What are best practices for importing models into LTspice? The answer can depend on several factors. What kind of model is it? Is the model compatible with a symbol already included in LTspice? Does a new symbol need to be created? The decision tree for importing a model can be overwhelming.
Very often, the model being imported is an op amp model. Did you know the LTspice component library includes over 700 op amp models, ready to use without needing to be imported? Each model in the LTspice library has an associated example circuit. Using an op amp already available in LTspice is certainly simpler than importing a model.
What if you need to examine the behavior of an op amp not included in the LTspice device library? In this blog post, I will demonstrate The Quintessential Method for importing an op amp model. The resulting schematic will require no custom symbols and no additional files to import.
Start with a Working Schematic
I will start with a schematic that I already know works—for two reasons. First, I am lazy efficient. Second, I am prone to errors when drafting a schematic from scratch; starting with something that already works saves time.
To follow along, open the AD795 example circuit by selecting File → Open Examples from the top menu. Navigate into the Applications folder, and open AD795.asc.
I will simplify the AD795 example circuit by removing the resistors in the feedback path and reconfiguring the feedback path to be a buffer/follower configuration. If you need some pointers on making changes in a schematic, see the Schematic Capture section in the LTspice Help Manual (Help → LTspice Help).
Run the simulation by clicking the green play button in the toolbar. Ensure that this basic simulation is working as expected before continuing.
Figure 1: Starting with a Simple Working Example
This is always a great place to start—we have sensible supply voltages, no typos in our node names, no errors in our simulations. Work in incremental steps, starting with something that simulates as expected.
Add an opamp2 Symbol
Delete the existing op amp symbol and replace it with the opamp2 symbol. To do this, select Edit → Component from the menu. Navigate into the OpAmps directory and select opamp2. Scroll all the way to the right to find it. Place the opamp2 symbol where the previous op amp was; it should be a perfect fit.
Figure 2: Adding opamp2 Symbol to Schematic
Looks good, but not quite ready to simulate yet.
Ensure the Model Is a Good Fit
For this example, I will use a model for the AD8656, which is available for download here. I am also going to hand-wave a bit and tell you: the AD8656 is a good fit for the opamp2 symbol. The AD8656 model has five pins, and they are in the correct order for the opamp2 symbol.
Include the Model Contents
With the model file opened in a text editor, select all the text in the file and copy to clipboard (usually right-click → Copy, or CTRL-C in a text editor).
Click on your schematic to make it active. Zoom out (Shift+Z) to expose some blank space on the schematic. Add a SPICE directive by selecting from the menu Edit → SPICE Directive (or pressing .). The Edit Text on the Schematic dialog will appear; paste the clipboard contents into the text entry box. Click OK and click on the schematic to place the model contents.
Figure 3: Pasting Model Text into Schematic as a SPICE Directive
To reduce the space the text block takes on your schematic, right-click on the text block and decrease the font size in the drop-down.
Link the opamp2 Symbol
Make note of the model name in the.SUBCKT line of the model text (for my example, the model name is AD8656). This is the value needed to properly link the symbol to the model.
Right-click on the opamp2 symbol. Change the value from "opamp2" to the name of your model (AD8656 for this example). Then click OK.
Figure 4: Linking opamp2 Symbol to AD8656 Model
Adjust your Supplies and Input Signal
Using the AD8656, I need to adjust the supply voltages to ensure I am within the required 2.7 V to 5.5 V supply range specified in the datasheet.
Figure 5: Setting Compatible Supplies, and Illustrating Linkage Between Symbol and Model
Simulate!
Simulate your circuit again. Do you get something that appears to behave like a buffer/follower?
Figure 6: Successful Simulation
If so, congratulations! Continue making incremental changes and frequently simulate until your schematic accurately represents the desired topology and configuration.
What's Next?
This blog post offers a straightforward and simple method for incorporating an op amp model into your LTspice schematic. Stay tuned for the next post, where I will go into more detail on how to ensure if an op amp model is a good match for the opamp2 symbol and what to do if you need to modify the symbol or create a new one. I’ll also discuss how to ensure your power supplies and input signals are within the allowable range of the op amp model.
Read all the blogs in A Pinch of LTspice series.