Robert Baer said:I see no way to add an arbitrary device and use X to call its use.
Not even if it happens to be a zener defined with a .SUBCKT ..
Good thing i kept my DOS version of TopSpice!
I see no way to add an arbitrary device and use X to call its use.
Not even if it happens to be a zener defined with a .SUBCKT ..
Good thing i kept my DOS version of TopSpice!
I see no way to add an arbitrary device and use X to call its use.
Not even if it happens to be a zener defined with a .SUBCKT ..
Good thing i kept my DOS version of TopSpice!
Thanks; i will try exactly as you suggested.Helmut said:Hello Robert,
LTspice can handle subcircuits of course.
Maybe you haven't correctly setup your subcircuit or symbol.
There are in general differences between the SPICE varieties
when it comes to parameter passing to subcircuits.
LTspice is mostly compatible to PSPICE regarding parameters.
Why haven't you posted your LTspice schematic and subcircuit?
Now I have to make some guess what you have done wrong.
I have assumed that you try to use Z-diode subcircuit models
from ONSEMI. They provide two models for each Z-diode.
Prefer to use the PSPICE compatible models(.lib) and not the
SPICE3 models(.sp3) from ONSEMI, because SPICE3 has a different
syntax for the model statement of resistors. Normally you don't
have or need .model statements for resistors.
PSPICE:
RBV 6 0 MDRBV 1749.5
.MODEL MDRBV RES TC1=-0.000940267
SPICE3:
RBV 6 0 1749.5 MDRBV
.MODEL MDRBV R TC1=-0.000940267
LTspice allows you to have the tempco in the same line.
RBV 6 0 1749.5 TC1=-0.000940267
I have made an example for you with a Z-diode(4.7V) from ONSEMI.
It is defined with a subcircuit. The only important thing with
the ONSEMI library is to use the PSPICE compatible ".lib"
file and not the SPICE3(.sp3) file.
Save the attached schematic file with name "zdiode_test.asc"
and save the model file as "bzx84b4v7lt1.lib".
Please keep both files in the same directory.
I have also attached a few instructions how to change symbols
which are designed for models so that they can be used for
subcircuits. So you don't have to draw an extra symbol.
Best regards,
Helmut
------ INSTRUCTIONS FOR SUBCIRCUIT( ZENER-)DIODES ------
1. Add a diode to the schematic.
2. Move the cursor over the placed diode.
Press <Ctrl>RightMouseButton
Change Prefix D to X
OK
Now this diode expects a ".SUBCKT ..." definition, because of the X.
3. Change the value D of the diode in your schematic to bzx84b4v7lt1.
4. Place the subcircuit definition in the schematic or load it from a file.
In the ladder case add a ".include bzx84b4v7lt1.lib" to the schematic.
Save the subcircuit definition file "bzx84b4v7lt1.lib" in the same directory
where your schematic has been saved.
------------------------------------------------------------
Schematic: zdiode_test.asc
Version 4
SHEET 1 1488 1540
WIRE -240 192 -240 128
WIRE -240 320 -240 272
WIRE -160 128 -240 128
WIRE 16 128 -160 128
WIRE 160 128 96 128
WIRE 160 192 160 128
WIRE 160 320 160 256
FLAG -240 320 0
FLAG 160 320 0
FLAG -160 128 vp
FLAG 160 128 vz
SYMBOL voltage -240 176 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value PULSE(0 10 5n 5n 5n 1u 2u)
SYMBOL res 0 144 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R1
SYMATTR Value 100
SYMBOL zener 176 256 R180
WINDOW 0 -20 72 Left 0
WINDOW 3 5 -5 Right 0
SYMATTR InstName D1
SYMATTR Value bzx84b4v7lt1
SYMATTR Prefix X
TEXT -248 16 Left 0 !.tran 10u
TEXT -256 -24 Left 0 !.include bzx84b4v7lt1.lib
Model from ONSEMI: bzx84b4v7lt1.lib
.SUBCKT bzx84b4v7lt1 2 1
**************************************
* Model Generated by MODPEX *
*Copyright(c) Symmetry Design Systems*
* All Rights Reserved *
* UNPUBLISHED LICENSED SOFTWARE *
* Contains Proprietary Information *
* Which is The Property of *
* SYMMETRY OR ITS LICENSORS *
*Commercial Use or Resale Restricted *
* by Symmetry License Agreement *
**************************************
* Model generated on Dec 11, 03
* MODEL FORMAT: PSpice
* anode cathode
*node: 2 1
* Forward Section
D1 2 1 MD1
.MODEL MD1 D IS=5.21532e-16 N=1 XTI=1 RS=0.5
+ CJO=1.3e-10 TT=1e-08
* Leakage Current
R 1 2 MDR 1e+07
.MODEL MDR RES TC1=0 TC2=0
* Breakdown
IZG 4 2 0.12
R4 4 2 2000
D3 2 4 MD3
.MODEL MD3 D IS=2.5e-12 N=2.70127 XTI=0 EG=0.1
D2 5 4 MD2
.MODEL MD2 D IS=2.5e-12 N=8.46982 XTI=0 EG=0.1
EV1 1 5 6 0 1
IBV 0 6 0.001
RBV 6 0 MDRBV 1749.5
.MODEL MDRBV RES TC1=-0.000940267
*-- PSpice DIODE MODEL DEFAULT PARAMETER
* VALUES ARE ASSUMED
*IS=1E-14 RS=0 N=1 TT=0 CJO=0
*VJ=1 M=0.5 EG=1.11 XTI=3 FC=0.5
*KF=0 AF=1 BV=inf IBV=1e-3 TNOM=27
.ENDS bzx84b4v7lt1
I am trying a zener diode, but the method should be the same.Ken said:Huh ?????
I use subcircuits to handle the IRF MOSFETs etc. In the schematic, they
look like a MOSFET symbol so the schematic is easy to understand but they,
in fact call out a SUBCKT in the net list. Is this the sort of thing you
are trying to do?
Robert Baer said:.LIB (more familiar with TopSpice) than the .INCLUDE you mentioned.
I am trying a zener diode, but the method should be the same.
[email protected] forging knowledgeKen Smith said:As far as I know, .LIB and .INCLUDE do exactly the same thing in ltspice.
I do something different from the method you are learning. Rather than
confusing things with another set of instructions, I'll come by and check
this thread again in tomorrow to see if you've got it working.
And i did try embedding the .SUBCKT descriptions, but may not have
tried the variant you mentioned on the device itself.
I tried embedding the whole library (it is short) and it does notHelmut said:Hello Robert,
LTspice can handle subcircuits of course.
Maybe you haven't correctly setup your subcircuit or symbol.
There are in general differences between the SPICE varieties
when it comes to parameter passing to subcircuits.
LTspice is mostly compatible to PSPICE regarding parameters.
Why haven't you posted your LTspice schematic and subcircuit?
Now I have to make some guess what you have done wrong.
I have assumed that you try to use Z-diode subcircuit models
from ONSEMI. They provide two models for each Z-diode.
Prefer to use the PSPICE compatible models(.lib) and not the
SPICE3 models(.sp3) from ONSEMI, because SPICE3 has a different
syntax for the model statement of resistors. Normally you don't
have or need .model statements for resistors.
PSPICE:
RBV 6 0 MDRBV 1749.5
.MODEL MDRBV RES TC1=-0.000940267
SPICE3:
RBV 6 0 1749.5 MDRBV
.MODEL MDRBV R TC1=-0.000940267
LTspice allows you to have the tempco in the same line.
RBV 6 0 1749.5 TC1=-0.000940267
I have made an example for you with a Z-diode(4.7V) from ONSEMI.
It is defined with a subcircuit. The only important thing with
the ONSEMI library is to use the PSPICE compatible ".lib"
file and not the SPICE3(.sp3) file.
Save the attached schematic file with name "zdiode_test.asc"
and save the model file as "bzx84b4v7lt1.lib".
Please keep both files in the same directory.
I have also attached a few instructions how to change symbols
which are designed for models so that they can be used for
subcircuits. So you don't have to draw an extra symbol.
Best regards,
Helmut
------ INSTRUCTIONS FOR SUBCIRCUIT( ZENER-)DIODES ------
1. Add a diode to the schematic.
2. Move the cursor over the placed diode.
Press <Ctrl>RightMouseButton
Change Prefix D to X
OK
Now this diode expects a ".SUBCKT ..." definition, because of the X.
3. Change the value D of the diode in your schematic to bzx84b4v7lt1.
4. Place the subcircuit definition in the schematic or load it from a file.
In the ladder case add a ".include bzx84b4v7lt1.lib" to the schematic.
Save the subcircuit definition file "bzx84b4v7lt1.lib" in the same directory
where your schematic has been saved.
------------------------------------------------------------
Schematic: zdiode_test.asc
Version 4
SHEET 1 1488 1540
WIRE -240 192 -240 128
WIRE -240 320 -240 272
WIRE -160 128 -240 128
WIRE 16 128 -160 128
WIRE 160 128 96 128
WIRE 160 192 160 128
WIRE 160 320 160 256
FLAG -240 320 0
FLAG 160 320 0
FLAG -160 128 vp
FLAG 160 128 vz
SYMBOL voltage -240 176 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value PULSE(0 10 5n 5n 5n 1u 2u)
SYMBOL res 0 144 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R1
SYMATTR Value 100
SYMBOL zener 176 256 R180
WINDOW 0 -20 72 Left 0
WINDOW 3 5 -5 Right 0
SYMATTR InstName D1
SYMATTR Value bzx84b4v7lt1
SYMATTR Prefix X
TEXT -248 16 Left 0 !.tran 10u
TEXT -256 -24 Left 0 !.include bzx84b4v7lt1.lib
Model from ONSEMI: bzx84b4v7lt1.lib
.SUBCKT bzx84b4v7lt1 2 1
**************************************
* Model Generated by MODPEX *
*Copyright(c) Symmetry Design Systems*
* All Rights Reserved *
* UNPUBLISHED LICENSED SOFTWARE *
* Contains Proprietary Information *
* Which is The Property of *
* SYMMETRY OR ITS LICENSORS *
*Commercial Use or Resale Restricted *
* by Symmetry License Agreement *
**************************************
* Model generated on Dec 11, 03
* MODEL FORMAT: PSpice
* anode cathode
*node: 2 1
* Forward Section
D1 2 1 MD1
.MODEL MD1 D IS=5.21532e-16 N=1 XTI=1 RS=0.5
+ CJO=1.3e-10 TT=1e-08
* Leakage Current
R 1 2 MDR 1e+07
.MODEL MDR RES TC1=0 TC2=0
* Breakdown
IZG 4 2 0.12
R4 4 2 2000
D3 2 4 MD3
.MODEL MD3 D IS=2.5e-12 N=2.70127 XTI=0 EG=0.1
D2 5 4 MD2
.MODEL MD2 D IS=2.5e-12 N=8.46982 XTI=0 EG=0.1
EV1 1 5 6 0 1
IBV 0 6 0.001
RBV 6 0 MDRBV 1749.5
.MODEL MDRBV RES TC1=-0.000940267
*-- PSpice DIODE MODEL DEFAULT PARAMETER
* VALUES ARE ASSUMED
*IS=1E-14 RS=0 N=1 TT=0 CJO=0
*VJ=1 M=0.5 EG=1.11 XTI=3 FC=0.5
*KF=0 AF=1 BV=inf IBV=1e-3 TNOM=27
.ENDS bzx84b4v7lt1
I tried embedding the whole library (it is short) and it does not work;
error message is "not found".
The bad thing is that line is over 2000 characters long...
However, one could trim the line to have only the first .SUBCKT which i
tried to no avail.
.LIB and .INC also fail exactly the same way.
...
--------- SNIPped for brevity ------
*That* is the magic! A Component Editor!!
Thanks; it works now.
I imported the subcircuit for the part i wanted to study this time
(makes the last line only 346 characters) and then "built" the circuit i
had in mind.
But it seems there may be something wrong with the model, so i added the
"short" you see to "home in" to the problem.
In TopSpice,the maximum temperature that works is 77C; the error message
at higher temperatures is meaningless to a user, only to the original
programmer.
In LTspice, it seems to work to about 105C and at 125C it runs forever
in a Newton-Rapheson(sp?? ) loop, and at 185C the zener voltage is just
plain wrong.
At 135C an error message is generated that may give a clue as to what
the problem in the model may be.
With this info, could you determine what is needed to fix it?
Thanks. Perhaps Diodes Inc gave the wrong value in their model.Helmut said:----- Original Message -----
From: "Robert Baer" <[email protected]>
Newsgroups: sci.electronics.cad
Sent: Wednesday, July 27, 2005 10:31 PM
Subject: Re: SwitcherCad / Pspice SUBCKT calls?
Hello Robert,
The problem has been caused by the low value of N in your diode model.
I assume it results in too large exponent values in the diode
equations used in SPICE. Normal diodes have N=1 to 2 .
Your model.
.MODEL DR D ( IS=5.02f RS=34.5 N=0.223 )
Please change N to at least 0.3.
.MODEL DR D ( IS=5.02f RS=34.5 N=0.3 )
The simulation has been ok with N=0.3 even for Temp=185C.
Best regards,
Helmut
Robert Baer said:Thanks. Perhaps Diodes Inc gave the wrong value in their model.
Is there some electrical testing that could be used to determine N, and
is it relatively constant over current and /or temperature?
Thanks for the good tutorial as how one gets N.Helmut said:Hello Robert,
Let's take a look to the datasheet curve on page 3 of 6 (bottom left).
http://www.diodes.com/products/catalog/search.php
DDZ9694
The model in question is for the diode DR used in Zener-region.
From the datsheet:
-----------------
delta_V = 0.17V, 1u->10m
Let's assume Rs=5Ohm as we see later.
delta_V_internal = 0.12V
Diode equations:
----------------
I1 = Is*exp(V1/(N*Vt))
I2 = Is*exp(V2/(N*Vt))
I2/I1= exp((V2-V1))/(N*Vt))
log(I2/I1)=(V2-V1)/(N*Vt)
N=(V2-V1)/(Vt*log(I2/I1))
Values from datsheet:
V2-V1 = 0.12V, I2/I1=1e4
N = 0.12/(0.025*log(10000))= 0.2/0.025*9.21)
N = 0.5
Rs=.15V/30m = 5Ohm
My guess:
----------------------------------
.MODEL DR D ( IS=5.02f RS=5 N=0.5)
----------------------------------
Sorry, I will not spend more effort into this diode model.
Best regards,
Helmut
The original model:
http://www.diodes.com/products/spicemodels/category.php?category-id=1
*SRC=DDZ9694;DI_DDZ9694;Diodes;Zener <=10V; 8.20V 0.500W Diodes Inc.
zener
*SYM=HZEN
.SUBCKT DI_DDZ9694 1 2
* Terminals A K
D1 1 2 DF
DZ 3 1 DR
VZ 2 3 8.07
.MODEL DF D ( IS=25.1p RS=33.6 N=1.10
+ CJO=47.6p VJ=0.750 M=0.330 TT=50.1n )
.MODEL DR D ( IS=5.02f RS=34.5 N=0.223 )
.ENDS
Robert Baer said:Thanks for the good tutorial as how one gets N.
I will be getting some samples, so i can make measurements as indicated,
and calculate values that match reality and not some fakey datasheet.
It seems that N can indeed change over temperature.
Excellent point, most especially in making measurements above 125C.Helmut said:Hello Robert,
I recommend to use 10uA and 1mA to evaluate N.
Higher current will result in a significant temperature rise
of the diode which may lead to a high measurement error.
Maybe a pulsed measuremet is necessary for higher currents like 10mA.
Best regards,
Helmut
