The core SPICE engine is NOT case-sensitive; it comes from an era when you might only have uppercase on your terminal. Therefore "m' or "M" is milli, and SPICE breaks SI convention by requiring "meg" (any letter-case) for million.
You may have a front-end which "fixes" this; but it is probably good practice to spell-out MEG so you aren't tracing silly GIGO errors.
>
knows how to handle resistors, capacitors, diodes -n- such. The various opamps or tubes are not default componentsSPICE was written, well really to get a degree, but nominally to model huge MOSFET logic arrays for the then-new LSI chips. While the final result of logic is yes/no, when you run fast there's a lot of rounding and SPICE can compute waveforms very well so you know if a gate is getting behind the action. It has insane levels of MOSFET models built-in. They need voltage supplies. It has resistors and caps and coils because these are basic blocks. It has JFETs and BJTs. It has a lot of abstract functions because they are easy (a VCVS voltage controlled voltage source is an ideal transformer with infinite response but without in/out conductivity; it's pretty much just 4 pins and an equals sign).
>
opamps or tubes are not default componentsThere may be generic OPAMP and GAIN building blocks; pSPICE has them. Its OPAMP is subtle: it has hidden power supplies, and if it clips it is liable to blow-up the math and quit.
If a perfect (tho buggy) OPAMP is not enough, then you want something which wasn't mature when SPICE was born; that's why it has sub-circuits. You can download models of most chip opamps or near-kin, Do NOT trust them too far: a full simulation of a chip opamp is too complicated and thus too slow to be useful. Most model input current, gain rolloff, and rough clipping. Almost none model power pin currents correctly (load current tends to flow in/out a phantom ground which has no physical reality).
SPICE _must_ be told where "ground" is because it references all computations to a "zero" voltage. In the real world electrons don't need ground (there's no ground on a flashlight) but without a common reference the computations would be too messy.
pSPICE has r_pot. I'm shocked that LTSPICE doesn't, but this is so. It seems to be a developer bias. There is a user-written library with pots.
http://www.diystompboxes.com/smfforum/index.php?topic=24240.0http://gaussmarkov.net/wordpress/tools/software/ltspice/ltspice-analysis-and-the-dod-overdrive-250/http://groups.yahoo.com/group/LTspice/http://gaussmarkov.net/ltspice/DOD250-LTSpice.zipThere should be a "flip" command so that your L1 L2 could be placed with the curleys pretty, the dot at the top, and without the swastika connection.
LTspice labels the graph with node-numbers?? pSPICE finds the nearest part. And any wire, you can double-click, give it a name, and it may use that name for graphs.
R7 R8 R11 may be reduced to two resistors; make R7 R8 much larger and short R11. That's not exactly the same because supply current is lower; don't care here.
R12 is not needed in simulation. It does not affect audio response. The tube and wiring parasitics are not detailed enough to cause VHF troubles. I also think that 6SL7 in a clean layout does not need R12 in real life, but of course sometimes a hot tube works against parasitic L and C and needs a dash of R to stay stable. If you are using it as a schematic artwork tool, fine. R12 forces extra (pointless) computation but that won't lengthen the sim-run long enough to measure. (I remember, on 286 machines, when adding one resistor would slow the run.)
Topic: LT Spice (Read 12010 times)