Guys, I know most of you are experienced users of spice here :) Two short questions, I've already RTM without find the answers.
- I need a TIP 122 model... where I should look for?
- worst-case scenario: I set the tolerances of my resistors. How to run a simulation to get the worst-case? I'm talking about the maximum span of selected traces when components reach their end values.
Are you certain you want ALL the worst case values at the SAME time? The statistical likelihood of that is supposed to be extremely small.
We only used the 'worst case box' for milspec designs, where if the circuit didn't perform to spec, you had to point tothe component that was out of spec, else...
More likely scenario was for cmmecial designs where we used a Guassian distribution for the component tolerances, like 'square root of the sum of the squares' tolerances which was quite a bit more lenient to design. But even in Production that wasn't realistic - sometimes. We found the resistor manufacturers made runs of resistors measured what thy made, which created a flat distribution, but then they culled out special values which put 'holes' in that distribution! Usually we got distributions with the centers cut out. In other words likely to get + values and like to get - values, and rarely got exactly what the label said.
Then there are the 'just get by' values. Where you have them in stock, they're almost the right value, but not quite, but it's 12 weeks to get the right ones, so you NEED to use these.
Once when designing an IC, after being told to expect beta of 3:1 and not trusting; I designed the circuit to take a beta range of 5:1 Brother! did THAT pay off!
Once when designing CCD cameras, and being told to expect a 'sensitivity' of such and such and again not trusting; I designed to accept 50% of the minimum sensitivity. Boy, did THAT pay off. Especially when you get a lot in that doesn't meet spec, and there are NO others and you're supposed to be shipping 2,000 units/mo and you have a room full of workers who will have NOTHING to do if you reject that lot.
So question goes back to the OP...why do you need to design to milspec style? Unless your customer is milspec, you have overdesigned for instrumentation volumes and probably underdesigned for consumer volumes [10,000,000 per year]
Not sure in LTSpice, but in PSpice the worst case sim does this. First, it does a base run, and gets your 'output' value. Then, it goes to each toleranced part, changes the value a small bit, and runs a new sim. It notes whether that output value changes plus, or minus. After testing the sensitivity on all the parts, it takes each part, adjusts its value in the direction indicated by the sensitivity to its limit, and runs a final, worst case simulation.
Note that this is not necessarily the absolute worst case. In some circuits, especially filters, the actual worst case may be a some point within the tolerances where resonance effects are worse. Also, if you were not careful in setting your distribution types and values, you can get wild values for the sim, especially if you have gaussian distibution parts (PSpice sets the tolerance as the one sigma point, so worst case is three sigmas...)
Usual practice is to do the worst case high, worst case low, and then some Monte Carlo runs. Display them all in the same probe window, and you can see what the distribution of results tends to be.
No milspec at all. For example, if you followed the thread about the current limiter, I want know how much will change the limited current in function of the tolerance of the resistor. It's a protection, so I do need to know if it will safe with any value I may expect.
It's just an example, but I hope you understand what I'm saying.
Yes, being conservative is good. I used the term 'milspec' merely as a descriptor to make it easy to refer to using the worst case box of tolerance values. Don't forget to add the tolerances of all the measuring intrumentation, too.
.asy files are *symbols*, ie. the shape that shows on a schematic.
Put TIP122.sp2 in /lib/sub, and add the LTspice directive ".lib TIP122.sp2" to your LTspice schematic.
Use the standard NPN symbol, but don't assign a device model. Instead, control-right-click on it, which will open a dialog box where you can make it into an "X" subcircuit device, and set the appropriate parameters.
A good read of the manual will make things clear.
If you use a lot of subcircuit devices, it's a good idea to make a dedicated "subcircuit npn" symbol.
"For a successful technology, reality must take precedence
over public relations, for nature cannot be fooled."