https://groups.io/g/LTspice/topic/how_to_add_an_op_amp_to/78979046



Gerry asked, "Could someone kindly point me to the specific instruction/tutorial for adding an op-amp to LTspice ?"

Open LTspice.  Click Help > Help Topics.  Start at the beginning, and read.  All of it.

When you do that, pay attention to the page F.A.Q. > Third-party Models.

Your question has already been asked (and answered) here more times than I care to count.  There are no "specific" instructions because there is no single way to do it.  There are many.  Not to mention, it greatly depends on how you plan to add this model.  Are you writing the model yourself?  Did you download it?  From where?  What does the model look like?  There is no simple answer.

If the model is encrypted (for PSpice or HSPICE), stop here because you can't add it to LTspice.

If it is an actual SPICE model, chances are excellent that it needs no importing, and it works in LTspice with no changes.  But there are some SPICE models, from some IC vendors, which work poorly or not at all and may need some tweaking to get them to work better.  SPICE models are readable text, so if the file isn't like that, then you're looking at the wrong file.  For example, PSpice models come with a handful of files but LTspice needs only one of them (often with a .LIB filename extension).

Check our group's Files to see if someone here has already done this.  You can save yourself work by using what someone else already did.

The shortest (not necessarily easiest) way to use a third-party model in LTspice, is to either copy-and-paste it into your schematic, or add a .INCLUDE or .LIB statement to import the model file.  Then add a subcircuit call to your schematic with a SPICE Directive that may look something like this:

Xamp In1 In2 VDD VSS Out FunnyOpAmp

But you probably wanted a schematic symbol.  Generally speaking, there are two common ways to do that.

The method I DO NOT prefer is this:  Let LTspice auto-generate the symbol.  Follow the steps in the Help page Schematic Capture > Creating New Symbols > Automatic Symbol Creation.  You'll get a dumb-looking box for a symbol that doesn't look anything like an op-amp symbol.  Now open the symbol that you just created in LTspice's symbol editor, press Ctrl-A, go to the ModelFile attribute, and edit it to completely remove the path, leaving just the filename.ext.  Save the symbol.

This method is better, for MOST op-amps:  Add the "opamp2" symbol to your schematic.  Right-click on the text "opamp2" and change it to the name of the op-amp subcircuit you're using.  It is not the name of the file; it's the name that appears inside the model file after ".SUBCKT", which is probably closer to the top of the file.  Skip past all the lines that start with "*".  For example, if you see this:

.SUBCKT 737MAX      1 2 99 50 30

then the name is "737MAX".  (The name contains no spaces).

Then add a .INCLUDE or .LIB statement to the name of the model file.  Also keep that file in the same directory with your schematic that uses it.

After you run into problems -- then come back here and ask for more help.

Andy


=============================

Hi Gerry

I would just use the built in Universal OP Amp 2, and
tweak the specs to match the real part
Right click on the symbol
Way simpler

Al D.