LTspice is fantastically great (IMO). Congratulations.
Here is a sort of "master list" of spice models on the web:
**broken link removed**
Using most P-Spice-type models with LTSpice is easy. They're usually subcircuit-type models. For an opamp model, there's already a handy existing symbol you can use, "opamp2" in the Opamps library. Plop it onto your schematic, right-click on it, click in the "Value" column in the "Prefix" row and then enter X in the "edit box", above the table (X tells the program it's a sub-circuit model). Then click in the "Value" column of the "Value" row, and enter the subcircuit name (e.g. LF358), as it appears in your model file. Then, on your schematic, place a spice directive (with the .op button) like .include yourmodelfilename.sub, where sub is whatever the filename extension is (Often, it's sub, but needn't be.).
The LT-SPICE Yahoogroups group is truly excellent. The people there are amazing. Be sure to download the library file that lists all of the library files, and the one that lists all of the message topics. Then you can search through them with Wordpad, or whatever, which is often more productive than doing it only on line, although it WOULD be nice to have the full text of all of the messages, as well, since yahoogroups' m-searching is so clunky.
-----------------
A few things that might be good to learn sooner rather than later, just off the top of my head, and in no particular order:
You can right-click on a plot and select "Add Plot Pane", to have more than one simultaneous plot. It's handy for plots with way-different scales, et al. You can click anywhere in a plot pane and then the next thing you click on in the schematic will be plotted in that pane. You can also just drag a plotted quantity's label from wherever it is to anyplace in a plot pane you want to move it to.
You can drag a rectangle around any part of a plot, to make it fill the plot pane, i.e. magnify portions of a plot, repeatedly if desired. You can also drag rectangles to measure things. The deltas are displayed in the bar at the bottom.
You can Alt-Leftclick on any device, to plot its total power dissipation!
You can right-click on any plot label and enter ANY ALGEBRAIC EXPRESSION to be plotted! And if you enter a voltage divided by a current, the plot units will be shown as Ohms, for example.
After a run is stopped, you can Ctrl-Leftclick on any plot label and it will INTEGRATE that plot, for you, giving RMS, AVG, and/or Integral values, as appropriate. Note that it will integrate only the currently-visible window. So if you only want to integrate over part of a plot, you can drag a rectangle around the part you want, so it fills the window. (FFTs can work that way, too, but give you a choice of either way.)
Always un-check the three compression options, in the Control Panel, or, better yet, include .options plotwinsize=0 on all of your schematics, to turn off compression.
(Almost) Always specify a min timestep, for transient runs.
You can use .WAV files, as both inputs and outputs!!! The possibilities are staggering...!
Learn to make your own subcircuits, so you can have hierachical schematics. It's great, especially for larger projects. You can eventually have what amounts to a block diagram, with just your interconnected subcircuit symbols, and can then "drill down" to wherever you want, in the hierarchy. It's easy. If you have a schematic that will be part of a larger schematic, and you have labeled the inputs and outputs, just create a symbol for it, with the same name as the schematic, and put whatever inputs and outputs you want, in the symbol. Then it can be added to any other schematic, using the regular "add component" button, by using the "Top Directory" box at the top of the "add component" dialog to get to the "personal" library of subcircuits in the current folder. And whenever you're in a schematic that has a subcircuit symbol, you can right-click on the symbol and select Open Schematic, if you want. Also, if you go into the control panel and select all of the Save... voltage and currents, you'll be able to plot from such schematics just like from the top-level one.
The MEASURE commands are too cool, and very powerful. There are examples in the Files section of the LT-SPICE group.
The .STEP commands are powerful. You can set a component's value (by right-clicking on it) to, say, {C}, and then use a .STEP command such as .STEP {C} list 2.2p 3.3p 4.7p 10p to run a simulation for each value of C in the list, or something like .STEP {C} 10p 1010p 100p, to run sims with C from 10p to 1010p in 100p steps. The plots will be plotted together, with different colors. Right clicking on the plot pane and selecting Select Steps will show you which color is for which stepped value. You can also nest the step commands, at least two levels deep.
To get all of the node voltages, etc, like you mentioned, I think you just do a .DC op pnt analysis, and a window pops open with all of the voltages etc, which you can copy to the clipboard with Ctrl-C, if you want. Then, whenever you pass the cursor over a node, the DC operating point is displayed in the bar at the bottom of the screen.
Oh, make sure that you set up your Keyboard Shortcuts, in the Control Panel!!
I guess there's so much more that I might as well just quit, for now. And I'm sure that I haven't thought of some of the really good ones, here. I'll post again, if I run across them.
Have fun!
- Tom Gootee
**broken link removed**
-