Too many parameters error in LTSpice III

[Martin Whybrow]

I am trying to simulate TL074 in LTSpice, here is my tl074.mod file
(downloaded from TI)

* TL074 OPERATIONAL AMPLIFIER "MACROMODEL" SUBCIRCUIT
* CREATED USING PARTS RELEASE 4.01 ON 06/16/89 AT 13:08
* (REV N/A) SUPPLY VOLTAGE: +/-15V
* CONNECTIONS: NON-INVERTING INPUT
* | INVERTING INPUT
* | | POSITIVE POWER SUPPLY
* | | | NEGATIVE POWER SUPPLY
* | | | | OUTPUT
* | | | | |
..SUBCKT TL074 1 2 3 4 5
*
C1 11 12 3.498E-12
C2 6 7 15.00E-12
DC 5 53 DX
DE 54 5 DX
DLP 90 91 DX
DLN 92 90 DX
DP 4 3 DX
EGND 99 0 POLY(2) (3,0) (4,0) 0 .5 .5
FB 7 99 POLY(5) VB VC VE VLP VLN 0 4.715E6 -5E6 5E6 5E6 -5E6
GA 6 0 11 12 282.8E-6
GCM 0 6 10 99 8.942E-9
ISS 3 10 DC 195.0E-6
HLIM 90 0 VLIM 1K
J1 11 2 10 JX
J2 12 1 10 JX
R2 6 9 100.0E3
RD1 4 11 3.536E3
RD2 4 12 3.536E3
RO1 8 5 150
RO2 7 99 150
RP 3 4 2.143E3
RSS 10 99 1.026E6
VB 9 0 DC 0
VC 3 53 DC 2.200
VE 54 4 DC 2.200
VLIM 7 8 DC 0
VLP 91 0 DC 25
VLN 0 92 DC 25
..MODEL DX D(IS=800.0E-18)
..MODEL JX PJF(IS=15.00E-12 BETA=270.1E-6 VTO=-1)
..ENDS

And this is my TL074.asy, modified from on of the existing op-amp models:
Version 4
SymbolType CELL
LINE Normal -32 32 32 64
LINE Normal -32 96 32 64
LINE Normal -32 32 -32 96
LINE Normal -28 48 -20 48
LINE Normal -28 80 -20 80
LINE Normal -24 84 -24 76
LINE Normal 0 32 0 48
LINE Normal 0 96 0 80
LINE Normal 4 44 12 44
LINE Normal 8 40 8 48
LINE Normal 4 84 12 84
WINDOW 0 16 32 Left 0
WINDOW 3 16 96 Left 0
SYMATTR Value 1/4 TL074
SYMATTR Prefix X
SYMATTR SpiceModel C:\Program Files\LTC\SwCADIII\lib\sym\Opamps\tl074.mod
SYMATTR Value2 1/4 TL074
SYMATTR Description Picoamp Input Current, µVolt Offset, Low noise
Operational Amplifier
PIN -32 80 NONE 0
PINATTR PinName 1
PINATTR SpiceOrder 1
PIN -32 48 NONE 0
PINATTR PinName 2
PINATTR SpiceOrder 2
PIN 0 32 NONE 0
PINATTR PinName 3
PINATTR SpiceOrder 3
PIN 0 96 NONE 0
PINATTR PinName 4
PINATTR SpiceOrder 4
PIN 32 64 NONE 0
PINATTR PinName 5
PINATTR SpiceOrder 5

This has been modified to change the description and model names and the
pinattr values have beem changed to match the .mod file.
When I use this component in LTSpice, I get the error "Fatal Error: Too many
parameters for subcircuit type "tl074" (instance: x§u1)"
Where am I going wrong?
Martin

 

[Jim Thompson]

I am trying to simulate TL074 in LTSpice, here is my tl074.mod file
(downloaded from TI)

* TL074 OPERATIONAL AMPLIFIER "MACROMODEL" SUBCIRCUIT
* CREATED USING PARTS RELEASE 4.01 ON 06/16/89 AT 13:08 [snip]
FB 7 99 POLY(5) VB VC VE VLP VLN 0 4.715E6 -5E6 5E6 5E6 -5E6

[snip]

Is this legitimate poly notation?

...Jim Thompson

 

[Mike Engelhardt]

Martin,

Change

SYMATTR Value2 1/4 TL074
to

SYMATTR Value2 TL074

Then your symbol will netlist just fine and
the model runs fine, too.

--Mike

 

[Martin Whybrow]

Martin,

Change


Then your symbol will netlist just fine and
the model runs fine, too.

--Mike

Mike
Thanks for that, it works fine now.
Martin.