The personal website of Scott W Harden

Using MOD Files in LTSpice

This page shows how to use the LM741 op-amp model file in LTSpice. This is surprisingly un-intuitive, but is a good thing to know how to do. Model files can often be downloaded by vendor sites, but LTSpice only comes pre-loaded with models of common LT components.

Step 1: Download a Model (.mod) File

I found LM741.MOD available on the TI's LM741 product page.

Save it wherever you want, but you will need to know the full path to this file later.

Step 2: Determine the Name

Open the model file in a text editor and look for the line starting with .SUBCKT. The top of LM741.MOD looks like this:

* connections:      non-inverting input
*                   |   inverting input
*                   |   |   positive power supply
*                   |   |   |   negative power supply
*                   |   |   |   |   output
*                   |   |   |   |   |
*                   |   |   |   |   |
.SUBCKT LM741/NS    1   2  99  50  28

The last line tells us the name of this model's sub-circuit is LM741/NS

Step 3: Include the Model File

Click the ".op" button on the toolbar, then add .include followed by the full path to the model file. After clicking OK place the text somewhere on your LTSpice circuit diagram.

Step 4: Insert a General Purpose Part

We know the part we are including is a 5-pin op-amp, so we can start by placing a generic component. Notice the description says you must give the value a name and include this file. We will do this in the next step.

Step 5: Configure the Component to use the Model

Right-click the op-amp and update its Value to match the name of the subcircuit we read from the model file earlier.

Step 6: Simulate Your Circuit

Your new component will run using the properties of the model you downloaded.

Newer: ECG Simulator Circuit
Older: Exponential Fit with Python
All Blog Posts