原创 Spice Error "Too many parameters for subcircuit

 2010-3-10 20:02  3067 2 2 分类: 模拟

Spiceorder has nothing to do with pin names or numbers. It has everything to do with the order of the pins in the .subckt line of your model file:

Code:

.SUBCKT  lmv324     3  2  4  5  6

If a device has N pins that are used for I/O and power, then the Spiceorder must start with 1 and end with N. The LMV324 has 5 pins, so the Spiceorder goes from 1 to 5.
The subcircuit in the model file is a netlist of the circuit that represents the device. Each pin and internal node is assigned an arbitrary number or name. In this case, the engineer decided on the following node numbers for the I/O and power pins:

Code:

* Connections       non-inverting input
*                   |  inverting input
*                   |  |  positive power supply 
*                   |  |  |  negative power supply 
*                   |  |  |  |  output 
*                   |  |  |  |  |
.SUBCKT  lmv324     3  2  4  5  6

They are placed in this order because the package pins are defined in the .asy file (which "draws" the symbol) as below:

Code:

PINATTR PinName In-
PINATTR SpiceOrder 2
PIN -32 80 NONE 0
PINATTR PinName In+
PINATTR SpiceOrder 1
PIN 0 32 NONE 0
PINATTR PinName V+
PINATTR SpiceOrder 3
PIN 0 96 NONE 0
PINATTR PinName V-
PINATTR SpiceOrder 4
PIN 32 64 NONE 0
PINATTR PinName OUT
PINATTR SpiceOrder 5

Note that the Spiceorder can be in any order

, just so long as 1-5 are all present.

Remember, the subckt nodes, which were numbered 2, 3, 4, 5, 6, could have been called joe, bob, bill, ron, and wookie. So long as these were listed in the correct order in the .subckt line, the model and .asy file would still work together.

I guess that was about as clear as mud.