I have toyed with a circuit idea. And during xmas holiday a plan to do some simulations just to check if my idea may work or certainly not work. The chip I am going to use is a MC1496 balanced modulator. But I do not have any spice model. Can anyone help me out here? Also please tell me which package type the model is designed for. DIP and metal cans have different pin number

 

Here is a library file that contains subcircuits that I created for both the 10 pin (LM1496H) and the 14 pin (LM1496N) versions. I'm including a sample .ASC file so you can see how they are used in LTspice. For any other version of spice, you're on your own.

If you are using LTspice, copy and paste the following into Notepad, then save in your SUB folder as LM1496.lib.

*LM1496N 14 pins
*              +sig_in gain1 gain2 -sig_in bias out1 NC  +carr_in NC  -carr_in NC  out2 NC  V- 
.subckt LM1496N    1      2     3      4     5    6   7      8     9      10    11   12  13  14
Q1 6 8 N001 0 CA3046
Q2 12 10 N001 0 CA3046
Q3 6 10 N002 0 CA3046
Q4 12 8 N002 0 CA3046
Q5 N001 4 3 0 CA3046
Q6 N002 1 2 0 CA3046
Q7 3 5 N003 0 CA3046
R1 N003 14 500
Q8 2 5 N004 0 CA3046
R2 N004 14 500
Q9 5 5 N005 0 CA3046
R3 N005 14 500
R101 7 9 1e12
R102 9 11 1e12
R103 11 13 1e12
R104 13 7 1e12
R105 13 0 1e12
.ends LM1496N
*******************


* LM1496H 10 pins
*              +sig_in gain1 gain2 -sig_in bias out1  +carr_in  -carr_in  out2  V- 
.subckt LM1496H    1      2     3      4     5    6     8    10   12   14
Q1 6 8 N001 0 CA3046
Q2 12 10 N001 0 CA3046
Q3 6 10 N002 0 CA3046
Q4 12 8 N002 0 CA3046
Q5 N001 4 3 0 CA3046
Q6 N002 1 2 0 CA3046
Q7 3 5 N003 0 CA3046
R1 N003 14 500
Q8 2 5 N004 0 CA3046
R2 N004 14 500
Q9 5 5 N005 0 CA3046
R3 N005 14 500
R101 7 9 1e12
R102 9 11 1e12
R103 11 13 1e12
R104 13 7 1e12
R105 13 0 1e12
.ends LM1496H
**************************************

.model CA3046 NPN (IS=10.0e-15 XTI=3.000e+00 EG=1.110e+00 VAF=1.00e+02 VAR=1.000e+02 

BF=145.7e+00 ISE=114.286e-15 NE=1.480e+00 IKF=46.700e-03 XTB=0.000e+00 BR=.1000e+00 

ISC=10.005e-15 NC=2.000e+00 IKR=10.00e-03 RC=10.000e+00 CJC=991.71e-15 MJC=0.333e-00 

VJC=0.7500e-00 FC=5.000e-01 CJE=1.02e-12 MJE=.336E- 00 VJE=0.750e-00 TR=10.000e-09 

TF=277.01e-12 ITF=1.750e-00 XTF=309.38e+00 VTF=16.37e+00 PTF=0.000e+00 RE=0.0e+00 

RB=0.00e+00)

 

Here is a library file that contains subcircuits that I created for both the 10 pin (LM1496H) and the 14 pin (LM1496N) versions. I'm including a sample .ASC file so you can see how they are used in LTspice. For any other version of spice, you're on your own.

If you are using LTspice, copy and paste the following into Notepad, then save in your SUB folder as LM1496.lib

Nice one Ron. I will be using Altium for simulation. I am looking forward to test your file. Perhaps to day. Just need some time to draw the schematics.