Modeling and Simulation occur error

Question

I have established a model about APEX PA78, but the simulation reports some error, please help me!
Spreadsheet view report is followed:
------ Checking SPICE netlist for PA78 - 2010-01-28 20:12:00 ------
SPICE Netlist Error in schematic RefDes 'u2', element 'xu2':  Unexpected '15' found on subckt instance line - too many nodes or parameter value missing name. 
SPICE Netlist Error in schematic RefDes 'u2', element '<unknown>':  Due to errors, the subckt instance 'xu2' has been omitted from the simulation
SPICE Netlist Error in schematic RefDes 'u1', element 'xu1':  Unexpected '1' found on subckt instance line - too many nodes or parameter value missing name. 
SPICE Netlist Error in schematic RefDes 'u1', element '<unknown>':  Due to errors, the subckt instance 'xu1' has been omitted from the simulation
======= SPICE Netlist check completed, 4 error(s), 0 warning(s) =======
The accessory includes three files, they are: 
PA78.TXT is the BERKELEY SPICE model about PA78 from
http://apex.cirrus.com/en/products/apex/design_software.html
PA78U_B.pdf is data sheet about PA78 from
http://apex.cirrus.com/en/products/pro/detail/P1163.html
PA78.ms10 is a bridge-connected configuration, but PA78 itself don't run a simulation.
帖子被Fangel在 01-28-2010 06:38 AM
时编辑过了
Solved!
Go to Solution.
Attachments:
PA78.TXT ‏7 KB
PA78U_B.pdf ‏820 KB
PA78.ms10 ‏139 KB

Answer 1

Hi,
I'll expand a little on what Angela said about the .ENDS, and then try to clear up the pins.
The SPICE model that you are using for the PA78 includes several subcircuits and models. Best practice for creating a component in Multisim is to have only a single .SUBCKT or .MODEL per component. The point of this is to make sure that any additional subcircuits or models are contained so that they don't interfere with each other in the final netlist. The easiest way to fix this is to move the .ENDS for the main subcircuit to the end of the entire block - so instead of just adding the .ENDS at the end, you would need to also remove the first .ENDS line in the file. For this circuit, you probably don't need to do that, however in general it's a good idea to do it when making a component like this.
As for the pins, step 6 of the Component Wizard is asking you for the order that the pins will be used in the model. The (original) model you have only has 10 nodes, so it's not a problem if you only have 10 pins there. If you have 12 pins on your symbol, and only 10 model nodes, then you just mark the two unused pins as "NC"(you can also add two "fake" pins to the .SUBCKT which is what you did, but you don't have to).
For the rest of the pins, look at the .SUBCKT line and the comments just before it:
* PINOUT ORDER +IN -IN IL OUT +VS -VS CR+ CC+ CR- CC-
* PINOUT ORDER 7 6 1 2 12 4 8 11 10 3
.SUBCKT PA78 7 6 1 2 12 4 8 11 10 3
 The comments telling you the pinout order are telling you the order that the pins must be listed when using the PA78 .SUBCKT. As you can see from the .SUBCKT line and comments, even though IL is pin 1 on the component, it actually needs to be listed third when using the .SUBCKT. That's what Step 6 in the Component Wizard is asking you for. Step 6 lets you tell Multisim the order in which to use the pins. The comment tells you that +IN is model node 1, -IN is model node 2, IL is model node 3, etc, and then you tell Multisim this by setting the model node numbers
Hope that helps!
Christopher Lansing
Software Developer
National Instruments