开云体育

--- In LTspice@..., "ingodettmann <ingod@y...>"
<ingod@y...> wrote:

Hi everbody,

does anyone know, how I can add a noise source in a transient
simulation (if it is possible at all)?
I tried to modell a noise source with a behavioral voltage source
but i didn't work.

Hello Ingo,

there is a very easy way to make such a noise source.
Firstly we should be aware that the rand() funktion has equal
probability for every voltage level between 0 and 1.
This is not like a gaussian noise where you have higher values with
lower probabilty. I remembered a theorem that the generated noise
becomes more gaussian by adding many such noise sources.
I have preferred three sources.

Example:
Digital noise clock is 1e4Hz. "time" is the keyword for time in
the .tran analysis. You can use it in your B-sources.
You have to increase the rand() frequency 1e4 to your requirements.
I think that the offset parameter in the rand() function should be
increased proportionally to the frequency. The intention of this
offset parameter is to make the three rand() functions more like
independant noise sources.

Best Regards
Helmut


Example; f=1.0e4

B1: V=2*rand(time*1e4)
B2: V=2*rand(time*1e4+0.0911e4)
B3: V=2*rand(time*1e4+0.2131e4)

.tran 0 100m 0 10u


Example; f=1.0e9

B1: V=2*rand(time*10e9)
B2: V=2*rand(time*10e9+0.0911e9)
B3: V=2*rand(time*10e9+0.2131e9)

.tran 0 1u 0 0.1n


netlist
-------

*
B1 N001 0 V=2*rand(time*1e9+0.2131e9)
B2 N002 N001 V=2*rand(time*1e9+0.0911e9)
B3 N003 N002 V=2*rand(time*1e9)
R1 N003 out 50
C1 out 0 1p
.tran 0 1u 0 0.1n
.backanno
.end


Schematic
---------

SHEET 1 912 712
WIRE 192 80 192 32
WIRE 192 208 192 160
WIRE 192 -96 192 -48
WIRE 192 -176 192 -224
WIRE 192 -224 464 -224
WIRE 544 -224 576 -224
WIRE 576 -224 576 -192
WIRE 576 -128 576 -96
FLAG 192 208 GND
FLAG 576 -96 0
FLAG 576 -224 out
SYMBOL BV 192 64 R0
SYMATTR InstName B1
SYMATTR Value V=2*rand(time*1e9+0.2131e9)
SYMBOL bv 192 -64 R0
SYMATTR InstName B2
SYMATTR Value V=2*rand(time*1e9+0.0911e9)
SYMBOL bv 192 -192 R0
SYMATTR InstName B3
SYMATTR Value V=2*rand(time*1e9)
SYMBOL res 448 -208 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R1
SYMATTR Value 50
SYMBOL cap 560 -192 R0
SYMATTR InstName C1
SYMATTR Value 1p
TEXT 192 -256 Left 0 !.tran 0 1u 0 0.1n

--- In LTspice@..., <Bernhard_Kraemer@w...> wrote:

Hello,

After a re-install of my system, I downloaded the newest edition of
LTSpice. Now I tried out to simulate a simple circuit, and I

discovered that whatever it is, my circuit works well, but with the >
STEP command I get the error :

Multiple instances of "Cjo=1.0760e-12".

Hello Bernhard,

Cjo is normally a parameter of a semiconductor device. It seems
you have any such device in your circuit, but your posted netlist
doesn't show it.

What could this possibly be? What could I do to solve the problem?
Here my short circuit:

Kondensatorme?bruecke

*Widerst?nde

R1 2 0 1K
R2 3 0 {var}

*Kondensatoren

C1 1 2 1u
Cubk 1 3 2u

*Strom- und Spannungsquellen

Vsin 1 0 SIN(0 5 200)

.PARAM var=1K

** Analysis setup **
.OP
.STEP LIN PARAM var 1 10K 1K <<<< This Line gives the error!
.tran 50us 50m

.END

I have tried your circuit with with LTSpice version 2.00k
and it has been simulated without any error. Firstly I used the
schematic editor to enter the circuit. Then I tried your text version
also sucessfully.
When I look to my netlists they are eactly the same like yours.

Which version of LTSpice are you using?
Please try the latest 2.00k.
If you really use already 2.00k, then feel free to send me your
original .asc file and/or your netlist file for further investigation.


Best Regards
Helmut

HelmutSennewald@...



Textversion:
-------------

*Kondensatorme?bruecke
*Widerst?nde

R1 2 0 1K
R2 3 0 {var}

*Kondensatoren

C1 1 2 1u
Cubk 1 3 2u

*Strom- und Spannungsquellen

Vsin 1 0 SIN(0 5 200)

.PARAM var=1K

** Analysis setup **
.OP
.STEP LIN PARAM var 1 10K 1K
.tran 50u 50m

.END


From schematic version:
-----------------------

*
R1 2 0 1k
R2 3 0 {var}
Cubk 1 3 2?
C1 1 2 1?
Vsin 1 0 SINE(0 5 200)
.PARAM var=1K
.STEP LIN PARAM var 1 10K 1K
.tran 50us 50m
.backanno
.end

Hello,

After a re-install of my system, I downloaded the newest edition of LTSpice. Now I tried out to simulate a simple circuit, and I discovered that whatever it is, my circuit works well, but with the STEP command I get the error :

Multiple instances of "Cjo=1.0760e-12".

What could this possibly be? What could I do to solve the problem?
Here my short circuit:

Kondensatorme?bruecke

*Widerst?nde

R1 2 0 1K
R2 3 0 {var}

*Kondensatoren

C1 1 2 1u
Cubk 1 3 2u

*Strom- und Spannungsquellen

Vsin 1 0 SIN(0 5 200)

.PARAM var=1K

** Analysis setup **
.OP
.STEP LIN PARAM var 1 10K 1K <<<< This Line gives the error!
.tran 50us 50m

.END



Greetings,

Bernhard Kr?mer
______________________________________________________________________________
Werden Sie kreativ! Jetzt HTML-Mails nicht nur schreiben - nein -
GESTALTEN, bei WEB.DE FreeMail!

You can run them if they're defined with, e.g.,
PSpice subcircuits. Latter versions of LTspice
comes with documenation about making symbols
for 3rd party devices.

--Mike

--- "polapart <sahawley@...>" <sahawley@...>
wrote:

Is there a simple way to convert TI models to run in
LTSpice?

__________________________________________________
Do you Yahoo!?
Yahoo! Mail Plus - Powerful. Affordable. Sign up now.

You might be able to use the rand() function
to get what you're looking for. Check the
example ./LTC/SwCADIII/examples/Educational/PLL.asc
There it is used to generate a random bit stream
by boolean comparison to 0.5.

--Mike
--- "ingodettmann
<ingod@...>"
<ingod@...> wrote:

Hi everbody,

does anyone know, how I can add a noise source in a
transient
simulation (if it is possible at all)?
I tried to modell a noise source with a behavioral
voltage source
but i didn't work.

Thanks,

Ingo

__________________________________________________
Do you Yahoo!?
Yahoo! Mail Plus - Powerful. Affordable. Sign up now.

Is there a simple way to convert TI models to run in LTSpice?

Hi everbody,

does anyone know, how I can add a noise source in a transient
simulation (if it is possible at all)?
I tried to modell a noise source with a behavioral voltage source
but i didn't work.

Thanks,

Ingo

Michel,

I experienced the following problem using a lossy
transmission line. Even though the simulation (.op)
can proceed, a non fatal error is occuring all the
time: Unknown parameter "td". As I read in the
online help Td is not a parameter of a lossy
transmission line. So I wonder wy this problem is
occuring.

I think this as a problem in the definition of the
lossy T-line symbol. Try updating to 2.00c and
possibly redrafting the schematic.

Also, I haven't f find in the help a clear procedure
explaining where to insert the value of the
parameters of a complex model like a transmission
line. After a few try, I have created a spice
directive like the folowing : " model neg_terre_1
LTRA(R=9.6 G=122 L=0 C=0 len=10000) " and it
worked.

Congratuations. Yes, this is an aspect of the help
documentation that still needs improvement.

Finnally, I want to extract the numbers appearing at
the end of the .raw file. Can you tell me the format
of this string?

Helmut Sennewald wrote a utility to extract this
data. I think a released version is availible in
this group's files.

Best Regards,

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Mail Plus - Powerful. Affordable. Sign up now.

I experienced the following problem using a lossy transmission line. Even though the simulation (.op) can proceed, a non fatal error is occuring all the time: Unknown parameter "td". As I read in the online help Td is not a parameter of a lossy transmission line. So I wonder wy this problem is occuring.


Also, I haven't f find in the help a clear procedure explaining where to insert the value of the parameters of a complex model like a transmission line. After a few try, I have created a spice directive like the folowing : " model neg_terre_1 LTRA(R=9.6? G=122? L=0 C=0 len=10000) " and it worked.


Finnally, I want to extract the numbers appearing at the end of the .raw file. Can you tell me the format of this string?

Thanking you in advance for your reply


Michel Allaire ing.

SSTM
Société de Transport de Montréal
Soutien opérationnel


Courriel : michel.allaire@...
Téléphone : (514) 280-6335
Télécopie : (514) 280-5677
Tél. privé : 6301

Version 2.00 of LTspice/SwitcherCAD III is now
available. From Version 1.16s, this version
introduces

1. a graphical symbol editor
2. hierarchical schematics
3. improved help documentation.

The schematic file format changed a little, but
2.00 should be able to read the old schematics
and symbols.

I'm particularly interested in feedback relating to
(i) things that are now broken and ii) sections
of the help that don't tell you how to do something.

Best Regards,

Mike Engelhardt

__________________________________________________
Do you Yahoo!?
Yahoo! Mail Plus - Powerful. Affordable. Sign up now.

The line

"SYMATTR Prefix MP"

should read

"SYMATTR Prefix X"

in order for the symbol to be used with a subcircuit
definition. See Helmult's notes on the subject.

--Mike

--- "Dale <dchishol@...>"
<dchishol@...> wrote:

Quick Hints (Check this post carefully; NOT
GUARANTEED ERROR FREE):
(Wife is waiting in parking lot to tell me her NEXT
husband will
always leave work on time . . . )

The On Semi file is a SUBCIRCUIT model (of a MOSFET,
plus some
corrections for its non-idealness as well as package
parasitics, etc)
while the "STANDARD.MOS" file is a database of
parameters for MOS
DEVICE models. It's certainly confusing and perhaps
unfortunate that
MOSFETS (in particular) are commonly modeled by both
methods, but
that's how it is. What REALLY tripped you up is
when the subcircuit
model builder chose to call a resistor "Rg" which is
the same name as
a parameter in the MOS device model. (He should
have stuck with
something like "R101" and let us guess what it's
role is.)

You probably want to copy the On Semi file to the "
.&#92;LIB&#92;SUB&#92;"
directory and call it something like
"ntmd6p02r2.sub". (If you have
a bunch of these files, you might creat a
sub-directory
called ".&#92;LIB&#92;SUB&#92;ON_SEMI&#92;" to hold them; or
concatenate them into a
largeer file called "ON_SEMI_MOSFET.LIB")

Next make a symbol file that references this model,
perhaps
called ".&#92;lib&#92;sym&#92;PowerMOS&#92;ntmd6p02r2.asy". Do this
with the symbol
editor in LTSpice, or copy the following:

Version 3
SymbolType CELL
LINE Normal 12 12 12 24
LINE Normal 4 20 12 20
LINE Normal 4 12 6 12
LINE Normal 12 12 6 11
LINE Normal 12 12 6 13
LINE Normal 6 11 6 13
LINE Normal 4 2 4 6
LINE Normal 4 10 4 14
LINE Normal 4 18 4 22
LINE Normal 0 20 2 20
LINE Normal 2 4 2 20
LINE Normal 12 4 4 4
LINE Normal 12 0 12 4
WINDOW 0 14 8 Left 0
WINDOW 3 14 18 Left 0
SYMATTR Prefix MP
SYMATTR SpiceModel NTMD6P02R2.SUB
SYMATTR Value NTMD6P02R2
SYMATTR SpiceLine *
SYMATTR SpiceLine2 *
SYMATTR Description P-MOSFET 20V, 6A
PIN 0 20 NONE 0
PINATTR PinName G
PINATTR SpiceOrder 2
PIN 12 0 NONE 0
PINATTR PinName D
PINATTR SpiceOrder 1
PIN 12 24 NONE 0
PINATTR PinName S
PINATTR SpiceOrder 3

Close and re-start LTSpice. You should be able to
find the symbol
you just created in the component selection menu,
and it should point
to your subcircuit model file when you simulate.

(You can probably figure out most of this by poking
around in the
LTSpice "HELP" files for a while, but it's not
explained very
clearly. Note that both the model file and the
symbol file are
straight ASCII and can be attacked with your
favorite text editor,
but you'll have to re-start LTSpice to pick up the
changes so you
might as well use the LTSpice editor.

The newsgroups at
<
8&oe=UTF-8&group=sci.electronics.cad> and

<

8&group=sci.electronics.design> are good sources of
info on LTSpice:
Mike Englehardt (author of LTSpice) checks them
regularly. Search
them with "LTSpice" as a keyword & you'll probably
find a discussion
on this very question!)

Dale


--- In LTspice@..., "ravton
<ravton@y...>" <ravton@y...>
wrote:

I've only been using LTSpice for a couple of weeks

and have finally

gotten stuck. I'm trying to import some

additional MOSFET models

(for example,

)

and am at a loss on how to do it.

I've waded through the online manuals and googled

forever. I tried

just copying values from the PSpice model into the

standard.mos

file but it's not clear what to copy.

For example, in standard.mos the first parameter

is "Rg". The

manual states that "Rg" is "Gate ohmic

resistance". But in the

PSPice model the only line with Rg is "RG 2 7

10.013". Now since

every other line in the standard.mos file has Rg=3

I'm totally

confused on how to proceed.

Can anyone provide any hints of guidance on how to

import these?

Thanks!

__________________________________________________
Do you Yahoo!?
Yahoo! Mail Plus - Powerful. Affordable. Sign up now.

Ralph,

Pardon my ignorance as I am a Ham running small
spice circuits, but I
cant find any documentation on what the dot
command, .backanno, means.
I would appreciate a pointer to the documentation
for this command.

.backanno directs LTspice to embed port information
in the .raw file so that the waveform viewer can
refer to subcircuit port currents by pin name. The
command is placed in every netlist generated by the
netlister. It lets you plot a pin current by
pointing at the symbol's pin. You can ignore that
fact it's in the netlist. It has no meaning to
other spice programs.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Mail Plus - Powerful. Affordable. Sign up now.

Hi,
Pardon my ignorance as I am a Ham running small spice circuits, but I cant find any documentation on what the dot command, .backanno, means. I would appreciate a pointer to the documentation for this command.
Ralph
KB9KKR

PS: It's rumored that most of what the subcircuit models attempt to
do can be done by specifying parameters in the higher-level MOS
models (the "LEVEL=__" parameter) but I haven't found any
documentation or explanation of how to do it.

Dale

Quick Hints (Check this post carefully; NOT GUARANTEED ERROR FREE):
(Wife is waiting in parking lot to tell me her NEXT husband will
always leave work on time . . . )

The On Semi file is a SUBCIRCUIT model (of a MOSFET, plus some
corrections for its non-idealness as well as package parasitics, etc)
while the "STANDARD.MOS" file is a database of parameters for MOS
DEVICE models. It's certainly confusing and perhaps unfortunate that
MOSFETS (in particular) are commonly modeled by both methods, but
that's how it is. What REALLY tripped you up is when the subcircuit
model builder chose to call a resistor "Rg" which is the same name as
a parameter in the MOS device model. (He should have stuck with
something like "R101" and let us guess what it's role is.)

You probably want to copy the On Semi file to the " .&#92;LIB&#92;SUB&#92;"
directory and call it something like "ntmd6p02r2.sub". (If you have
a bunch of these files, you might creat a sub-directory
called ".&#92;LIB&#92;SUB&#92;ON_SEMI&#92;" to hold them; or concatenate them into a
largeer file called "ON_SEMI_MOSFET.LIB")

Next make a symbol file that references this model, perhaps
called ".&#92;lib&#92;sym&#92;PowerMOS&#92;ntmd6p02r2.asy". Do this with the symbol
editor in LTSpice, or copy the following:

Version 3
SymbolType CELL
LINE Normal 12 12 12 24
LINE Normal 4 20 12 20
LINE Normal 4 12 6 12
LINE Normal 12 12 6 11
LINE Normal 12 12 6 13
LINE Normal 6 11 6 13
LINE Normal 4 2 4 6
LINE Normal 4 10 4 14
LINE Normal 4 18 4 22
LINE Normal 0 20 2 20
LINE Normal 2 4 2 20
LINE Normal 12 4 4 4
LINE Normal 12 0 12 4
WINDOW 0 14 8 Left 0
WINDOW 3 14 18 Left 0
SYMATTR Prefix MP
SYMATTR SpiceModel NTMD6P02R2.SUB
SYMATTR Value NTMD6P02R2
SYMATTR SpiceLine *
SYMATTR SpiceLine2 *
SYMATTR Description P-MOSFET 20V, 6A
PIN 0 20 NONE 0
PINATTR PinName G
PINATTR SpiceOrder 2
PIN 12 0 NONE 0
PINATTR PinName D
PINATTR SpiceOrder 1
PIN 12 24 NONE 0
PINATTR PinName S
PINATTR SpiceOrder 3

Close and re-start LTSpice. You should be able to find the symbol
you just created in the component selection menu, and it should point
to your subcircuit model file when you simulate.

(You can probably figure out most of this by poking around in the
LTSpice "HELP" files for a while, but it's not explained very
clearly. Note that both the model file and the symbol file are
straight ASCII and can be attacked with your favorite text editor,
but you'll have to re-start LTSpice to pick up the changes so you
might as well use the LTSpice editor.

The newsgroups at <
8&oe=UTF-8&group=sci.electronics.cad> and
<
8&group=sci.electronics.design> are good sources of info on LTSpice:
Mike Englehardt (author of LTSpice) checks them regularly. Search
them with "LTSpice" as a keyword & you'll probably find a discussion
on this very question!)

Dale


--- In LTspice@..., "ravton <ravton@y...>" <ravton@y...>
wrote:

I've only been using LTSpice for a couple of weeks and have finally
gotten stuck. I'm trying to import some additional MOSFET models
(for example, )
and am at a loss on how to do it.

I've waded through the online manuals and googled forever. I tried
just copying values from the PSpice model into the standard.mos
file but it's not clear what to copy.

For example, in standard.mos the first parameter is "Rg". The
manual states that "Rg" is "Gate ohmic resistance". But in the
PSPice model the only line with Rg is "RG 2 7 10.013". Now since
every other line in the standard.mos file has Rg=3 I'm totally
confused on how to proceed.

Can anyone provide any hints of guidance on how to import these?

Thanks!

--- In LTspice@..., "ravton <ravton@y...>" <ravton@y...>
wrote:

I've only been using LTSpice for a couple of weeks and have finally
gotten stuck. I'm trying to import some additional MOSFET models
(for example, )
and am at a loss on how to do it.

I've waded through the online manuals and googled forever. I tried
just copying values from the PSpice model into the standard.mos

file

but it's not clear what to copy.

For example, in standard.mos the first parameter is "Rg". The

manual

states that "Rg" is "Gate ohmic resistance". But in the PSpice

model

the only line with Rg is "RG 2 7 10.013". Now since every other

line

in the standard.mos file has Rg=3 I'm totally confused on how to
proceed.

Can anyone provide any hints of guidance on how to import these?

Hello ravton,
the provided model is a subcircuit. You can make a symbol like you
would do it for a specific opamp.
Another option is to use a more generalized symbol like my x-models.
I have uploaded these x-models this evening to this group's
files/library menues. There is also a help file there.
Anyway I will send you an example with your model directly.
If you still have problems with it, let me know.

Best Regards
Helmut

I've only been using LTSpice for a couple of weeks and have finally
gotten stuck. I'm trying to import some additional MOSFET models
(for example, )
and am at a loss on how to do it.

I've waded through the online manuals and googled forever. I tried
just copying values from the PSpice model into the standard.mos file
but it's not clear what to copy.

For example, in standard.mos the first parameter is "Rg". The manual
states that "Rg" is "Gate ohmic resistance". But in the PSpice model
the only line with Rg is "RG 2 7 10.013". Now since every other line
in the standard.mos file has Rg=3 I'm totally confused on how to
proceed.

Can anyone provide any hints of guidance on how to import these?

Thanks!

Hello,
I have written a utilty program that makes the LTSpice program
even more useful.

The features are:

1.
Merge as many raw files you want into one raw file.
The advantage is that you can have different simulations in one graph.

2.
Extract data to your spreadsheet or favorite graph program.
You select the signals you want ang get a column based output.

3.
Equalize time steps of .TRAN simulation.
Normally you have never exact the time steps you want in a raw file.
This can become necessary if you want export data to other programs.

These are the most important functions of the program.

If you ever have experienced different simulations in one plot or
easy exporting data to another graphic program, you will be impressed.

I hope that in some future time, all these features are implented in
LTSpice.

Thanks to Mike Engelhardt for the great LTSpice and the support.

Enjoy the program!

Helmut

Helmut Sennewald wrote:

Hello Mike,
sorry for the late response, but I am more in open
newsgroups until now. There I often help people
starting with LTspice.

Hi .. thanks for the reply! Which newsgroup do you suggest?
I only went for the yahoo list because the LTspiceman
pointed me towards it.

If you still have problem with that MAX931 model, then
let me know and I will do it as an example for you.

That's very kind of you, I may take you up on that.
(For now, I've switched to an LT device.)

Mike

--- Mike Cowlishaw <mfcowli@...> schrieb: >
Ralph R. Reinhold wrote:

Mike
It looks like you may have not included a ".lib"

command line in the

schematic.

OK, will investigate ... thanks! Though I think it
is finding the file OK,
because it complained when I had the wrong number of
parameters on the
.subckt statement.

Mike Cowlishaw

Hello Mike,
sorry for the late response, but I am more in open
newsgroups until now. There I often help people
starting with LTspice.

If you still have problem with that MAX931 model, then
let me know and I will do it as an example for you.

Best Regards
Helmut

__________________________________________________________________

Gesendet von Yahoo! Mail -
Weihnachts-Einkufe ohne Stress!