How can i check what pin is configured to what netlist order from the SPICE model?

Question

I am trying to make a model for an op-amp (AD8000) in LT SPICE. So far here is what i did:

First I downloaded the model from https://www.analog.com/en/products/ad8000.html and opened it from my downloads:

Which then gave me this page with text. I right clicked AD8000

and clicked create symbol

then I went to documents>LTSPICEXVII>lib>sym>Autogenerated>AD8000 I right clicked on AD8000 and then hit open with NOTEPAD

I went to documents>LTSPICEXVII>lib>sym>OpAmps then right clicked on LTC6253-7 and clicked open with NOTEPAD like i did with AD8000

Then I highlighted everything from the line that says "version 4" to the line above "windows", copied

and pasted it to everything on the AD8000 file above "windows"

then highlighted everything from the following section of the LTC6253-7 NOTEPAD file:

And pasted it into the following AD8000 file below the last line that says SYMATTR

then i closed both of the notepad files and opened up a new LTSPICE window and, on the menu bar of LTSPICE at the top, I clicked file>open then selected documents>LTSPICEXVII>lib>sym>Autogenerated>AD8000

which gave me the aesthetically pleasing Op-Amp-esque symbol for my AD8000 that was derived from LTSPICE's built in LTC6253-7 meaning that it came with a shutdown pin.

I went ahead and removed the "!S" logo.

Now the important question i have: How do I know if the inverting pin on that symbol really corresponds to the inverting pin, if the non-inverting pin corresponds to the non-inverting pin, etc. from the following:

edit: I opened the symbol for LTC6253-7 and right clicked each pin. The pin assignments were copied and pasted to the AD8000. The picture above of the model file for AD8000 lists the order as noninverting (1), inverting(2), positive supply(3), negative supply(4), output(5), and powerdown(6). However, when i right clicked each pin from LTC6253-7 and the newly created symbol for AD8000, the pin assignments are: output(1), negative supply(2), inverting(3), non-inverting(4), shutdown(5), and positive supply(6). Should I switch the pin order of the AD8000 symbol so it matches its model file?

edit 2: This edit is for anyone other than myself who encounters this problem in the future. I followed @periblepsis suggested technique and I got the same results they did. Initially I ran into the problem "could not open Ad8000.lib". To fix this problem, I went to Tools>control panel> sym. & lib. search paths. Under library search path I copy and pasted the directory containing the AD8000 model I downloaded "...LTspiceXVII\lib" (I of course did this after moving the AD8000.lib file from the download folder to ...LTspiceXVII\lib) and it fixed the problem. Prior to doing this, the search paths for symbol and library were both empty. This may explain why LTSPICE could not fine my model file.

Answer 1

I've never used the auto-generate capability. Not once. And now that I see how you used it and what you got out of it, I probably never will use it.

This is how I've been creating symbols using the regular editing features in LTspice:

1. Create a new schematic sheet in LTspice. Hit F2 key to pop up the Select Component Symbol dialog box. Double-click the [OpAmps] folder. Start using the down-arrow key looking for the symbol shape I wanted. Here, I find that the ADA4097-1 device looks promising:

2. Escape out and close down the sheet I just opened. Now, select File/Open or ctrl-O and select the installation folder for LTspice and pick out the ...\lib\sym\OpAmps subdirectory there, looking for a file called ADA4097-1.asy and open it up.

3. Right-click on the text, ADA4097-1, to pop up the Symbol Attribute dialog, double-check that it says it is the <Value> attribute (which it is), cancel out of the dialog, and then delete it entirely.

4. Right-click on the text, S, to pop up the Edit Text on the Symbol dialog and change it to say PD, adjust the size if I want, and then hit OK. Then move it around, if desired.

5. Select the menu option Edit\Attributes\Edit Attributes to load up the Symbol Attribute Editor and change the SpiceModel to the text AD8000 (no extension, as this is the SUBCKT name, and no longer a file name), clear out both Value and Value2, modify the Description as wanted, and put the test AD8000.LIB (which is the name I would give to the file holding the downloaded model) into the ModelFile field.

6. Right-click on each of the pin ports, one by one, to verify that they match up with the downloaded model. Which in this case they luckily do. So nothing needs to be changed. That's good!

7. Select the menu option Edit\Attributes\Attribute Window to load up the Attribute Window to Add dialog, select SpiceModel and hit OK. Place the AD8000 text somewhere handy:

8. Select the File\Save As option and save it as AD8000.asy.

9. Close the symbol sheet.

10. Take the downloaded model file and save it into ...\lib\ as AD8000.LIB.

That's all. Now fake up a new schematic and test things out:

Well, it didn't explode. So maybe I got it added in okay. I'm not familiar with the datasheet, so I didn't try to do anything special here. Just a quick test.

This isn't the only way, of course. But it's how I go. The method here also allows me to add additional models into the same .LIB file, if all of them can use the same symbol drawing. For example, by using this approach for the following PUJT symbol, I'm able to have these two different spice models in the same .LIB file and LTspice will automatically scan the entire file, find all of the model names in it, and show them to me in a drop-down box:

Convenient, at times.