Which tool can simulate MC1496 ?
i want to simulate the the MC1496 (differentialModulator and DeModulator).
which program can simulate it?
regards.
Mostafa
if you search , you find :
https://www.edaboard.com/viewtopic.php?p=466669
Circuit Maker 2000 student version includes a MC1496 spice model. Install this software and try to copy the model to Pspice.
h**p://www.microcode.com/downloads/files/cmstudnt.exe
or with google:
http://tardis.union.edu/~hedrickj/eer133/lab6.html
FFFFFF
Model from CM2000 is here:
*******************
*MC1496 MCE 1-31-96
*Balanced Modulator/Demodulator
*Nodes: GainAdj Vc Vc Vs Vs Vee Bias Out Out GainAdj
*Motorola/MCE Balanced Modulator/Demod pkg:DIP14 pkg:SO-14
.SUBCKT XMC1496 3 11 10 9 8 7 6 4 5 2
Q1 3 6 14 QNPN
Q2 15 9 3 QNPN
Q3 4 11 15 QNPN
Q4 5 11 16 QNPN
Q5 5 10 15 QNPN
Q6 16 8 2 QNPN
Q7 2 6 13 QNPN
Q8 4 10 16 QNPN
D1 6 12 DDIODE
R1 7 12 500
R2 7 13 500
R3 7 14 500
.MODEL QNPN NPN()
.MODEL DDIODE D()
.ENDS XMC1496
***********************
hi Borber and FFFFFF
really thanks! it is working, also i found this IC in PROTEL99 SE.
regards, Mostafa
Here is more "realistic" model:
*************************
.subckt MC1496 1 2 3 4 5 6 8 10 12 14
* Tail current Source
Q1 3 5 19 Q2nn
Q2 2 5 13 Q2nn
* Input transistors
Q3 7 4 3 Q2nn
Q4 9 1 2 Q2nn
*LO quad switching Transistors
Q5 6 8 7 Q2nn
Q6 6 10 9 Q2nn
Q7 12 10 7 Q2nn
Q8 12 8 9 Q2nn
* Emitter degeneration resistors
RE1 19 14 500
RE2 13 14 500
*
* Current Mirror
Q9 5 5 15 Q2nn
Rd 15 14 500
.ENDS
.MODEL Q2nn NPN(
+ISS=0 XTF=1 NS=1
+CJS=0 VJS=0.5 PTF=0
+MJS=0 EG=1.1 AF=1
+ITF=0.5 VTF=1 BF=280.92203
+BR=20 IS=2.3673E-15 VAF=130.20848
+VAR=11.074004 IKF=0.23419 ISE=3.0707E-16
+NE=1.19409 IKR=7.80101 ISC=3.5223E-12
+NC=1.33867 IRB=1.8864E-4 NF=0.97302
+NR=0.97623 RBM=1E-2 RB=69.94226
+RC=3E-02 RE=0.2569 MJE=0.36064
+MJC=0.29228 VJE=0.81795 VJC=0.45460
+TF=5E-10 TR=6.2636E-09 CJE=6.7441E-12
+CJC=3.4247E-12 FC=0.95 XCJC=0.95425)
************************************************** ****
hi Borber
i can simulate this IC in protel 99 SE, but i couldn't simulate it in OrCAD(captureCIS). how can i import your model file into orcad.
regards
Errors corrected!
This is PSpice subcircuit. Check if Orcad uses PSpice, I don't know.
Hi, How can I use this model in PSpice?
Thanks
You can use this model in a simulation program which supports PSpice. Microcap, Multisim...