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
|
LTspice running under Linux
In my PC running Linux (SuSe 8.1) I installed wine, then I installed
SwitcherCADIII. The program seems to work well, I have only a little problem, I am not able to update the program using internet.If I try to sync release I get the the message "could not access web ..." I have the connection to internet active, but I get this message. I dont know if using wine it is possible to update the program. Someone can help me ? Stefano Delfiore |
|
Re: computed expression values
Jonathan Kirwan
On Sat, 8 Mar 2003 13:58:35 -0800 (PST), you wrote:
Thanks for that wonderful letter you wrote. IHehe. Sure! I want folks at Linear to realize it's all appreciated. For your question, it might help you to know thatWorks for me. Looks good. Thanks! ... Is there way to get the peak-to-peak over a specific time range? One simple calculation I'd like to do is to get a close estimate of the gain figure by, say, dividing the output p-p by the input p-p. But I want this figure computed, based on the time range of, say, t0=100ms to t1=200ms? I'm also going to have to figure out a simple way to look at effects of temperature variation and component variation on gain and DC quiescent point, again only over a specified time range. What about computing group delay through a filter or amplifier? And can LT Spice conserve or account for charge in the calculations? Sorry, I keep wondering about all the possibilities, now. Jon |
|
Re: computed expression values
Jon,
Thanks for that wonderful letter you wrote. I forwarded it to the Chief Technical Officer at Linear. Hope that's okay. For your question, it might help you to know that you can see what your {} expressions evaluated to in this manner: 1. Go to Tools=>Control Panel=>Operation. 2. Check "Generate Expanded Listing" 3. Then, after you run the simulation, make the schematic the active window and use the menu command View=>SPICE Error Log. In the listing you will see how the {} expressions were evaluated. Anyway, that's how I do it. Regards, --Mike __________________________________________________ Do you Yahoo!? Yahoo! Tax Center - forms, calculators, tips, more |
|
computed expression values
Jonathan Kirwan
I want to start out by saying that I'm a hobbyist, not an
electronics professional. When I first heard of SwitcherCAD III/LT Spice perhaps a year ago, I went to the Linear web site with the intent to download the program and completely failed to understand what I almost had in hand. From the descriptions, it looked like some kind of specialized program for switcher-based power supplies and that was far too limited to be very interesting at the time. It wasn't until later reading of comments by one of the active members of the LT Spice team (Mike) that I began to realize my mistake and attempted to download LT Spice in January. Boy, was that a good decision. In the past, I've tried, and actually purchased, a few other programs claiming to provide electronics simulations. I've had a crashed Windows, substantial memory leaks, and overly complex setup for simulation and overly complex arrangements to observe the signal values I'm interested in (in some cases, having to manually wire up a "meter" in order to get those results, and even then with difficulty.) By comparison, and this isn't simply a false impression because of my building on prior experience, LT Spice was a dream to use. Once I set down to seriously confront a simple circuit, it took me no time at all (and without reading any help files) to create it and get results I was interested in seeing. This stands in stark contrast to past experience. As I've spent a little more time in LT Spice, every moment has been well paid back by discovery of still more useful and interesting features. It's actually such a joy, that I've gone out and purchased an original Spice II PhD thesis from 1975, recommended by Mike, and another similar book and have found all of it very useful. Every minute has been well-paid and I can barely imagine a tool which is easier to use. Of course, I'm still too much a neophyte, both in electronics knowledge as well as in simulation depth, to know whether or not this program provides simulations which are incorrect in some important details and which will lead me into very wrong impressions which will be hard to unlearn. But I'm pretty confortable in my current belief, tested in a few cases I've actually built and used, that it's providing good results. And comforted aslo by the active support of this program. All that is by way of introduction for a question I have: I've taken advantage of .param in order to allow me to specify certain important values for a basic degenerative amplifier design. The components used in this model design are all specified with expressions using the set signs, {}. Simulation results look encouraging to me, now, but I'd like to see what the results of the calculations for these expressions were, in simulation, so that I can now specify real values and build one for testing. I could go use my calculator, of course, and figure these out. But I'd like LT Spice to display the results of its own calculations without my having to use a calculator, by hand. Is this easily doable? My guess is that I could write an expression into the graphical display as another trace and just see the value of the straight line, but that's not a good way to do this. What I'm considering as "nice" would be to right-click over the expression on the schematic and call up a dialog box for extering the expression, but where this dialog box would *also* show the current result of the existing expression. Anyway, that's my question for now. Thanks to all! Jon |
|
Re: Analog MUX
--- In LTspice@..., "Helmut Sennewald
<helmutsennewald@y...>" <helmutsennewald@y...> wrote: --- In LTspice@..., "polapart <sahawley@m...>"two more following inverters. The output of the first inverter wasor MP2 has to be connected to node '4'. I supposed MP2. The simulationlibrary. Hello, I reported this bug to Philips. Today I have got feedback that my correction of this model has been correct. They promised to fix it in their library until mid of March. Best Regards Helmut |
|
Re: Vacuum tube models in LTspice?
--- In LTspice@..., "Helmut Sennewald
<helmutsennewald@y...>" <helmutsennewald@y...> wrote: --- In LTspice@..., Bill Lewis <wrljet@y...> wrote:And again some more information.Thanks! I'm checking it out now.Hello Bill, The model in my example file is from this link: Another source is: Best Regards Helmut |
|
Re: Vacuum tube models in LTspice?
--- In LTspice@..., Bill Lewis <wrljet@y...> wrote:
Thanks! I'm checking it out now.Hello Bill, I forgot to mention that the symbols for the triode, tetrode and pentode are all in the "misc" directory of LTSpice. I am not shure you were aware of that. Best Regards Helmut |
|
Re: Vacuum tube models in LTspice?
Bill Lewis
Thanks! I'm checking it out now.
Bill --- "Helmut Sennewald <helmutsennewald@...>" <helmutsennewald@...> wrote: --- In LTspice@..., "Bill Lewis <wrljet@y...>" __________________________________________________ Do you Yahoo!? Yahoo! Tax Center - forms, calculators, tips, more |
|
Re: Vacuum tube models in LTspice?
--- In LTspice@..., "Bill Lewis <wrljet@y...>"
<wrljet@y...> wrote: Has anyone migrated any of the vacuum tube models floatingHello Bill, I did it once for a pentode. The model is included in the schematic, but this can be changed using a library file valve.lib. Then add instead .include valve.lib in the schematic. It is very important to look on the used pin order. Everybody has another pin order used in his library. It have to be changed according to the pin order of your symbol or you make your own symbol with the appropriate pin order. I couldn't attach it, because the lines will be split by this awful YAHOO reader. I put it into this group's Files->examples->apps folder. It is the file "pentode.asc". Best Regards Helmut |
|
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 |
Mike Engelhardt
to navigate to use esc to dismiss