, I tried placing one in different places to get one to open, with the same switch model in each). Maybe the powers that be at Linear Technology can throw something together and put it in the Files location on this site. Or if any of the members have a little tidbit that they found useful maybe we can set up a folder for them? Anyone have thoughts on this one? Bunny --- In LTspice@..., "Helmut Sennewald <helmutsennewald@y...>" <helmutsennewald@y...> wrote: --- In LTspice@..., "bunnyblues2001syntax. pages. Finally I was successful. The value of the CSW symbol must contain |
|
Re: Can't open library file.
--- In LTspice@..., "bunnyblues2001
<bunnyblues2001@y...>" <bunnyblues2001@y...> wrote: OK where did I go wrong, I'm getting - Could not open include fileHello Bunny, the problem is that your model/subcircuit doesn't follow SPICE syntax. Your switch model in the library has to be only: .model CSWITCH1 CSW( Ron=0.1 Roff=1MEG It=1 Ih=0.5) Only lines like these can model CSW switches. See the help pages. All the other things have to be done in the schematic. I have never used a CSW before and frankly speaking I tried in the schematic until the netlist followed the syntax in the help pages. Finally I was successful. The value of the CSW symbol must contain two values either in value-line or in the second field value2. Right click over the symbol to look at. value: V1 CSWITCH1 or value: V1 value2: CSWITCH1 Best Regards Helmut CSW = (C)urrent controlled (SW)itch Circuit example with CSW: ------------------------- Version 4 SHEET 1 1424 692 WIRE 752 464 752 496 WIRE 752 496 480 496 WIRE 208 496 208 400 WIRE 208 496 208 512 WIRE 208 240 480 240 WIRE 480 384 480 352 WIRE 480 464 480 496 WIRE 480 272 480 240 WIRE 208 320 208 240 WIRE 752 272 752 240 WIRE 752 240 480 240 WIRE 752 352 752 384 WIRE 480 496 208 496 WIRE 752 80 752 112 WIRE 752 112 432 112 WIRE 208 112 208 16 WIRE 208 112 208 128 WIRE 208 -144 432 -144 WIRE 208 -64 208 -144 WIRE 752 -112 752 -144 WIRE 752 -32 752 0 WIRE 432 -48 432 -144 WIRE 432 -144 752 -144 WIRE 432 32 432 112 WIRE 432 112 208 112 FLAG 208 512 0 FLAG 208 128 0 SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\csw 752 272 R0 WINDOW 0 55 20 Left 0 SYMATTR InstName W2 SYMATTR Value V2 CSWITCH1 SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\res 736 368 R0 SYMATTR InstName R2 SYMATTR Value 10 SYMBOL F:\PROGRAMME\LTC\SWCADIII\lib\sym\res 464 368 R0 SYMATTR InstName R20 SYMATTR Value 10 SYMBOL F:\PROGRAMME\LTC\SWCADIII\lib\sym\voltage 480 256 R0 WINDOW 0 37 34 Left 0 WINDOW 3 38 80 Left 0 WINDOW 123 0 0 Left 0 WINDOW 39 0 0 Left 0 SYMATTR InstName V2 SYMATTR Value 0 SYMBOL F:\PROGRAMME\LTC\SWCADIII\lib\sym\voltage 208 304 R0 WINDOW 123 0 0 Left 0 WINDOW 39 24 132 Left 0 SYMATTR InstName V3 SYMATTR Value SINE(0 20 2k) SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\csw 752 -112 R0 WINDOW 0 55 20 Left 0 SYMATTR InstName W1 SYMATTR Value V1 SYMATTR Value2 CSWITCH1 SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\res 736 -16 R0 SYMATTR InstName R1 SYMATTR Value 10 SYMBOL F:\PROGRAMME\LTC\SWCADIII\lib\sym\voltage 208 -80 R0 WINDOW 123 0 0 Left 0 WINDOW 39 24 132 Left 0 SYMATTR InstName V1 SYMATTR Value SINE(0 20 2k) SYMBOL F:\PROGRAMME\LTC\SWCADIII\lib\sym\res 416 -64 R0 SYMATTR InstName R10 SYMATTR Value 10 TEXT 206 -256 Left 0 !.tran 0 1m 0 1u TEXT 208 -216 Left 0 !.model CSWITCH1 CSW( Ron=0.1 Roff=1MEG It=1 Ih=0.5) TEXT 208 -328 Left 0 ;CURRENT CONTROLLED SWITCH\nValue must be "Vsense modelname", e.g. "V1 CSWITCH1". TEXT 208 -184 Left 0 ;.include mylibrary1.lib New "mylibrary1.lib", but it is not needed in the example above. ---------------------------------------------------------------- .model CSWITCH1 CSW( Ron=0.1 Roff=1MEG It=1 Ih=0.5) |
|
Re: Can't open library file.
Then it should have been able to include the file.
Until the help documents the paths searched for .lib and .inc files. Until you get the problem figured out, you might just use absolute paths. --Mike __________________________________________________ Do you Yahoo!? Yahoo! Tax Center - forms, calculators, tips, more |
|
Re: Can't open library file.
That was the first thing I checked. There's only one extention on the
toggle quoted message
Show quoted text
file. Does the rest of the code check out? --- In LTspice@..., Panama Mike <panamatex@y...> wrote:
Is the file really called "MYLIBRARY1.LIB" or |
|
Re: constructing opamp models
Dale <[email protected]>
--- In LTspice@..., "Dale <dchishol@c...>" <dchishol@c...>
wrote: --- In LTspice@..., "oztek_jtg <jgraham@o...>"- - - > SNIP < - - - If anybody knows of more recent works than what I previously cited, I am definitely interested in learning about them!! I've been putting together an EXCEL spreadsheet that takes a couple dozen values from the datasheet & spits out a macromodel text file, but it's not yet ready for general distribution. Dale |
|
Re: constructing opamp models
Dale <[email protected]>
--- In LTspice@..., "oztek_jtg <jgraham@o...>"
<jgraham@o...> wrote: What's the best way of creating an opamp model if the manufacturerIf you're employed as a design engineer, sometimes you can get a vendor to develop a model on request. Mere mortals have to use what's available on published data sheets and try to fit it into the component values of standard macromodel topologies. Several published works deal with this. The seminal paper is useful and readable, but later works are much better: 'Macromodeling of Integrated Circuit Operational Amplifiers', (Boyle et al), IEEE Journal of Solid State Circuits vol SC-9 (Dec 1974) Copy it from the library of any University near you that has an Engineering school, or decent Physics department. (In this area, that's Washington Univ or Univ of Mo - St Louis; even the St Louis Public Library has a LOT(!!) of the IEEE pubs on microform.) Walk in like you own the place and ask for help finding the right shelves - no librarian has ever thrown out anybody who was behaving himself. Three manufacturers have published app notes that do a pretty good job of linking data sheets to model parameters via equations: 'SPICE-Compatible Op Amp Macro-Models', (Alexander & Bowers), Analog Devices Application Note AN-138 (1990) (originally published as 'Designer's Guide to SPICE-Compatible Macromodels', in Electronic Design News (EDN), vol 35 no 4, Feb 15 1990 (Part 1) & no 5, Mar 1 1990 (Part 2)) 'Using the LTC Op Amp Macromodels', (Jung), Linear Technology Application Note 48 (1991) 'Development of an Extensive SPICE Macromodel for "Current-Feedback" Amplifiers', National Semiconductor Application Note 840 (Jul 1992) These are all available as PDF files from the respective vendors web sites, and other places on the web. Don't dismiss the National paper because it says "Current-Feedback" - most of what it says applies to modeling ANY op-amp. Along the same lines, you might look at: 'A Comprehensive Simulation Macromodel for "Current-Feedback" Operational Amplifiers', (Bowers), IEE Procedings vol 137 pg 137-145 (Apr 1990) Note that this is published by the U.K. IEE, not the American IEEE! Dale |
|
Re: Can't open library file.
Is the file really called "MYLIBRARY1.LIB" or
"MYLIBRARY1.LIB.txt"? I turn off "Hide file extension for known file types" in Explorer=>Tools=>Folder Options=>View "MYLIBRARY1.LIB" needs to be the full name of the file and it must be an ASCII file. --Mike --- "bunnyblues2001 <bunnyblues2001@...>" <bunnyblues2001@...> wrote: OK where did I go wrong, I'm getting - Could not __________________________________________________ Do you Yahoo!? Yahoo! Tax Center - forms, calculators, tips, more |
|
Can't open library file.
OK where did I go wrong, I'm getting - Could not open include file
"MYLIBRARY1.LIB" I copied the switch out of help, and the library is in the sub directory. MYLIBRARY1.lib *SYM=CSW .MODEL CSWITCH1 1 2 W1 out 0 Vsense CSWITCH1 Vsense a b 0. .model CSWITCH1 CSW(Ron=.1 Roff=1Meg Vt=0 Vh=-.5) .ENDS Version 4 SHEET 1 892 692 WIRE 448 384 448 448 WIRE 448 528 448 560 WIRE 448 560 208 560 WIRE 208 560 208 384 WIRE 208 560 208 576 WIRE 208 304 448 304 FLAG 208 576 0 SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\voltage 208 288 R0 WINDOW 123 24 132 Left 0 WINDOW 39 24 160 Left 0 WINDOW 0 42 52 Left 0 SYMATTR Value2 AC 20 SYMATTR SpiceLine Rser=1 SYMATTR InstName V1 SYMATTR Value SINE(0 20 5000) SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\csw 448 304 R0 WINDOW 0 55 20 Left 0 SYMATTR InstName W1 SYMATTR Value CSWITCH1 SYMBOL C:\PROGRAM\ FILES\LTC\SWCADIII\lib\sym\res 432 432 R0 SYMATTR InstName R1 SYMATTR Value 10 TEXT 488 560 Left 0 !.include MYLIBRARY1.lib TEXT 174 600 Left 0 !.tran 0 .1 .001 .001 * C:\Program Files\LTC\schematics\current.asc V1 N002 0 SINE(0 20 5000) AC 20 Rser=1 W1 N002 N001 CSWITCH1 R1 N001 0 10 .include MYLIBRARY1.lib .tran 0 .1 .001 .001 .backanno .end |
|
Re: New User - A question & suggestion
--- In LTspice@..., "bolocolombo <colombobolo@h...>"
<colombobolo@h...> wrote: I recently discovered LTSpice and I love the program.gate delay. I know how to do this on the netlist, but I cannot see how Ican do this from the schematic entry - when I right click on the NPN,where can I modify things like BF, Is, etc.? I have not found anythingabout this in the help. Did I miss it?Hello Bolo, I remember one method to do something like that. So at least the .STEP command allows access to the transistor's parameters. Example syntax: .STEP NPN QPMBT3904(bf) list 100, 250, 500 The simulation would run with bf=100, 250 and 500. The basic example is in the file "stepmodelparam.asc" in the "educational"-directory of SwitcherCADIII. I have attached another example that uses a .INCLUDE statement for the transistor library, because it doesn't use a model from the standard.bjt library. I think this is exactly the case you have with your ECL-gate library. Put the library file and the schematic file in the same directory. I would be ecstatic if we could plot/display S-parameters withinbut one needs to build this fictitious circuit around the real circuitin order to extract the S-parameters. And then one needs to write outhuge expressions to plot H21, MAG/MSG, and U... If Linear Technology isWhat's about to hide these long expressions in B-sources? I am interested in the S-Parameter simulations you did. Can you post some sample files with an explanation? Best Regards Helmut Circuit file "curvetrace1.asc" ----------------------------- Version 4 SHEET 1 2376 1528 WIRE 1984 1376 1984 1296 WIRE 1984 1200 1984 1152 WIRE 1984 1152 2160 1152 WIRE 2160 1152 2160 1216 WIRE 2160 1296 2160 1376 WIRE 1808 1280 1808 1248 WIRE 1808 1248 1920 1248 WIRE 1808 1360 1808 1376 FLAG 2160 1376 GND FLAG 1984 1376 GND FLAG 1808 1376 GND SYMBOL NPN 1920 1200 R0 SYMATTR InstName Q1 SYMATTR Value QPMBT3904 SYMBOL voltage 2160 1200 R0 SYMATTR InstName V1 SYMATTR Value 0. SYMBOL CURRENT 1808 1360 M180 WINDOW 0 24 88 Left 0 WINDOW 3 24 0 Left 0 SYMATTR InstName I1 SYMATTR Value 0. TEXT 1768 1440 Left 0 !.dc V1 0 15 10m I1 50u 100u 50u TEXT 1416 1512 Left 0 ;This example schematic is supplied for informational/educational purposes only. TEXT 1696 1080 Left 0 !.step NPN QPMBT3904(bf) list 100, 1000 TEXT 1696 1120 Left 0 !.include philips.lib Library "philips.lib" ----------------------- * .MODEL QPMBT3904 NPN( + IS=4.639E-15 + NF=0.9995 + ISE=2.091E-14 + NE=1.6 + BF=160.1 + IKF=0.12 + VAF=98.69 + NR=1.001 + ISC=3.257E-12 + NC=1.394 + BR=5.944 + IKR=0.06 + VAR=19.29 + RB=1 + IRB=1E-06 + RBM=1 + RE=0.3614 + RC=1.755 + XTB=0 + EG=1.11 + XTI=3 + CJE=5.631E-12 + VJE=0.7002 + MJE=0.3385 + TF=3.001E-10 + XTF=27 + VTF=1.461 + ITF=0.2723 + PTF=0 + CJC=4.949E-12 + VJC=0.5969 + MJC=0.1928 + XCJC=0.864 + TR=9.4E-8 + CJS=0 + VJS=0.75 + MJS=0.333 + FC=0.5582 ) * |
|
New User - A question & suggestion
I recently discovered LTSpice and I love the program.
My question is the following: I wish to modify the model parameters of say, the NPN bipolar transistor, so as to see the impact of various parameters on ECL gate delay. I know how to do this on the netlist, but I cannot see how I can do this from the schematic entry - when I right click on the NPN, where can I modify things like BF, Is, etc.? I have not found anything about this in the help. Did I miss it? Suggestion: I appreciate LTSPice is "free", so one can only do so much work on it in terms of filling requests... But here is mine anyway. I would be ecstatic if we could plot/display S-parameters within LTSpice, in a Smith Chart and Bode format. I managed to plot them, but one needs to build this fictitious circuit around the real circuit in order to extract the S-parameters. And then one needs to write out huge expressions to plot H21, MAG/MSG, and U... If Linear Technology is interested in the RF market, it might make sense to add S-parameter tools down the line. Being able to export data w/o the Ltutil.exe would be good too. Thanks for a great tool. Cheers! Bolo |
|
Re: how to use cell attributes to bind a symbol to a subcircuit
I need a method to bind schematics to cell andYou can do this if the symbol is modeled with a subcircuit. It's described in one of the downloads of this group and now also in the help section Schematic Capture=>Creating New Symbols=>Adding Attributes: There is a special combination of attributes that will cause a required library to be automatically included in every schematic that uses the symbol: Prefix: X SpiceModel: <name of file including the spicemodel> Value: <What ever you want vis. on the schematic> Value2: <The value as you want in the netlist> If the device is modeled with a .model card, then you need to put the .model statement in the appropriate standard.* file. --Mike __________________________________________________ Do you Yahoo!? Yahoo! Shopping - Send Flowers for Valentine's Day |
|
how to use cell attributes to bind a symbol to a subcircuit
I need a method to bind schematics to cell and block symbols that uses the
symbol attributes, so that instantiating and placing a symbol causes that symbol's definition to be included as a subcircuit in the netlist. This needs to work a) when the symbol and schematic have the same name (albeit with differing extensions), b) when the symbol and schematic have different names (e.g., "XXX.asy" bound to "simplified_XXX.asc"), and c) when a generic symbol is bound after placement to a specific differently-named schematic (e.g., when binding different power supply designs into a common test framework). File hierarchy location of the files for the symbols and schematics is not important, as long as they are not placed under the SCad3 Program Files hierarchy. (They aren't LTC's.) The solution could require that all of the symbols and schematics files be in the same folder, probably the folder on which SCad3 is focussed. Or the solution could require replicating a lib hierarchy under the folder on which SCad3 is focussed. Or ??? Requiring the instantiating user to know the correlation between symbol and schematic and add a .lib statement for each such is unacceptable, just as it would be were a .lib to be needed for each LT part and discrete that is added to a schematic. Besides, adding a .lib statement does not solve the problem of binding a symbol with one name to an instance with a different name, as occurs in the LT-provided symbols (e.g., CNY17-3.asy binding to CNY17.sub as in last example below) Placing a pre-bound symbol should be adequate when the symbol has a fixed binding to a subcircuit netlist. Placing an unbound symbol and setting one or two of the symbol instance's attributes to the name of the netlist should be adequate for binding a generic symbol to one of a set of equivalent netlists. (Note that a .lib cannot accomplish this, particularly when two identical generic symbols in the schematic are bound to different instance values, as occurs regularly with generic symbols for discretes.) I've tried binding the schematic to the symbol definition and/or to the symbol instance via the SpiceModel attribute. I've also tried binding it via the SpiceLine2 attribute by putting a "\n.lib " prefix before the schematic name, hoping that this would cause SCad3 to treat this as a separate hidden .lib declaration. Neither of these approaches works. Nor does removing the represented cell's or block's name, which is otherwise appended to the constructed SPICE line after the SpiceModel field. (Incidentally, cell's _do_ need names, so removing the name would not be an acceptable method either. But it was worth trying.:) Has anyone solved this problem? Does anyone have any suggestions? Is there a methodology for adding bogus pins to the symbol to cause the SPICE parse of the constructed SpiceLine to work? Mike? Helmut? Others? Two example symbols and schematics follow: **attempt to use SpiceModel attribute** ==============diode bridge symbol================ Version 4 SymbolType CELL LINE Normal -20 16 -20 -16 LINE Normal -44 16 -44 -16 LINE Normal -44 -16 -20 0 LINE Normal -44 16 -20 0 LINE Normal -64 0 -44 0 LINE Normal -20 0 0 0 LINE Normal 60 64 60 32 LINE Normal 36 64 36 32 LINE Normal 36 32 60 48 LINE Normal 36 64 60 48 LINE Normal 0 48 36 48 LINE Normal 60 48 80 48 LINE Normal 60 16 60 -16 LINE Normal 36 16 36 -16 LINE Normal 36 -16 60 0 LINE Normal 36 16 60 0 LINE Normal 16 0 36 0 LINE Normal 60 0 80 0 LINE Normal -20 -32 -20 -64 LINE Normal -44 -32 -44 -64 LINE Normal -44 -64 -20 -48 LINE Normal -44 -32 -20 -48 LINE Normal -64 -48 -44 -48 LINE Normal -20 -48 16 -48 LINE Normal 16 -48 16 -48 LINE Normal 16 0 16 -48 LINE Normal 80 -48 16 -48 LINE Normal 0 48 0 0 LINE Normal -64 48 0 48 RECTANGLE Normal 80 72 -64 -71 TEXT -16 -96 Left 0 BRW40 WINDOW 0 -51 59 Left 0 SYMATTR Prefix X SYMATTR Description Diode bridge SYMATTR SpiceModel BRW40.asc PIN -64 -48 NONE 0 PINATTR PinName A1 PINATTR SpiceOrder 1 PIN -64 0 NONE 0 PINATTR PinName A2 PINATTR SpiceOrder 2 PIN -64 48 NONE 0 PINATTR PinName AC2 PINATTR SpiceOrder 3 PIN 80 48 NONE 0 PINATTR PinName C2 PINATTR SpiceOrder 4 PIN 80 0 NONE 0 PINATTR PinName C1 PINATTR SpiceOrder 5 PIN 80 -48 NONE 0 PINATTR PinName AC1 PINATTR SpiceOrder 6 ==============diode bridge model================ Version 4 SHEET 1 1504 692 WIRE 256 256 240 256 WIRE 272 384 240 384 WIRE 240 320 240 384 WIRE 240 384 176 384 WIRE 256 256 256 320 WIRE 256 256 336 256 WIRE 256 320 272 320 WIRE 176 256 160 256 WIRE 176 320 160 320 WIRE 336 320 352 320 WIRE 336 384 352 384 FLAG 176 384 AC2 IOPIN 176 384 In FLAG 336 256 AC1 IOPIN 336 256 In FLAG 160 256 A1 IOPIN 160 256 Out FLAG 160 320 A2 IOPIN 160 320 Out FLAG 352 320 C1 IOPIN 352 320 Out FLAG 352 384 C2 IOPIN 352 384 Out SYMBOL diode 272 336 R270 WINDOW 0 32 32 VTop 0 WINDOW 3 0 32 Invisible 0 SYMATTR InstName Dc1 SYMATTR Value DBRW SYMBOL diode 272 400 R270 WINDOW 0 32 32 VTop 0 WINDOW 3 0 32 Invisible 0 SYMATTR InstName Dc2 SYMATTR Value DBRW SYMBOL diode 176 336 R270 WINDOW 0 -30 28 VTop 0 WINDOW 3 0 32 Invisible 0 SYMATTR InstName Da2 SYMATTR Value DBRW SYMBOL diode 176 272 R270 WINDOW 0 -31 29 VTop 0 WINDOW 3 -124 4 VRight 0 SYMATTR InstName Da1 SYMATTR Value BRW40 TEXT 168 488 Left 0 !.model BAS40BRW D(Ron=0.1 Roff=2meg Vfwd=0.6 Vrev=40 Rrev=0.1 mfg="Diodes Inc"); pn="BAS40BRW") RECTANGLE Normal 344 406 169 233 Similarly for BRW70, which references a 70V (Vrev=70) BAS70BRW part. **attempt to use SpiceLine2 attribute with leading "\n.lib "** ==============optoisolator w. shunt reference symbol============= Version 4 SymbolType CELL LINE Normal 96 -64 56 -64 LINE Normal 56 -48 56 -64 LINE Normal 56 -24 56 0 LINE Normal 96 0 56 0 LINE Normal 72 -48 40 -48 LINE Normal 56 -24 40 -48 LINE Normal 56 -24 72 -48 LINE Normal 72 -24 40 -24 LINE Normal -96 -48 -68 -48 LINE Normal -96 16 -72 16 LINE Normal -40 -16 -68 -48 LINE Normal -40 -16 -60 4 LINE Normal -40 -32 -40 0 LINE Normal -72 16 -56 8 LINE Normal -72 16 -64 0 LINE Normal -56 8 -64 0 LINE Normal -24 -32 -12 -36 LINE Normal -24 -32 -20 -44 LINE Normal -20 -36 -24 -32 LINE Normal 72 20 72 28 LINE Normal 72 20 40 20 LINE Normal 40 20 40 12 LINE Normal 72 44 40 44 LINE Normal 40 44 56 20 LINE Normal 72 44 56 20 LINE Normal 56 64 56 44 LINE Normal 56 20 56 0 LINE Normal 96 64 56 64 LINE Normal 64 32 96 32 RECTANGLE Normal 96 -80 -96 80 ARC Normal 4 -20 -20 -44 4 -32 -16 -36 ARC Normal 28 -20 4 -44 4 -32 28 -28 WINDOW 0 0 -64 Center 0 WINDOW 3 -31 64 Center 0 SYMATTR Value FOD2741 SYMATTR Prefix X SYMATTR Description Shunt reference and optoisolator, transistor output PIN 96 -64 NONE 0 PINATTR PinName LED PINATTR SpiceOrder 1 PIN 96 0 NONE 0 PINATTR PinName COMP PINATTR SpiceOrder 2 PIN 96 32 NONE 0 PINATTR PinName FB PINATTR SpiceOrder 3 PIN 96 64 NONE 0 PINATTR PinName GND PINATTR SpiceOrder 4 PIN -96 16 NONE 0 PINATTR PinName E PINATTR SpiceOrder 5 PIN -96 -48 NONE 0 PINATTR PinName C PINATTR SpiceOrder 6 ==============optoisolator w. shunt reference model============= Version 4 SHEET 1 1024 740 WIRE 288 416 288 464 WIRE 224 400 224 464 WIRE 384 400 384 464 WIRE 208 144 528 144 WIRE 208 240 224 240 WIRE 16 144 0 144 WIRE 16 208 0 208 WIRE 224 320 224 240 WIRE 224 240 528 240 WIRE 368 320 384 320 WIRE 288 320 288 352 WIRE 432 336 480 336 WIRE 224 464 288 464 WIRE 288 464 384 464 WIRE 384 464 432 464 WIRE 432 464 480 464 WIRE 432 384 432 464 WIRE 480 464 528 464 WIRE 480 384 480 336 WIRE 480 336 528 336 FLAG 0 144 c IOPIN 0 144 In FLAG 0 208 e IOPIN 0 208 Out FLAG 528 144 LED IOPIN 528 144 In FLAG 528 240 comp IOPIN 528 240 BiDir FLAG 528 336 fb IOPIN 528 336 In FLAG 528 464 ground IOPIN 528 464 Out SYMBOL %SCAD3%\lib\sym\Optos\CNY17-3 112 208 M0 SYMATTR InstName U1 SYMBOL %SCAD3%\lib\sym\e 384 304 M0 WINDOW 0 -14 57 Left 0 WINDOW 3 -72 58 Invisible 0 SYMATTR InstName E1 SYMATTR Value 1.0 SYMBOL %SCAD3%\lib\sym\current 480 384 R0 WINDOW 0 -22 35 Left 0 WINDOW 3 32 20 Left 0 WINDOW 123 0 0 Left 0 WINDOW 39 33 43 Left 0 SYMATTR InstName I1 SYMATTR Value 5.2 SYMATTR SpiceLine load SYMBOL %SCAD3%\lib\sym\f 224 320 R0 WINDOW 0 -28 36 Left 0 WINDOW 3 3 35 Left 0 SYMATTR InstName F1 SYMATTR Value E1 SYMATTR Value2 -1.0 SYMBOL %SCAD3%\lib\sym\zener 304 416 R180 WINDOW 0 -35 32 Left 0 WINDOW 3 -55 3 Left 0 SYMATTR InstName D1 SYMATTR Value Z2.5V SYMBOL %SCAD3%\lib\sym\res 384 304 R90 WINDOW 0 0 83 VBottom 0 WINDOW 3 -28 45 VTop 0 SYMATTR InstName R1 SYMATTR Value 10 TEXT -40 552 Left 0 !.model Z2.5V D(Ron=0.1 Roff=2meg Vfwd=2.5 Vrev=0.35 Rrev=0.1)\n.lib CNY17.sub TEXT 96 336 Left 0 ;current\nmirror TEXT 400 280 Left 0 ;voltage\nmirror |
|
Re: Need a model for a gas discharge tube (spark gap) and general help.
On Thu, 13 Feb 2003 20:55:11 -0000, bunnyblues2001@... wrote:
I need a model for a gas discharge tube similar to the Siemens A81-Spectrum Software (makers of MicroCap) has an application note concerning gas tubes at While the syntax might be different from LTSpice, the schematics should get you started. ----- Pat Lawler <pat.lawler@...> |
|
Re: "Timestep too small" error while simulation
--- In LTspice@..., "analogueman2002 <rd.weaver@n...>"
<rd.weaver@n...> wrote: --- In LTspice@..., "Helmut Sennewaldwrote: usedMike, could you tell us what tolerance is used in what type of complexin .TRAN simulation. I would try the settings below.Hello Gents, business but here is a sequence of things to try which has beenfound useful by many Spice users. It applies to .TRAN convergenceproblems which occur some way into the simulation rather than at thebeginning. Hello Russell and Mike, thanks for your advices to solve convergence problems. I will keep your messages in my archive, because I am shure that every SPICE user will run into these problems from time to time. I recommend to spend a chapter about this in the help pages of LTSpice. Best Regards Helmut |
Mike Engelhardt
to navigate to use esc to dismiss