The thing is, do I change them in those lib folders in the Spice menu? Or elsewhere?
The general idea is covered here,
https://adamsiembida.com/adding-spice-models-to-ltspice/A few of things worth adding:
- you can add models to your project folder, which is only available to the project,
or, you can add them to the LTspice folders so they are available to all project.
The precise location of the folders depends on you OS, it's in the article.
- Normally you have to put a .lib or .inc on your schematic.
- You can put a heap of .models or .subckts in the one file to make a project library
or you own personal library.
- The article talks about the <system path> \lib\sub folder. There's also stuff
in the <system path> \lib\cmp folder.
- On LTspice I haven't worked out how to add you own library without adding .lib or .inc;
just as you don't need to add .lib or .inc for the "builti-in" LTspice parts
So you’re saying they’re low, as for they’re wrong?
What is now pissing me is that R.G does refer to the values measured as VGSoff somewhere in the text, which is not correct…
They are only wrong if you interpret them as VGS_off. Some people have complained about this in the past. The values produced by RG's tester are fine for matching. However, yes, calling it VGS_off does cause problems; I guess that's my only beef. The main problem is people on the group use different testers and that don't say which one they use. So when people put up their VGS measurements you have no idea how to interpret the value. If people say which tester they use then at least you can correct the values from RG's using the correction factor I calculated (or one like it).
I did the testiings changing the input (AC small-signal) and putting there a probe (and the gain). Here you go:
Voltages are 0.1, 0.5, 1, 2, 15 V.
OK I get it.
When you plot gain (Vout/Vin) you *expect* the gain to be constant with level. If you have a gain of 10 (20dB), 1V in is 10V out and 2V in is 20V out but in both cases Vout/Vin is 10 (or 20dB). The whole reason for plotting Vout/Vin was to get a gain which is independent of Vin! The other alternative, which is what I prefer, is to plot Vout and use 1V inputs. That way plotting Vout is the same as gain. However, if for some reason you want to see the output voltage for a different input you just chain it - since you changed it you don't expect to see gain anymore.
I doesn't matter which way to you do so long as you know how to interpret the results - otherwise you will be scratching your head in frustration! (And no, I'm not immune to this even after 35 years of using spice, I just do it less often.)
Alright, that’s important. But you don’t go there verifying every component you use, or do you? Like really seriuosly, if I would do that it “seems” (because it’s just a guess) that it would take a very long time.
So the main problem is if you *never* check against reality you are just seeing numbers on the computer. They could be anything. One simple check against reality is what you expected, perhaps from rough calculations, perhaps from when you build the real unit, perhaps from experience, perhaps from common sense.
Beyond that yes it's a big job. So the idea is you use existing models, if they look wrong, find another one. If you develop a mistrust for all the models you need to check against reality. Then if you are convinced all the models suck you need to create your own.
To tell you the truth I vary rarely enter a whole circuit from the "design" schematic into spice. I use the least amount of models possible. For example a circuit might have an oscillator using a NE555 timer. I don't use the NE555 I use a spice square wave or rectangular wave. That replaces 50 parts in a possibly non-working model with one part which has to work. If I'm simulating AC response I never use opamp models ie. the ones with a power supply. For opamps I'd use something like the 'opamp' model and type-in the Gain and Bandwidth product into the parameters. For a zener I use a voltage source.
For the phaser AC response I'd probably enter most of it like you have but with the simpler opamp model. I would replace the LFO with a DC fixed DC voltage. I might simulate the LFO separately to work out the peak to peak output voltage and frequency. If I wanted the LFO I'd probably use spice voltage source to create a triangle wave.
Basically I don't *rely* on models. My simulations are probably 10 times faster than most peoples. They much easier to debug because most of it *has* to work. When you plop down a whole heap of ICs with unverified models the results are hit and miss.
Fair enough, Just starting to understand the bullcrap regarding electronics.
There's a lot of it. Some things are just technically difficult you might to know a whole book to answer one seemingly simple question. However, things like datasheets can be difficult to interpret or don't have the full enough info. It's often difficult to translate datasheet to spice models. There are programs to do this but they aren't free. There's a few sites on the web about converting datasheets to spice models
Nice… So it’s all about the slope then! And in the datasheet is it supposed to show the slope related to the maximum and minimum values of voltage? The slope that appears there should be related to the subtraction of the max/min I would suppose.
Slope is about how well the Zener regulate, which is kind of it's job. The slope changes at different currents. There's other issues like one manufacturer will rate their 4.7V zener at 5mA and another might rate theirs at 20mA or 43mA. As far as the datasheet goes they are incomplete from a spice model perspective, or even a from a user perspective for that matter eg. little low current info. For design we might care about worst case but for spice we might want to know typical. The datasheet have a few spare points maybe Vz + Iz or Zz (slope) vs Iz. Typical values aren't always given. The manufacturer tests against the values in the datasheet, so they will use min and max. that's all they are willing to guarantee you. If you measured 10 zeners with the same part number and the same batch you might end-up with a different view of the world, but at least one which will match the circuit you build.
A lot of parts are not precisely defined. Look at transistors (BJTs). The gain(hFE) in the datasheet is all over the map. If you measured 10 real parts the hFE values will be tighter. Next batch you might measure something else. It's a moving target from a spice point of view. At best you could come up with three models for the same part: low gain, typical gain, high gain. You might do your basic checks against typical but then you need to make sure the circuit at least works with high and low gain cases.
The fine details of electronics is a headache. You can go a long way with ignorance is bliss philosophy but one day it will catch up with you. There's plenty of debugging threads on this forum with some very obscure problems, often they are very difficult to debug via forum posts.
