Pspice transfer function

[Robert Baer]

When i test the actual circuit, the output has a transition "hump"
between the linear I/O part and the regulation part; it is about 900mV
in amplitude.
The Spice does not show it; why?
** Regulator.asc
Version 4
SHEET 1 880 680
WIRE -400 208 -400 -32
WIRE -368 -32 -400 -32
WIRE -272 -32 -288 -32
WIRE -272 144 -272 -32
WIRE -240 144 -272 144
WIRE -32 144 -160 144
WIRE -32 144 -32 64
WIRE -32 176 -32 144
WIRE -32 336 -32 272
WIRE 64 -32 -272 -32
WIRE 64 144 -32 144
WIRE 64 224 32 224
WIRE 64 224 64 208
WIRE 112 64 -32 64
WIRE 112 64 112 32
WIRE 256 -32 160 -32
WIRE 256 64 256 -32
WIRE 256 224 64 224
WIRE 256 224 256 144
WIRE 256 272 256 224
WIRE 256 384 256 352
WIRE 336 384 256 384
WIRE 336 384 336 240
WIRE 368 -32 256 -32
WIRE 368 128 368 -32
WIRE 368 240 336 240
WIRE 368 240 368 192
WIRE 368 272 368 240
WIRE 480 -32 368 -32
WIRE 480 128 480 -32
WIRE 480 240 368 240
WIRE 480 240 480 208
FLAG -400 288 0
FLAG -32 400 0
FLAG 368 272 0
SYMBOL npn 64 32 R270
WINDOW 0 136 33 VRight 0
WINDOW 3 100 7 VRight 0
SYMATTR InstName Q1
SYMATTR Value ZTX849
SYMBOL Misc\\battery -400 192 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value 38V
SYMBOL res -272 -48 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R1
SYMATTR Value 1e-3
SYMBOL npn 32 176 M0
WINDOW 0 103 58 Left 0
WINDOW 3 77 24 Left 0
SYMATTR InstName Q3
SYMATTR Value FMMT459
SYMBOL zener -16 400 R180
WINDOW 0 24 72 Left 0
WINDOW 3 62 38 Left 0
SYMATTR InstName D1
SYMATTR Value BZX84C12L
SYMBOL cap 48 144 R0
SYMATTR InstName C1
SYMATTR Value 150pF
SYMBOL current -240 144 R270
WINDOW 0 -32 40 VBottom 0
WINDOW 3 32 40 VTop 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName I1
SYMATTR Value 1mA
SYMBOL cap 352 128 R0
SYMATTR InstName C2
SYMATTR Value .01ľF
SYMBOL res 240 48 R0
SYMATTR InstName R2
SYMATTR Value 175K
SYMBOL res 240 256 R0
SYMATTR InstName R3
SYMATTR Value 125K
SYMBOL res 464 112 R0
SYMATTR InstName R4
SYMATTR Value 10K
TEXT 304 -72 Left 0 ;N006
TEXT -96 -64 Left 0 ;N002
TEXT 144 248 Left 0 ;N005
TEXT -128 120 Left 0 ;N003
TEXT -328 -176 Left 0 !.dc V1 31 33 0.01
TEXT -328 -144 Left 0 !.LIB D:\\SPICE\\ZMODELS.LIB

 

[Helmut Sennewald]

"Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
news:kfWke.6344$Lc1.6222@newsread3.news.pas.earthlink.net...

When i test the actual circuit, the output has a transition "hump"
between the linear I/O part and the regulation part; it is about 900mV in
amplitude.
The Spice does not show it; why?

Hello Robert,
Where did you uy the 1mA-current source?
Type:?
Manufacturer:?

Is it just a schematic simplification?
Then please provide the real circuit(schematic) for this current source.

Is this Z-diode in the real circuit or is this also some kind of
simplification for another device?

Have you tried to replace this crrent source with a simple 33k resistor.
It would be very interesting how your real circuit behaves then
compared to the simulation.

Best regards,
Helmut

 

[Robert Baer]

Helmut Sennewald wrote:

"Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
news:kfWke.6344$Lc1.6222@newsread3.news.pas.earthlink.net...

When i test the actual circuit, the output has a transition "hump"
between the linear I/O part and the regulation part; it is about 900mV in
amplitude.
The Spice does not show it; why?



Hello Robert,
Where did you uy the 1mA-current source?
Type:?
Manufacturer:?

Is it just a schematic simplification?
Then please provide the real circuit(schematic) for this current source.

Is this Z-diode in the real circuit or is this also some kind of
simplification for another device?

Have you tried to replace this crrent source with a simple 33k resistor.
It would be very interesting how your real circuit behaves then
compared to the simulation.

Best regards,
Helmut





The current source is a DMOSFET; the DN3545 and a 2.2K resistor.

Do not know how to model that.
This was tested using an E-B transistor junction (in reverse) for the
zener; the transistor type was selected to have no negative R effects
and have low noize at all currents from nanoamps to milliamps.
The "hump" mentioned was measured not only with meters, but also seen
on a curve tracer.

 

[Helmut Sennewald]

"Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
newscgle.591$IL3.180@newsread3.news.pas.earthlink.net...

Helmut Sennewald wrote:

"Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
news:kfWke.6344$Lc1.6222@newsread3.news.pas.earthlink.net...

When i test the actual circuit, the output has a transition "hump"
between the linear I/O part and the regulation part; it is about 900mV
in amplitude.
The Spice does not show it; why?

Hello Robert,
Where did you uy the 1mA-current source?
Type:?
Manufacturer:?

Is it just a schematic simplification?
Then please provide the real circuit(schematic) for this current source.

Is this Z-diode in the real circuit or is this also some kind of
simplification for another device?

Have you tried to replace this crrent source with a simple 33k resistor.
It would be very interesting how your real circuit behaves then
compared to the simulation.

Best regards,
Helmut

The current source is a DMOSFET; the DN3545 and a 2.2K resistor.
Do not know how to model that.

Hello Robert,

You could try to find a SPICE model of a similar device
from another manufacturer.

This was tested using an E-B transistor junction (in reverse) for the
zener; the transistor type was selected to have no negative R effects and
have low noize at all currents from nanoamps to milliamps.
The "hump" mentioned was measured not only with meters, but also seen on
a curve tracer.

That's it.
If you replace this "bad" device with a real Zener diode, the
problem should go away. It's a very very bad idea to use the
B-E breakdown as a Zener-diode for any serious application.

I rate the whole thing not as a problem to find a SPICE
model for the B-E breakdown. It's simply a bad design
practice to use this B-E breakdown as a reference voltage.

Best regards,
Helmut

 

[Robert Baer]

Helmut Sennewald wrote:

"Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
newscgle.591$IL3.180@newsread3.news.pas.earthlink.net...

Helmut Sennewald wrote:


"Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
news:kfWke.6344$Lc1.6222@newsread3.news.pas.earthlink.net...


When i test the actual circuit, the output has a transition "hump"
between the linear I/O part and the regulation part; it is about 900mV
in amplitude.
The Spice does not show it; why?

Hello Robert,
Where did you uy the 1mA-current source?
Type:?
Manufacturer:?

Is it just a schematic simplification?
Then please provide the real circuit(schematic) for this current source.

Is this Z-diode in the real circuit or is this also some kind of
simplification for another device?

Have you tried to replace this crrent source with a simple 33k resistor.
It would be very interesting how your real circuit behaves then
compared to the simulation.

Best regards,
Helmut


The current source is a DMOSFET; the DN3545 and a 2.2K resistor.
Do not know how to model that.


Hello Robert,

You could try to find a SPICE model of a similar device
from another manufacturer.


This was tested using an E-B transistor junction (in reverse) for the
zener; the transistor type was selected to have no negative R effects and
have low noize at all currents from nanoamps to milliamps.
The "hump" mentioned was measured not only with meters, but also seen on
a curve tracer.


That's it.
If you replace this "bad" device with a real Zener diode, the
problem should go away. It's a very very bad idea to use the
B-E breakdown as a Zener-diode for any serious application.

I rate the whole thing not as a problem to find a SPICE
model for the B-E breakdown. It's simply a bad design
practice to use this B-E breakdown as a reference voltage.

Best regards,
Helmut


Sorry, this particular transistor E-B junction is superior to any

zener diode i have seen. Furthermore, if i add in the B-C junction in
forward mode, i get a voltage reference good to 180C.
Furthermore, when i replace it with a UCC2801 (zeners near 13.5V), i
see exactly the same thing.

 

[Helmut Sennewald]

"Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
news:EXole.854$MI4.769@newsread2.news.pas.earthlink.net...

Helmut Sennewald wrote:

"Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
newscgle.591$IL3.180@newsread3.news.pas.earthlink.net...

Helmut Sennewald wrote:


"Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
news:kfWke.6344$Lc1.6222@newsread3.news.pas.earthlink.net...


When i test the actual circuit, the output has a transition "hump"
between the linear I/O part and the regulation part; it is about 900mV
in amplitude.
The Spice does not show it; why?

Hello Robert,
Where did you uy the 1mA-current source?
Type:?
Manufacturer:?

Is it just a schematic simplification?
Then please provide the real circuit(schematic) for this current source.

Is this Z-diode in the real circuit or is this also some kind of
simplification for another device?

Have you tried to replace this crrent source with a simple 33k resistor.
It would be very interesting how your real circuit behaves then
compared to the simulation.

Best regards,
Helmut


The current source is a DMOSFET; the DN3545 and a 2.2K resistor.
Do not know how to model that.


Hello Robert,

You could try to find a SPICE model of a similar device
from another manufacturer.


This was tested using an E-B transistor junction (in reverse) for the
zener; the transistor type was selected to have no negative R effects
and have low noize at all currents from nanoamps to milliamps.
The "hump" mentioned was measured not only with meters, but also seen
on a curve tracer.


That's it.
If you replace this "bad" device with a real Zener diode, the
problem should go away. It's a very very bad idea to use the
B-E breakdown as a Zener-diode for any serious application.

I rate the whole thing not as a problem to find a SPICE
model for the B-E breakdown. It's simply a bad design
practice to use this B-E breakdown as a reference voltage.

Best regards,
Helmut
Sorry, this particular transistor E-B junction is superior to any zener
diode i have seen. Furthermore, if i add in the B-C junction in forward
mode, i get a voltage reference good to 180C.
Furthermore, when i replace it with a UCC2801 (zeners near 13.5V), i see
exactly the same thing.

Hello Robert,

Is this "bump" a dynamic behaviour when the inut voltage is ramped up
with a certain speed or is it also visible when you manually
increase the input voltage very slowly?

Means this "bump" a higher or a lower voltage?

Best regards,
Helmut

 

[Robert Baer]

----------- SNIPped for brevity -----------

Sorry, this particular transistor E-B junction is superior to any zener
diode i have seen. Furthermore, if i add in the B-C junction in forward
mode, i get a voltage reference good to 180C.
Furthermore, when i replace it with a UCC2801 (zeners near 13.5V), i see
exactly the same thing.



Hello Robert,

Is this "bump" a dynamic behaviour when the inut voltage is ramped up
with a certain speed or is it also visible when you manually
increase the input voltage very slowly?

Means this "bump" a higher or a lower voltage?

Best regards,
Helmut


The "bump" is seen at any speed - curve tracer or manual input

voltage increments.
The "bump" is seen "at" the transition between the linear I-V from
zero to the regulation at the output.
I have experimented with various voltage dividers, the E-B-C
transistor, the UCC2801 (which is what will be used) and a 15V zener.
Depending on what i use, i see two different kinds of curves.
1) I-V slope abruptly changes to a lower value (higher R) during turn-on
of the depletion mode MOSFET, then abruptly flat ("infinite" R) at
regulation; no "bump".
2) I-V slope abruptly changes to a higher value (lower R) during turn-on
of the depletion mode MOSFET, then abruptly flat ("infinite" R) at
regulation; has "bump".
I fiddled around with a few FETS in the library (there are no models
for a depletion mode FET) to replace the current source.
The result is similar to case #1 above, except the first transition
is not abrupt (enhancement mode FETS are log Id VS Vgs, and maybe
depletion mode FETS are loglog?).
--------------
Version 4
SHEET 1 880 680
WIRE -400 208 -400 -32
WIRE -368 -32 -400 -32
WIRE -272 -32 -288 -32
WIRE -272 144 -272 -32
WIRE -80 144 -96 144
WIRE -80 192 -112 192
WIRE -80 192 -80 144
WIRE -32 144 -80 144
WIRE -32 144 -32 64
WIRE -32 176 -32 144
WIRE -32 336 -32 272
WIRE 64 -32 -272 -32
WIRE 64 144 -32 144
WIRE 64 224 32 224
WIRE 64 224 64 208
WIRE 112 64 -32 64
WIRE 112 64 112 32
WIRE 256 -32 160 -32
WIRE 256 64 256 -32
WIRE 256 224 64 224
WIRE 256 224 256 144
WIRE 256 272 256 224
WIRE 256 384 256 352
WIRE 336 384 256 384
WIRE 336 384 336 240
WIRE 368 -32 256 -32
WIRE 368 128 368 -32
WIRE 368 240 336 240
WIRE 368 240 368 192
WIRE 368 272 368 240
WIRE 480 -32 368 -32
WIRE 480 128 480 -32
WIRE 480 240 368 240
WIRE 480 240 480 208
FLAG -400 288 0
FLAG -32 400 0
FLAG 368 272 0
SYMBOL npn 64 32 R270
WINDOW 0 136 33 VRight 0
WINDOW 3 100 7 VRight 0
SYMATTR InstName Q1
SYMATTR Value ZTX849
SYMBOL Misc\\battery -400 192 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value 38V
SYMBOL res -272 -48 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R1
SYMATTR Value 1e-3
SYMBOL npn 32 176 M0
WINDOW 0 3 106 Left 0
WINDOW 3 -80 133 Left 0
SYMATTR InstName Q3
SYMATTR Value FMMT459
SYMBOL zener -16 400 R180
WINDOW 0 24 72 Left 0
WINDOW 3 62 38 Left 0
SYMATTR InstName D1
SYMATTR Value BZX84C6V2L
SYMBOL cap 48 144 R0
SYMATTR InstName C1
SYMATTR Value 150pF
SYMBOL cap 352 128 R0
SYMATTR InstName C2
SYMATTR Value .01ľF
SYMBOL res 240 48 R0
SYMATTR InstName R2
SYMATTR Value 175K
SYMBOL res 240 256 R0
SYMATTR InstName R3
SYMATTR Value 125K
SYMBOL res 464 112 R0
SYMATTR InstName R4
SYMATTR Value 10K
SYMBOL nmos -272 192 R270
WINDOW 0 69 11 VRight 0
WINDOW 3 -16 -37 VRight 0
SYMATTR InstName M1
SYMATTR Value IRL3915
SYMBOL Misc\\battery -208 192 R270
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
WINDOW 0 -53 3 VRight 0
WINDOW 3 -54 42 VRight 0
SYMATTR InstName V2
SYMATTR Value 4.25V
SYMBOL res -80 128 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 -56 57 VTop 0
SYMATTR InstName R5
SYMATTR Value 2.2K
TEXT 304 -72 Left 0 ;N006
TEXT -96 -64 Left 0 ;N002
TEXT 144 248 Left 0 ;N005
TEXT -56 40 Left 0 ;N003
TEXT -328 -176 Left 0 !.dc V1 10 25 0.001
TEXT -328 -144 Left 0 !.LIB D:\\SPICE\\ZMODELS.LIB

 

[Robert Baer]

----------- SNIPped for brevity -----------

Offending part: the UCC2801 has a *large* negative resistance "kink";
that is what caused the wierd curves seen.
The compensation capacitor used was large enough, in combination to
the gain loss in the feedback divider, allowed the regulator to operate
smoothly at all measured points.

And that brings up the question as to how to model such a beastie...

 

[Helmut Sennewald]

"Robert Baer" <robertbaer@earthlink.net> schrieb im Newsbeitrag
news:7Czle.1134$MI4.547@newsread2.news.pas.earthlink.net...

----------- SNIPped for brevity -----------

Offending part: the UCC2801 has a *large* negative resistance "kink";
that is what caused the wierd curves seen.
The compensation capacitor used was large enough, in combination to the
gain loss in the feedback divider, allowed the regulator to operate
smoothly at all measured points.

And that brings up the question as to how to model such a beastie...

Hello Robert,

You could add a resistor in series with a negative
resistance, e.g. -200 Ohm.
A more complex behaviour can be modeled with B-sources.
Be warned, dealing with negative resistance always causes
a lot of headache with convergence.

Btw, the DN3545 model is on the website of Supertex.
It's a 4-pin subcircuit. This requires to change the Prefix
in the instance of your "nmos4" to X. Don't change the
original symbol!!! An instance is the already placed
symbol in your schematic.

I have send my LTspice file to your email address.
I can't attach it here because it contains too long
lines. Only very experienced LTspice users could restruct
these splitted lines. If somebody eles wants this file,
then send me an email so I can send it to you.

Best regards,
Helmut


PS: We are simulating here with LTspice and not wit PSPICE.
LTspice is free and unlimited SPICE with a GUI. It's
also named SwitcherCADIII.
Download it from here: www.linear.com

There is also an independent user group. It's a moderated
group and it requires to register for access.
There are over 6000 messages now there and hundreds of
examples, links and other stuff.
http://groups.yahoo.com/group/LTspice

I am one of the two moderators of this group.



Supertex SPICE model
--------------------

*
* MARCH 07, 2000
*
* COMPOSITE MODEL FOR DN3545
*
..SUBCKT DN3545 1 2 3 4
*
* NODE 1 = DRAIN
* NODE 2 = GATE
* NODE 3 = SOURCE
* NODE 4 = BODY
*
MOS1 11 2 3 4 ND_DMOS L=2.5E-06 W=58E-3
JFET 1 3 11 JMOD 1
DBODY 4 1 DMOS
R 1 11 1E+6
*
..MODEL ND_DMOS NMOS
+ LEVEL=3 UO=307 VTO=-1.829 NFS=5.0E+11
+ TOX=5E-08 NSUB=3.59E+15 NSS=0 VMAX=5E+04
+ RS=1E-06 RD=1E-06 RSH=5000 CGDO=1.96E-9
+ CGSO=1.5E-09 CGBO=0 CBD=4.0E-11 CBS=1.0E-15
+ MJ=0.5003 MJSW=0.33 IS=5E-13 PB=0.4507
+ FC=0.5 XJ=1.2E-05 LD=0 DELTA=0
+ THETA=0 ETA=1.0E-6 KAPPA=1.0E-6
*
..MODEL DMOS D
+ IS=281.0E-15 N=0.950 RS=2.5
+ BV=450 IBV=1.0E-3 TT=1.0E-6
*
..MODEL JMOD NJF
+ VTO=-3.5 BETA=0.100 IS=281E-15
+ RD=9.0 LAMBDA=0
..ENDS