WTD LTSpice 74HC04 spice or subcircuit

"Joe G (Home)" schrieb im Newsbeitrag news:4617b83a$0$15781$ snipped-for-privacy@news.optusnet.com.au...

Hello Joe,

The important question is what behaviour should be modeled.

If you want make a simple digital inverter, then an A-device with Vhigh, Vlow, Ref, Trise and Td will fit. This A-device will be simulated very fast. Vhigh=5 Ref=2.5 Td=5 Trise=5 I recommend to add a 50 Ohm resistor in series to the output. Adding the built-in input diodes may be also necessary if the input voltage exceeds the rails.

I have written a small library based on the A-models. It's in the LTspice Yahoo group. The devices fom this library will run slower than pure A-devices.

NXP offers a real transistor level model. A simulation will run slower than with a simple A-device of course too.

Best regards, Helmut

Example schematic(circuit), file name "74hc04_a.asc"

Version 4 SHEET 1 880 680 WIRE -528 -16 -576 -16 WIRE -576 16 -576 -16 WIRE -48 64 -48 32 WIRE -576 128 -576 96 WIRE -464 176 -576 176 WIRE -48 176 -48 128 WIRE -48 176 -192 176 WIRE 64 176 -48 176 WIRE 160 176 128 176 WIRE 368 176 240 176 WIRE -576 208 -576 176 WIRE -48 240 -48 176 WIRE -576 336 -576 288 WIRE -48 336 -48 304 FLAG -48 32 VCC FLAG -48 336 0 FLAG -576 336 0 FLAG 368 176 out IOPIN 368 176 Out FLAG -464 176 in IOPIN -464 176 Out FLAG -576 128 0 FLAG -528 -16 VCC FLAG -192 176 in IOPIN -192 176 In SYMBOL Digital\\\\inv 64 112 R0 WINDOW 123 -17 130 Left 0 WINDOW 39 -12 162 Left 0 SYMATTR InstName A1 SYMATTR Value2 Vhigh=5 Ref=2.5 SYMATTR SpiceLine Trise=5n Td=5n SYMBOL res 144 192 R270 WINDOW 0 32 56 VTop 0 WINDOW 3 0 56 VBottom 0 SYMATTR InstName R1 SYMATTR Value 50 SYMBOL diode -64 128 M180 WINDOW 0 24 72 Left 0 WINDOW 3 24 0 Left 0 SYMATTR InstName D1 SYMATTR Value DD SYMBOL diode -64 304 M180 WINDOW 0 24 72 Left 0 WINDOW 3 24 0 Left 0 SYMATTR InstName D2 SYMATTR Value DD SYMBOL voltage -576 192 R0 WINDOW 123 24 160 Left 0 WINDOW 39 24 132 Left 0 SYMATTR InstName V1 SYMATTR Value PULSE(0 5 10n 5n 5n 45n 100n) SYMATTR Value2 AC 1 SYMATTR SpiceLine Rser=50 SYMBOL voltage -576 0 R0 SYMATTR InstName V2 SYMATTR Value 5 TEXT -96 392 Left 0 ;optional TEXT 0 336 Left 0 !.model DD D(Cjo=5p Rs=10) TEXT 64 -32 Left 0 ;74HC04 TEXT -584 -128 Left 0 !.tran 0 250n 0 .1n TEXT -584 -96 Left 0 !.options plotwinsize=0 RECTANGLE Normal 320 432 -144 -64 2 CIRCLE Normal 16 368 -112 -32 2

Hi Helmut,

Many thanks for your reply.

Application RF oscillator - so NXP spice models look more attactive.

I would like to integrate the spice net lists from the NXP 74HC models in to LTSpice.

Do you have any guidance to do this?

Regards Joseph

Hello Joseph,

LTspice is strictly standard SPICE on a netlist level. This means you can directly run the examples(.cir) from the NXP-zip-file.

There is no SPICE standard for schematic entry. This means symbols are different in every SPICE with schematic entry. I think that you prefer a schematic instead of a pure netlist. LTspice offers you different possibilities for symbols. There are symbols you can edit on an instance level and others you can't. Both types are useful the same in many cases. It's a tradeoff regarding versatility and fool proof. In some cases it's necessary to go with one of them.

It's Easter and so the Easter bunny will bring you a gift via email. Let's hope your email address is valid. If not, send it to my address. It's a schematic example of an LC-oscilator with the 74HC04U /74HC04 using the NXP-MOSFET models.. Just replace the value 74HC04U with 74HC04 to switch to a 74HC04. LC-oscillators should be made with the unbuffered 74HC04U!

Happy Easter!

Best regards, Helmut

PS: I remember having read that Australians have banned the rabbits/bunnies from school books. Is that true?

"Joe G (Home)" schrieb im Newsbeitrag news:4617d576$0$16552$ snipped-for-privacy@news.optusnet.com.au...