User's Guide - Level 1
Here's a quick tour of Op Amp Builder - Level 1, a web page where you create custom SPICE subcircuits that models Gain, Bandwidth and Input/Output Resistance.
Create a custom SPICE subcircuit that models Gain, Bandwidth and Input/Output Resistance. Use early in the design cycle with a high bandwidth to develop the overall topology. This macromodel simulates quickly and doesn't have convergence problems, unlike some manufacturer's models. Later in the design, replace it with a more complex model to address which secondary behaviors might impact your design.
SPICE CIRCUIT
NETLIST
* Device Pins In+ In- Vout
.SUBCKT OPAMP1 1 2 82
*
RIN 1 2 1e9
*
* AMPLIFIER STAGE: GAIN, POLE
* Aol=1e6, fu=10e6 Hz, fp1=10.000 Hz
G1 0 10 VALUE = { 1.0000 * V(1,2) }
R1 10 0 1e6
C1 10 0 1.5915e-8
*
* OUTPUT STAGE
EOUT 80 0 10 0 1
ROUT 80 82 100
.ENDS
QUICK OVERVIEW
| Function / Parameter | Description | |
| Input Resistance | RIN - Resistance between input terminals. | |
| Differential Amplifier | G1 and R1 create a differntial amplifier with input nodes 1 and 2 and output node 10. Learn More. | |
| Open Loop Gain | Open Loop gain defined by KG1*R1. Learn More. | |
| 1st Pole Low-Pass Filter | R1 and C1 create a low-pass filter and the bandwidth of the op amp mdeol. Learn More. | |
| Output Buffer and Resistance | EOUT provides output current drive and ROUT mimics the output resistance of the op amp. Learn More. |
EX 1 - OP AMP MODEL IN A NETLIST
Inserting a model into your netlist is a piece of cake. Just give the opamp a name starting with an "X" giving SPICE a heads up for a subcircuit else where in the file.
R1 1 2 5K
R2 2 3 10K
XOP1 0 2 3 OPAMP1
Then copy your op amp macro-model (SPICE subcircuit shown above) into your file. Be sure to include the whole enchilada from .SUBCKT to .ENDS. Note, that circuit nodes 0 2 3 will be connected to subcircuit nodes 1 2 82. For a quick review of subcircuits, check out Why Use Subcircuits?
As an option, copy the subcirecuit into a separate file named "opamp1.lib" for example, and add the statement
.INC opamp1.lib
to tell SPICE where to go fish for the op amp model.
EX 2 - OP AMP MODEL IN AN LTSPICE SCHEMATIC
Inserting a model into your netlist is a piece of cake. Just give the opamp a name starting with an "X" giving SPICE a heads up for a subcircuit else where in the file.
Then copy your op amp macro-model (SPICE subcircuit shown above) into your file. Be sure to include the whole enchilada from .SUBCKT to .ENDS. Note, that circuit nodes 0 2 3 will be connected to subcircuit nodes 1 2 82.
As an option, copy the subcirecuit into a separate file named "opamp1.lib" for example, and add the statement
to tell SPICE where to go fish for the op amp model.