LTSpice

[ivconic]

Anybody have model CD4528/CD4538 for LTSpice?

[Davor]

Izvoli

Works %)$#/=/($ slow though, have patience.

[ivconic]

Thanks Davor!

[Derx]

Anybody have model CD4060 for LTSpice?

[Davor]

Nope, too many flipflops. You can make it using basic building blocks and connect as many flipflops you actually need.

[Derx]

Model CD4020 already exists, this 14-stage counter, but without oscillator generator block

How to make CD4060 from CD4020? or from CD4040?

[Davor]

You can use a 4069 model for the missing inverter. It has symmetrical fets unlike 4049s and it should mimic the operation of 4060 better.

[ODM]

For generic HCMOS gate oscillators, check this reference:
http://www.fairchildsemi.com/an/AN/AN-340.pdf

[Derx]

How to convert ORCAD PSpice Macromodel to LTSpice macromodel?
need tools
--------
*$
* PART NUMBER:NJM4558
* MANUFACTURER: NEW JAPAN RADIO
* All Rights Reserved Copyright (c) Bee Technologies Inc. 2004
.Subckt NJM4558 OUT1 -IN1 +IN1 V- +IN2 -IN2 OUT2 V+
X_U1 +IN1 -IN1 V+ V- OUT1 NJM4558_SUB
X_U2 +IN2 -IN2 V+ V- OUT2 NJM4558_SUB
.ends NJM4558
*$
.subckt NJM4558_SUB 1 2 3 4 5
c1 11 12 7.7942E-12
c2 6 7 27.000E-12
dc 5 53 dy
de 54 5 dy
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 7.0736E6 -1E3 1E3 7E6 -7E6
ga 6 0 11 12 575.49E-6
gcm 0 6 10 99 18.198E-9
iee 3 10 dc 30.051E-6
hlim 90 0 vlim 1K
q1 11 2 13 qx1
q2 12 1 14 qx2
r2 6 9 100.00E3
rc1 4 11 1.7684E3
rc2 4 12 1.7684E3
re1 13 10 44.035
re2 14 10 44.035
ree 10 99 6.6553E6
ro1 8 5 50
ro2 7 99 25
rp 3 4 1.8032E3
vb 9 0 dc 0
vc 3 53 dc 1.7979
ve 54 4 dc 1.7979
vlim 7 8 dc 0
vlp 91 0 dc 2.9500
vln 0 92 dc 2.9500
.model dx D(Is=800.00E-1
.model dy D(Is=800.00E-18 Rs=1m Cjo=10p)
.model qx1 PNP(Is=800.00E-18 Bf=519.03)
.model qx2 PNP(Is=1.008900E-15 Bf=666.67)
.ends
*$

[Davor]

It should work as is, provided you have a LTspice symbol that fits with the .Subckt pinout statement.
You'll find MC4558 model and symbol ready for LTspice at yahoo group instead.

[Derx]

I take a lot of models from manufacturers directly so I need to learn how to convert these models so that they work properly.
I'm interested to know what do the letter abbreviations in the parameters

[Qiaozhi]

I take a lot of models from manufacturers directly so I need to learn how to convert these models so that they work properly.
I'm interested to know what do the letter abbreviations in the parameters

Get yourself a copy of Paul Tuinenga's SPICE book "A Guide to Circuit Simulation & Analysis Using PSpice", ISBN 0-13-158775-7
http://www.amazon.co.uk/Spice-Circui...2828642&sr=8-2

[Davor]

There are two kinds of symbols in LTspice, it's own uncooperative, and component specific. You can rename the component specific one and edit the model name within it - it is a text file after all. The important detail is contained in this line of a model:
.Subckt NJM4558 OUT1 -IN1 +IN1 V- +IN2 -IN2 OUT2 V+

If you commit yourself to learn how to make your own symbols, you'll find some tutorials on the net. I'm the lazy one - I tend to adopt the existing ones to my needs by editing , if necessary. In this particular case you have a model of a dual op amp, and a solution is using a pinout chip-like symbol.
This one works, just copy it to text editor and name it NJM4558.asc

Version 4
SymbolType CELL
RECTANGLE Normal -112 -128 112 128
WINDOW 0 0 -144 Center 0
WINDOW 3 0 144 Center 0
SYMATTR Value NJM4558
SYMATTR Prefix X
PIN -112 -96 LEFT 8
PINATTR PinName out
PINATTR SpiceOrder 1
PIN -112 -32 LEFT 8
PINATTR PinName -in
PINATTR SpiceOrder 2
PIN -112 32 LEFT 8
PINATTR PinName +in
PINATTR SpiceOrder 3
PIN -112 96 LEFT 8
PINATTR PinName VSS
PINATTR SpiceOrder 4
PIN 112 96 RIGHT 8
PINATTR PinName in+
PINATTR SpiceOrder 5
PIN 112 32 RIGHT 8
PINATTR PinName in-
PINATTR SpiceOrder 6
PIN 112 -32 RIGHT 8
PINATTR PinName out
PINATTR SpiceOrder 7
PIN 112 -96 RIGHT 8
PINATTR PinName VDD
PINATTR SpiceOrder 8

I recycled a wien bridge oscillator to show you how it works. This one is also for mikebg and his fascination with PID regulators in oscillator circuits - it acquires stability ... eventually, but only illusory stability - it will re-flutter once faced with any quick load change. Oscillator's envelope behaves as an integrator with constant slew rate, hence oscillation.

[mikebg]

Davor, your circuit diagram contains P-I controller. It can be redesigned for better operation.

[Davor]

Davor, your circuit diagram contains P-I controller.

And yours doesn't. That's the whole difference. Of course it works better. A charge pump adds only a single pole in the loop, hence no flutter.

Everything else considered, yes, some kind of control is OK in the oscillator circuitry if it achieves any of the design goals, but NOT the PID because of the "I" component. Considering the oscillator by itself is an integrator with all the saturation effects near the rail amplitude providing the proportional regulation, it is a self contained PI regulator. You could add some kind of control to avoid near the rail non-linearities, but be careful about it - regulating conduction angle is a bad idea.