IL300 Analog Optoisolator model problem

Mike, The old-style Microsim Schematics, which I use, rejects "^", but I can manually get PSpice itself to run a netlist with "^" in it as exponentiation.

The manual lists "^" as XOR, but I've not tried it... I only use the canned digital parts ;-)

Also, the manual only lists "**" for exponentiation. Maybe "^" is a legacy holdover that PSpice can handle simply because it's pretty easy to recognize logical operations as opposed to Algebraic.

...Jim Thompson

Cut n' Paste -- but I I am having problems getting my simulator to accept the TABLE for controlling the VCVS -- from a spice library

• A - Anode of LED
• C - Cathode of LED
• A1 - Anode of photodetector 1
• C1 - Cathode of photodetector 1
• A2 - Anode of photodetector 2
• C2 - Cathode of photodetector 2
• K1 - Servo gain
• K2 - Forward gain
• K3 - Transfer gain ..Subckt IL300 A C A1 C1 A2 C2 PARAMS: K1=0.007 K2=0.007 K3=1
• IL300 from Siemens * RAP 5/97 DLED A E Demit VE E C 0 E2 D1 0 TABLE ; {Ip2 vs IF}
• {(0.955414823*0.999409809^(1/(abs(I(VE))+0.1p))*I(VE)^0.963133681)}
• (0,0) (1,1) Rdly1 D1 D2 1K Cdly1 D2 0 0.17N Rdly2 D2 D3 1K Cdly2 D3 0 0.17N Gdly1 C1 A1 VALUE {K1*V(D3)} D1 A1 C1 Dtect RD1 A1 C1 15G Gdly2 C2 A2 VALUE {K3*K2*V(D3)} D2 A2 C2 Dtect RD2 A2 C2 15G ..model Demit D IS=1.51E-16 N=1.495822 RS=2.624361 BV=5 IBV=1U
• CJO=15P VJ=1 M=0.5 EG=1.424 TT=500N ..model Dtect D IS=0.5p N=1 RS=0.001 BV=50 IBV=1U
• CJO=14P VJ=0.159621 M=0.344264 EG=1.11 TT=10N ..ends

Thank you both.

Jack

Johnson,

It's a native PSpice model. LTspice can run it, but you need to change the "^" to "**" because LTspice understands "^" to be Boolean XOR instead of exponentiation. Below is the model running in a simple netlist in LTspice.

--Mike

• X1 A C A1 C1 A2 C2 IL300 V1 1 0 PULSE(-5 5 0 10n 10n 5u 10u) R1 1 A 1K R2 1 A1 1K R3 1 A2 1K V2 2 0 5 R4 2 C 1K R5 2 C1 1K R6 2 C2 1K

..Subckt IL300 A C A1 C1 A2 C2 PARAMS: K1=0.007 K2=0.007 K3=1 DLED A E Demit VE E C 0 E2 D1 0 TABLE ; {Ip2 vs IF}

• {(0.955414823*0.999409809**(1/(abs(I(VE))+0.1p))*I(VE)**0.963133681)}
• (0,0) (1,1) Rdly1 D1 D2 1K Cdly1 D2 0 0.17N Rdly2 D2 D3 1K Cdly2 D3 0 0.17N Gdly1 C1 A1 VALUE {K1*V(D3)} D1 A1 C1 Dtect RD1 A1 C1 15G Gdly2 C2 A2 VALUE {K3*K2*V(D3)} D2 A2 C2 Dtect RD2 A2 C2 15G ..model Demit D IS=1.51E-16 N=1.495822 RS=2.624361 BV=5 IBV=1U
• CJO=15P VJ=1 M=0.5 EG=1.424 TT=500N ..model Dtect D IS=0.5p N=1 RS=0.001 BV=50 IBV=1U
• CJO=14P VJ=0.159621 M=0.344264 EG=1.11 TT=10N ..ends

..tran 50u 50u ..probe ..end

Jim,

I wish it true because it's one of the few incompatibilities between LTspice and PSpice that I can't change without breaking models already using "^" as XOR. But in this ABM context, PSpice uses "^" as exponentiation instead of XOR. Here's an example to illustrate:

• V1 1 0 PULSE(0 2 0 .5m .5m 1u 1.002m ) E1 2 0 value { 2 ^ V(1) } ; LTspice: XOR, PSpice: exponentiation E2 3 0 value { 2 ** V(1) } ; LTspice & PSpice: exponentiation ..tran 3m 3m ..probe ..end

Regards,

--Mike