A Perfect Match – How to Determine if a Model is Compatible with an Existing Symbol: Part 2 of 3

How do you confirm that an existing symbol is a good fit for an imported model?  What factors should be considered to ensure you are providing compatible voltage supplies and signals to the pins of your op amp model?  As was the case with the previous post, the techniques in this blog post can be applied to other model types as well. In this blog post, I’ll cover some of the considerations that were glossed over in "The Simple Method to Import an Op Amp in LTSpice".

Picking up where we left off in the last post: let’s start with a working schematic, with an imported AD8656 op amp model - download the working schematic here.

Figure 1: Starting with a Simple Working Example

Inspect the Pinout of the Op Amp Symbol

Right-click on the op amp symbol to open the Component Attribute Editor.  Click Open Symbol. 

Figure 2: Opening a Symbol File from the Component Attribute Editor

With the symbol file (opamp2.asy) open, select View -> Pin Table.  The table displayed shows the ordering of the pin names with respect to the SPICE netlist order. 

Figure 3: Viewing the Symbol Pin Table

Make note of the pin list order in the table below

Table 1: Symbol Pin Table Including Pin Function

Inspect the Pinout of the Model

Let's examine the first non-commented line in the model: .SUBCKT indicates the model type, AD8656 is the model name, and the remainder of the line is a listing of the device pins (1 2 99 50 45).  The comments above this line give us details about the functionality of each pin.  The ordering of these pins matters, so it’s crucial to ensure the ordering of the pins in the model is compatible with what the opamp2 symbol expects.

Figure 4: Op Amp Model with Pin Orders and Descriptions

Combining the table created when examining the opamp2 symbol pin list with what we now know about the AD8656 model pin list can be seen in the table below.

Table 2: Adding Model Pin Numbers to Pin Table

Referring to the node assignments comments in the model header, we can confirm that the ordering of the pins in this model aligns with the ordering expected by the opamp2 symbol.  Pin 1 corresponds to In+, 2 to In-, 99 to V+, etc.

If you have a model that doesn't conform to the expected pinout, there is more work you’ll need to do.  I’ll discuss strategies for modifying symbols and creating new symbols in the next blog post.

Double-Check your Supplies and Input Signal

Take a few moments and study the op amp datasheet.  What is the allowable supply range?  What is the headroom of the input and output pins?  What is the bandwidth?  If needed, make modifications to the supply voltages and input signal to ensure they are compatible with the device you are simulating.

To simplify, make only a few changes to get to a point where you can simulate again.  Ensure the supplies remain balanced and the op amp’s common-mode voltage is maintained at 0 V. This may not match the configuration you ultimately want to simulate, but start with a simple configuration to verify that the model works as expected.

For my example using the AD8656, I adjusted 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: Modifying Voltage Supplies to Adhere to Operating Requirements of AD8656

What’s Next?

This blog post provides guidance on how to verify that the pin list for an LTspice symbol and a .SUBCKT header are compatible with each other.  Stay tuned for the next post, where I will discuss options and strategies for modifying or creating new symbols when necessary.

Read all the blogs in A Pinch of LTspice series.