another LT Spice question

First save the file wherever you want, but change the suffix such that it's...

AD8033.lib

Then follow Fred Abse' cute trick...

"Open the subckt file in LTspice.

Right click on the "subckt" line.

A symbol is automatically generated, and the symbol editor opens. You can then edit the symbol as much as you like.

Saving the symbol creates a new symbol category, "Auto Generated", if it doesn't already exist.

No need for an .include, or .lib statement. The file name is automatically inserted into the symbol "model file" attribute."

The symbol will just be a block... who cares. But you can fancy it up by redrawing the outline to suit your own tastes.

There's probably also a way to import existing graphics, but I don't know that gimmick yet. ...Jim Thompson

This is perfect! I need those very instructions to use Duncan's model

in tonight's home school class in UJT modeling. ;)

Never knew about that feature.

I always placed some similar symbol part on the schematic, then changed its reference to include the text from vendor, then put the whole thing back into Linear's Library - for future retrievals. Only to discover once that the 'update' removes things without telling you, so...had to put in another location, but still easy to find.

Also, just noticed I have July, 2013 ver 4.19i and it contains a myriad of LT1028 OpAmps, including LT1028N with the extra pin connection.

Could you post those models and associated asy's, or E-mail to me? I want to see what the model looked like before the recent revision. ...Jim Thompson

No need to change the file extension, .cir works just as well.

Certainly, with LTspice. I tend to be a stickler and follow Spice standard conventions, avoiding lots of confusion...

.CIR, circuit file, ready for simulation .NET, netlist file, components, but no simulation information .OUT, output file, bias points, etc.; sometimes numerical "listing" of output data in Berkeley Spice format (PSpice, HSpice, SmartSpice do this, LTspice does not :-( .DAT, output data for viewing in a post-processor .RAW, LTspice of conventional Spice .DAT .LIB, the most usual way of conveying models .MOD, .SUB, unconventional, but also used for models .INC, (.INCLUDE), the garbage way to pass libraries, takes much space since all devices listed in library are loaded. .LIB, loads only the devices in your schematic

PSpice has other extensions, as well, for passing messages and error notifications. ...Jim Thompson

"rawfiles" originated in Berkeley Spice.

" The standard suffix for rawspice files in VMS is ".raw"" (Spice 3f man page)

Probably why I never saw them. When I last used Berkeley Spice (~1980) I used the .OUT file to drive a tractor printer, outputting a numerical list of voltage versus time and *'s marking a rough waveform ;-) ...Jim Thompson

I can still do ASCII plots (Berkeley 3F). Not that I ever do.

LTspice should have a .PRINT statement like PSpice.

Undocumented now, but it's still there... I just made a symbol for it, somewhat like a probe symbol, but with a printer on top.

I stick it on a node where I want a numeric listing, and the listing appears in the .OUT file, ala Berkeley.

I use such listings to do post-processing in Excel, or create PWL sources, or in IBIS modeling.

The output data points are equal-spaced ("Print Step" in the .TRAN settings). In LTspice (there is no .OUT file), I understand that you can get an unevenly-spaced list, requiring using an executable by Helmut Sennewald to extrapolate to evenly spaced.

I have an executable (Aaron wrote it for me) that takes this evenly spaced data and optimizes it for least amount of points needed for PWL or IBIS models (IBIS has a 100 point limitation on most descriptors, a real PITA, so you have to be creative :-) ...Jim Thompson

Jim, I used .out files to look at effective transistor widths and lengths as well as the operating points. I miss this in LTSPICE. Is there a way to get these. Also, how could I get the probe with a printer t that you came up with?

My grammar was poor. There's an undocumented .PRINT in _PSpice_, that simply requires making a symbol (*) that spits out a .PRINT statement. AFAIK there is no such equivalent in LTspice, though one might try using the LTspice vernacular "Spice directive", .PRINT...

(*) An alternate way is discussed in... Subject: Interesting Spice Netlisting Quirk Date: Fri, 04 Apr 2014 10:59:42 -0700 Message-ID:

(And, by "Symbol", meaning as used in PSpice, with a netlisting template, etc.)

I just remembered, I have a Berkeley Spice3F3 manual which might offer some hints on finding hidden features in LTspice. I'll post a link tomorrow.

As for a .OUT file equivalent, I haven't found any such creature. ...Jim Thompson

Spice3F3, now on the "Tools & Macros" page of my website. ...Jim Thompson

What I will say, is that in SuperSpice, there is docked signal list tab that you can click on to display, for example, Vds and Vdsat together so that you can check immediately, over process corners, whether the device is operating in the correct region over DC or transient sweeps.

all main parameters such as gm,gds, vt, vgst are available

Kevin Aylward B.Sc.

I forgot to mention, there is also "LTspiceTutorials.zip" on the Simulation Tools & Macros page of my website. Lots of information there. ...Jim Thompson