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
Search
I'm ready to give up LTC all toghether.
|
I'mready to give up LTC all toghether.
The only think that made me use ltC components was the simulator. These guys in their plush officess have no idea how important the simulato ris for their bussines. Otherwise they would had put some more muscle behind Mike. i uploaded Draft 1.asc. I can not believe that such a simple think robbed me of an hour from my real work. G. |
|
Gunoi Nare
Thank you Helmut. Could you please point me to the place in the simulator help file that decribes what you have just done? G. BTW. The program is newer guilty. The Programmer/Technical Writer, yes! G.
|
|
G,
Calm down for five minutes and consider all those who had to design circuits without circuit simulators and nice assemblers to write machine code for them. Dave N From: LTspice@... [mailto:LTspice@...] Sent: 15 August 2016 12:26 To: LTspice@... Subject: [LTspice] I'm ready to give up LTC all toghether. I'mready to give up LTC all toghether. The only think that made me use ltC components was the simulator. These guys in their plush officess have no idea how important the simulato ris for their bussines. Otherwise they would had put some more muscle behind Mike. i uploaded Draft 1.asc. I can not believe that such a simple think robbed me of an hour from my real work. G. |
|
Gunoi Nare
Yes, Helmut, i saw it. However, I was looking for a definition of Trise etc. that really does not exist in the help file.. From what level to what level is the simulator considering the rise of a signal? Is Trise a .parameter , a key word or what?. How do you handle it' s substitutions. i guess you understand . BTW. If you leave unused pins of the gate just floating, how do you simulate latch-up conditions? I belive that the digital lib has a lot to desire. Some standard values had to be plugged in the symbols so they would be imediattely usable. If the user needs to tweak them, so be it. Is there a way for me to modify the lib so the components would have already some dummy values? One more time, thank you. g
|
|
Don't do down one of the most brilliant pieces of freeware ever!
If you want exhaustive help files and training try paying lot's and lot's of $$$$ for a product.? As for myself and am sure many many others we don't have $$$$$ and rely on people such as those at Lt to give away there hard work for free for the benefit of others.? I think as you use it will grow on you...good luck :) |
|
Gunoi Nare
If you ever think that you have found something FREE, THINK AGAIN G
|
|
Hello,
>?BTW. If you leave unused pins of the gate just floating, how do you simulate latch-up conditions? I guess you haven't heard about the idea of the digital A-devices. These devices should be as fast as possible in the simulation and only add small complexity. Unused pins should be left open. This allows the compiler to reduce a five-input AND to a two input AND when you only apply two signals.? When you want simulate latchup, you have to create and a add subcircuit with a ?SCR structure. Before you waste time on that, you have to characterize the latchup behavior of the target IC. Best regards, Helmut ? |
|
I also do not understand why the characters do not have the required parameters. Many people come to rake because of this. Since LtspiceIV in the near future will not be updated (if ever updated), then you yourself can change the characters of A-type. I advise you to make a reserve of symbols changed. Then you will simply use logic gates. I think the default is to make the output levels 5V and td = 5ns, Trise = 2.5 ns.
toggle quoted message
Show quoted text
Bordodynov. 15.08.2016, 16:13, "Gunoi Nare gunoiar@... [LTspice]" <ltspice@...>: Yes, Helmut, i saw it. |
|
At 07:08 AM (-0700) 8/15/2016, davnor49 wrote:
---------- Original Message ---------- G,---------- End of Original Message ---------- Yep. I amuse myself periodically by remembering that I designed ASIC's for 18 years before I had my hands on a simulator, and that was Berkeley Spice 2G6 on a VAX. And there was no schematic capture... I had to draw schematics on paper, number the nodes, then type up a netlist :-D In a way I think that's an advantage... I design circuits in my head, on paper, and with a calculator, then enter them into a simulator for verification. I find that many young engineers have no ability to IMAGINE a circuit. ...Jim Thompson Web Site: <> |
|
Gunoi Nare, let me offer my "take" on this. LTspice's A-devices like the one you used, originally were for LTC's internal use only and not documented at all.? Then Mike made them available for anyone to use and provided minimal documentation, in the Help page for them ("A. Special Functions"). As most of us here in this group know and occasionally discuss, LTspice's Help documentation is and has always been short on details.? We are OK with that because the program that comes with it, is so incredible.? The Help file alone really is not a good way to go from the ground up, to having a solid understanding of how to use LTspice, or SPICE in general.? There are other resources that help fill in the missing pieces.? But there also is a general understanding (partly learned from experience) about how SPICE/LTspice work, which might have prevented this problem that you had. I think you are correct that many of the Symbols that come built into LTspice, ought to have some parameters already attached to them, so that we don't have to always dig up the documentation or remember which ones we need to add.? That is especially true about the A-devices.? For example, I occasionally use the Modulate (VCO) component, and it doesn't work without the parameters Mark and Space -- so why doesn't LTspice have those two already attached to the symbol before I ever use it?? It's a good question, with no real answer.? That's just the way it is. ?(I suppose Mike might say that the standard library is "clean" with no parameters attached, because attaching parameters is the job of the user, or something like that.) However, you can edit those symbols!? Just open them in LTspice and attach the parameters yourself, and save them -- ASSUMING that Windows lets you! ?(It might not, if you installed LTspice in the Windows "Program Files" area.) ?Then they will be attached already whenever you use that symbol. ?(This answers your question,?"Is there a way for me to modify the lib so the components would have already some dummy values?") ?I'm not sure if they will last through an LTspice program update, but that's a separate issue. Now, let's examine why your schematic didn't work. You defined .PARAMs which you named TRISE and THIGH, and then used them within {braces}.? Using braces converts the user-defined .PARAMs into pure numbers.? So your NAND gate, A1, had the parameters 5.0e-9 and 3.0 attached to it -- but with nothing telling the SPICE engine (internal to LTspice) what they are for.? Think of it this way.? The schematic editor says that you have a NAND gate, with parameters 0.000000005 and 3.0.? And that's all it says.? Once those user-defined .PARAMs have been converted into numbers, everything downstream doesn't know that you named them TRISE or ELEPHANT. Even if the SPICE engine knew that you named them "TRISE" and "THIGH", it wouldn't help, because user-defined .PARAMs have names that are meaningful only to YOU.? LTspice doesn't (for the most part) care what names you use, and doesn't interpret them. User-defined .PARAM names are your private names. The NAND gate needs those values given to it as "name=number" pairs.? It needs to see "Trise=5ns" or "Trise=0.000000005" or "Trise={trise}" or "Trise={elephant}.? Otherwise, it doesn't know what to do with the number. This can be confusing, because SPICE is not 100% consistent about that.? With a resistor, you can use just the resistance value (a number), without having to say "Res=470".? But that pretty much only works with the things that SPICE (40+ years ago) defined that way.? Most other parameters need to have the "name=number" form, when they appear on the device that uses them. Here's a tip.? In SPICE, if a number must be used in a particular order, then probably it is used as a number alone. ?(Examples: the .TRAN statement, or the PULSE voltage source.) ?If the order doesn't matter, then it must always be used in "name=number" form. ?(Examples: all the values of a .MODEL statement, and all parameters attached to A- and B-elements.) Andy |
|
Replying to a few specific questions from Gunoi Nare: ? ?"However, I was looking for a definition of Trise etc. that really does not exist in the help file.." Well, it does.? In the Help page for A-devices, "Trise" etc. are in the table of parameters. ? ?"From what level to what level is the simulator considering the rise of a signal?" I think it is from 0% to 100%.? But your results may vary, depending on the Maximum Timestep of the simulation, as well as waveform compression (whether you have ".options plotwinsize=0"). ? ?"Is Trise a .parameter , a key word or what?. How do you handle it' s substitutions." Trise can be both, which can make it confusing if you don't keep them straight. As you used it, Trise was a USER-defined parameter and has meaning only to you. When you attach "Trise=5ns" to a NAND gate, it is an instance parameter of that NAND gate. When you attach "Trise={foo}" to a NAND gate, the user-defined parameter "foo" is substituted with its numeric value, which is then assigned to the instance parameter "Trise". When you attach "Trise={Trise}" to the NAND gate, the user-defined parameter "Trise" is substituted with its numeric value, which is then assigned to the instance parameter "Trise".? This "Trise" is totally different than your user-defined parameter by the same name. ? ?"BTW. If you leave unused pins of the gate just floating, how do you simulate latch-up conditions?" You were using the built-in NAND gate which is an A-device, and is not a real gate.? It has no transistors.? It has no latch-up, and no problem with inputs floating.? In fact, floating inputs are preferred, if you don't actually use them. If you want to simulate latch-up, you would have to come up with a real circuit for your own NAND gate. Regards, Andy |
|
John Woodgate
¿ªÔÆÌåÓýThe formal definitions of rise time and fall time relate to 10 % and 90 % of the amplitude, because it's not possible to say precisely when the pulse is no longer 0 % and when it first reaches 100 %. ? To find how LTspice interprets them, define a pulse with millisecond values and look at its waveform, with .opt plotwinsize=0. ? With best wishes DESIGN IT IN! OOO ¨C Own Opinions Only J M Woodgate and Associates Rayleigh England ? Sylvae in aeternum manent. ? From: LTspice@... [mailto:LTspice@...] ? ? Replying to a few specific questions from Gunoi Nare: |
|
John wrote: ? ?"The formal definitions of rise time and fall time relate to 10 % and 90 % of the amplitude, because it's not possible to say precisely when the pulse is no longer 0 % and when it first reaches 100 %." That is correct for the method to use to measure rise time and fall time in the lab, where real signals are not straight with sharp corners. But for generating step waveforms in SPICE, the prescribed rise and fall times refer to the 0% and 100% points of the waveform edges.? This is the convention that UC/Berkeley adopted when they created SPICE some 40 years ago, and LTspice conforms to that convention. It definitely applies to the PULSE voltage and current source waveforms, and it apparently applies here (to the [Digital] library of A-devices) too.? I just tried it with a NAND gate, and that is what I saw. I did see some curvature in the output waveform, near the end of the edge, so it is not a strictly linear ramp, but it's close.? So, the specified Trise or Tfall works for approximately the 0% to 97% or 99% points (on the cases I tried -- it depends on risetime).? But the slope over most of the edge fits as if it were 0% to 100%. Regards, Andy |
|
John Woodgate
¿ªÔÆÌåÓýYes, you did what I advised and found the definitive answer. ? With best wishes DESIGN IT IN! OOO ¨C Own Opinions Only J M Woodgate and Associates Rayleigh England ? Sylvae in aeternum manent. ? From: LTspice@... [mailto:LTspice@...]
Sent: Monday, August 15, 2016 7:43 PM To: [LTspice] group Subject: Re: [LTspice] Re: I'm ready to give up LTC all toghether. ? ? John wrote: ? ? ?"The formal definitions of rise time and fall time relate to 10 % and 90 % of the amplitude, because it's not possible to say precisely when the pulse is no longer 0 % and when it first reaches 100 %." ? That is correct for the method to use to measure rise time and fall time in the lab, where real signals are not straight with sharp corners. ? But for generating step waveforms in SPICE, the prescribed rise and fall times refer to the 0% and 100% points of the waveform edges.? This is the convention that UC/Berkeley adopted when they created SPICE some 40 years ago, and LTspice conforms to that convention. ? It definitely applies to the PULSE voltage and current source waveforms, and it apparently applies here (to the [Digital] library of A-devices) too.? I just tried it with a NAND gate, and that is what I saw. ? I did see some curvature in the output waveform, near the end of the edge, so it is not a strictly linear ramp, but it's close.? So, the specified Trise or Tfall works for approximately the 0% to 97% or 99% points (on the cases I tried -- it depends on risetime).? But the slope over most of the edge fits as if it were 0% to 100%. ? Regards, Andy ? |
|
Gunoi Nare
Thank you Andy. I do know these "facts" but simulator programmers have a tendency to "improve" on the agreed parameters. It is always wise to ask what the programmer thinks in this respect. G.
|
|
Gunoi Nare
"I find that many young engineers have no ability to IMAGINE a circuit." Well said Jim :) G.
|
|
> I did see some curvature in the output waveform, near the end of
the edge, so it is not a strictly linear ramp, but it's close.? So, the
specified Trise or Tfall works for approximately the 0% to 97% or 99%
points (on the cases I tried -- it depends on risetime).? But the slope
over most of the edge fits as if it were 0% to 100%. I think that's LTspice's engine doing its best to keep the derivatives smooth. The same is valid for the default (ideal) diode, for example. When run and zoomed in, the sharp knee is not so sharp. If the timestep is decreased, zooming in until only a few points around the knee are visible reveals the same slight smoothing, and it keeps on going. Even A-devices pulses, unaltered, have a tendency to show a slightly non-linear rise from 0 to 1 or vice-versa. It's just a guess, but it seems to go well along Mike's own words.Vlad ______________________ -- holding, among others: a universal analog/digital filter, block-level models for power electronics (and not only), math blocks with a more stream-lined approach, some digital ADC, DAC, (synchronous-)counter, JKflop, etc. |
to navigate to use esc to dismiss