开云体育

--- In LTspice@..., "David Pariseau"
<david.pariseau@s...> wrote:

Hello Dave,
this model from Fairchild has 4 pins. Please add a 4th pin to

your

symbol. You can see that requirement in the model file. I tried
this with success.

*20=DRAIN 10=GATE 30=SOURCE 50=VTEMP
.SUBCKT FDN304p 20 10 30 50

That's weird, the part is in an SOT-3 package w/ only 3 pins,
but it seems that the 4th input is temperature???

It has been also necessary to add a resistor to this additionally
node in the schematic. I connected a 1k resistor to ground in my
test circuit. This works at least for circuits where the drain is
connected to >=0V.

I added this and commented out the Diode line and there are no

errors

now in simulation, but the simulation is glacially slow and I'm not
sure correct.

Hello David,
you can send me your circuit file(s) for testing.
Please use the following e-mail address if you are interested.
HelmutSennewald@...

Best Regards
Helmut

Hello Dave,
this model from Fairchild has 4 pins. Please add a 4th pin to your
symbol. You can see that requirement in the model file. I tried
this with success.

*20=DRAIN 10=GATE 30=SOURCE 50=VTEMP
.SUBCKT FDN304p 20 10 30 50

That's weird, the part is in an SOT-3 package w/ only 3 pins,
but it seems that the 4th input is temperature???

It has been also necessary to add a resistor to this additionally
node in the schematic. I connected a 1k resistor to ground in my
test circuit. This works at least for circuits where the drain is
connected to >=0V.

I added this and commented out the Diode line and there are no errors
now in simulation, but the simulation is glacially slow and I'm not
sure correct.

Thanks for the input, Helmut,
Dave Pariseau.

--- In LTspice@..., "David Pariseau"
<david.pariseau@s...> wrote:

I've read through past messages, the SwCAD help
and such and attempted to add a 3rd party model
for the FDN304P. It seems to find the model fine
now, but I get the error "Too few parameters for
subcircuit type "fdn304p"".

I basically dropped the model file into the &#92;sub
directory, copied the pmos symbol file and changed
it to specify the FDN304p model.

Hello Dave,
this model from Fairchild has 4 pins. Please add a 4th pin to your
symbol. You can see that requirement in the model file. I tried this
with success.

*20=DRAIN 10=GATE 30=SOURCE 50=VTEMP
.SUBCKT FDN304p 20 10 30 50

It has been also necessary to add a resistor to this additionally
node in the schematic. I connected a 1k resistor to ground in my test
circuit. This works at least for circuits where the drain is
connected to >=0V.

Fairchilds fault?
The model has a badly designed breakdown section.
It shorts the drain if it is below zero volt relative to ground. So
it is unusable in this case. If you have a need for this then you can
comment the line with the diode D.

*D DB1 20 DBLK

Now it will run with a voltage below 0V too, but the breakdown is no
more modelled.

Original section:
*DIODE THERMO BREAKDOWN SECTION
EBL VB1 VB2 101 0 0.8
VBLK VB2 0 20
D DB1 20 DBLK
.MODEL DBLK D(IS=1E-14 CJO=.1p RS=.1)
EDB 0 DB1 VB1 0 1



Hello Mike or whoever exactly knows about,
if a model uses the node number 0, is it then referenced to the
common ground 0 of the top schematic or is this a floating node like
any other node inside the subcircuit?

Best Regards
Helmut

--- In LTspice@..., "Reinier Gerritsen" <r.gerritsen@c...>
wrote:

SNIP

- a way to store multiple analysis commands. If I use .tran and .ac
commands, only the parameters of the last one is saved, the other

gets lost

on exit of the program.

Thanks for you great software and support.

Reinier Gerritsen
The Netherlands

Hoi Reinier,

It is possible to save multiple analysis commands. First place a
simulation command on the sheet. When you add a second simulation
command with Simulate -> Edit Simulation Command (or right mouse
button -> Edit Simulation Command), and place the command on the
sheet, you'll see the "." in the first comman will change to ";".
E.g. you'll get:

.tran 10n
;ac dec 51 100 10G
;dc temp -40 125 2

If you save this schematic, and reopen it, you can choose using
Simulate -> Edit Simulation Command (or right mouse button -> Edit
Simulation Command).
It only works for different analysis types. I.e. you can't choose
between e.g. multiple .tran commands (however you can uncomment them).
Of course you can place these lines on the schematic manually.

Regards,

Ronnie (Also from the Netherlands :-) )

I've read through past messages, the SwCAD help
and such and attempted to add a 3rd party model
for the FDN304P. It seems to find the model fine
now, but I get the error "Too few parameters for
subcircuit type "fdn304p"".

I basically dropped the model file into the &#92;sub
directory, copied the pmos symbol file and changed
it to specify the FDN304p model.

Any thoughts?
Dave Pariseau.

Here are the files:

FDN304p.asy
-------------
Version 4
SymbolType CELL
LINE Normal 48 48 48 96
LINE Normal 16 80 48 80
LINE Normal 16 48 24 48
LINE Normal 48 48 24 44
LINE Normal 48 48 24 52
LINE Normal 24 44 24 52
LINE Normal 16 8 16 24
LINE Normal 16 40 16 56
LINE Normal 16 72 16 88
LINE Normal 0 80 8 80
LINE Normal 8 16 8 80
LINE Normal 48 16 16 16
LINE Normal 48 0 48 16
WINDOW 0 56 32 Left 0
WINDOW 3 56 72 Left 0
SYMATTR Value FDN304P
SYMATTR Prefix X
SYMATTR SpiceModel FDN304P.mod
SYMATTR Value2 FDN304P
SYMATTR Description P-Channel MOSFET transistor
PIN 48 0 NONE 0
PINATTR PinName D
PINATTR SpiceOrder 1
PIN 0 80 NONE 0
PINATTR PinName G
PINATTR SpiceOrder 2
PIN 48 96 NONE 0
PINATTR PinName S
PINATTR SpiceOrder 3

FDN304p.mod
---------------
*FDN304P at Temp. Electrical Model (T2)
*-------------------------------------
.SUBCKT FDN304p 20 10 30 50
*20=DRAIN 10=GATE 30=SOURCE 50=VTEMP
Rg 10 11x 1
Rdu 12x 1 1u
M1 2 1 4x 4x DMOS L=1u W=1u
.MODEL DMOS PMOS(VTO=-0.87 KP=2.5E+1
+THETA=0.25 VMAX=8.5E5 LEVEL=3)
Cgs 1 5x 1300p
Rd 20 4 7E-3
Dds 4 5x DDS
.MODEL DDS D(M=4.26E-1 VJ=3.39E-1 CJO=562p)
Dbody 20 5x DBODY
.MODEL DBODY D(IS=3.81E-10 N=1.145283 RS=0.00084 TT=14.5n)
Ra 4 2 7E-3
Rs 5x 5 0.5m
Ls 5 30 0.5n
M2 1 8 6 6 INTER
E2 8 6 4 1 2
.MODEL INTER PMOS(VTO=0 KP=10 LEVEL=1)
Cgdmax 7 4 1050p
Rcgd 7 4 10meg
Dgd 4 6 DGD
Rdgd 4 6 10meg
.MODEL DGD D(M=3.2E-1 VJ=4.23E-3 CJO=1050p)
M3 7 9 1 1 INTER
E3 9 1 4 1 -2
*ZX SECTION
EOUT 4x 6x poly(2) (1x,0) (3x,0) 0 0 0 0 1
FCOPY 0 3x VSENSE 1
RIN 1x 0 1G
VSENSE 6x 5x 0
RREF 3x 0 10m
*TEMP SECTION
ED 101 0 VALUE {V(50,100)}
VAMB 100 0 25
EKP 1x 0 101 0 .012
*VTO SECTION
EVTO 102 0 101 0 .0007
EVT 11x 12x 102 0 1
*DIODE THERMO BREAKDOWN SECTION
EBL VB1 VB2 101 0 0.8
VBLK VB2 0 20
D DB1 20 DBLK
.MODEL DBLK D(IS=1E-14 CJO=.1p RS=.1)
EDB 0 DB1 VB1 0 1
.ENDS FDN304p
*FDN304P (Rev.A) 12/4/00 **ST

First let me congratulate the author(s) and those that support this
software. It is really useful and easy to use. My daughter, who is
an engineeing sophmore, has even started to use LTSpice for some
labs.

I am looking for a way to either pass plot scales from a dot
statement (.PLOT or .VIEW kind of thing) or at least to freeze the
plot scales from run to run. It would be helpful when trying to
visually compare the the results between runs if the the plot did
not automatically rescale. It would also be nice to be able to have
an alias type statement to save reentering things like V(out)/V(in)
or V(N003, N006)/I(R7).

Again, thank you for the software and thanks to Linear Tech for
their part in this.

Thanks for the quick reply. I figured there had to be a way to do
this. I will give it a whirl.

--Brent

On Mon, 24 Mar 2003 15:43:54 -0800, you wrote:

On Mon, 24 Mar 2003 14:59:23 -0800 (PST), you wrote:

I put up a version of LTspice today with a
new feature. There's a new symbol attribute
called ModelFile. This lets you specify a
file to include as a library file whenever
this symbol is included. However, the symbol
is still edit-able. This let's you enter
parameters to pass to the subcircuit.
<snip>
Let me know if you find these things useful.

Yes! I'll be using it immediately. Thanks!

Jon

Okay, tried it and like it.

Originally, when I started using LT Spice, I wanted to add a new
symbol for the PUJT type of device. You gave me an example of
this which went a very long way in teaching me about using spice
(I was, and still largely am a neophyte in nearly every sense of
that.) This new feature you've added allowed me to create a
PUJT.LIB file and link it to the symbol (.asy) which you made
for me back in January. Now LT Spice naturally finds the model
without me having to specifically write a .include for it.
Thanks.

In the above case, it would be nice if LT Spice would put a
"Select Subcircuit" button on the dialog box which comes up when
I right-click on the symbol (if the .ASY symbol is an X type)
and provide me a list of .SUBCKT entries it found in the
specified library file. In that case, the PUJT.LIB case, this
means it would pop up 2N6027 and 2N6028, for example, and offer
those as options.

I haven't used spice enough to apprehend the implications of
doing that, but it's a suggestion which pops into my mind given
my limited use, to date.

Anyway, thanks much!

Jon

...But I need to model the time dependence of these
devices as the temperature is ramped. Is there any
way to specify a resistor value that is dependent
on the simulation time.

There's an undocumented means to do this. You might
have convergence trouble with it, especially if you
put it inside a feedback loop. Here's a resistance
that varies as the sine of time:

* arbitrary resistor -- even goes negative
R1 1 0 1K R=sin(time) ; the 1K is a dummy value
I1 0 1 1m
.tran 10
.end

The 1K "value" of the Resistor is there to bypass
the error message that the resistance must not be
zero. This value is not used when you use
R=<expression> syntax(I never thought of this
condition when I added the message so I'll get
rid of this error message when an expression is
used.)

One other caveat I would like to bring up is that
there are no time step size checks caused by this
resistance expression, so you may have to stipulate
a max time step when you use this construction.

Good luck with that critter. I thought it might
be useful when I wrote it but never really had
any use for it myself. Let me know if you find
something that needs fixing regarding this.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!

I just started using LTSPice a few weeks ago to model semi-insulating
electro-optic devices as RC-mesh/networks. It works great... But I
need to model the time dependence of theses devices as the
temperature is ramped. Is there any way to specify a resistor value
that is dependent on the simulation time. I know you can specify a
voltage that is dependent on simulation time by using the PULSE
command, or an behavioral voltage source using a mathmatical
expression with the variable "time". Can you specify a resistor
value that is a fuction of simulation time in a similar manner? If
not, is there any other way to accomplish this?

On Mon, 24 Mar 2003 14:59:23 -0800 (PST), you wrote:

I put up a version of LTspice today with a
new feature. There's a new symbol attribute
called ModelFile. This lets you specify a
file to include as a library file whenever
this symbol is included. However, the symbol
is still edit-able. This let's you enter
parameters to pass to the subcircuit.
<snip>
Let me know if you find these things useful.

Yes! I'll be using it immediately. Thanks!

Jon

I put up a version of LTspice today with a
new feature. There's a new symbol attribute
called ModelFile. This lets you specify a
file to include as a library file whenever
this symbol is included. However, the symbol
is still edit-able. This let's you enter
parameters to pass to the subcircuit.

There's two example symbols of the use of
these feature included, 1pole.asy and
2pole.asy in the opamp directory. These
are somewhat ideal opamps with allow the
following parameters to be entered to
model a specific opamp:

Avol open loop DC gain.
GBW open loop gain-bandwidth product
Slew slew rate
Ilimit output current limit
rail how close output can get to the rail
Vos input offset voltage
en equiv. input voltage noise
enk equiv. input voltage noise corner freq
in equiv. input current noise
ink equiv. input current noise corner freq

The model draws all current from the voltage
supplies and has a signal internal node.
Output stage emitter followers are set to 100
Ohms, but you can change that if you need a
more ideal opamp.

The 2pole version has two internal nodes and
an additional parameter, phimargin, which
specifies the 2nd pole in terms of the (approx
-imate) phase margin in degrees.

Input bias, input common mode range and PSRR
are not modeled.

Let me know if you find these things useful.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!

--- In LTspice@..., "john_oztek" <joconnor@o...> wrote:

Also, is there a way to selectively export plot data? It would be
really nice to be able to bring particular traces into Mathcad, for
example, for more detailed analysis. It would also be very
beneficial to be able to e-mail data to plot a few traces.

Hello John,
you can use the program "ltsputil.exe" program to export selectively
nodes of your circuit. The output is in a tabular form which can be
used directly with hopefully all of the math and graphic programs.
It is in the download area of this group. Path: Files->Util

Best Regards
Helmut

Use the .save command to list those nodes and voltages
that you wish...

--Mike

Mike,

Thanks for the quick response! I'll give that a try.

- John

Use the .SAVE command option, also in the tools control panel the
compression option can be set to ASCII data file which can parse by
Mathcad with a lot of effort.

--- In LTspice@..., "john_oztek" <joconnor@o...> wrote:

Is there any way to limit the number of voltages and currents that
are saved during a transient analysis? Over the weekend I ran a
simulation of a poly-phase voltage regulator. The resulting data
file was nearly 5G! It took about 20 minutes this morning just to
load up 7 or 8 traces to view. I've noticed that the time to load

a

trace grows with the number of nodes, not just the simulation

period,

so I'm thinking that I could save a lot of time if I could be
selective about what data I save.

Also, is there a way to selectively export plot data? It would be
really nice to be able to bring particular traces into Mathcad, for
example, for more detailed analysis. It would also be very
beneficial to be able to e-mail data to plot a few traces.

Thanks,
John

Is there any way to limit the number of voltages and
currents that are saved during a transient analysis?
[...]

Use the .save command to list those nodes and voltages
that you wish. If there is no .save command, then it
saves the defaults, which you can set in
Tools=>Control
Panel=>Save Defaults.(That's where you tell it to save
subcircuit nodes and device currents if you wish).

Also of interest might be the special .save keyword
of "dialogbox". For example, the syntax

".save V(in) V(out) dialogbox"

will throw up a dialog box at the start of simulation
of nodes and currents to save. V(in) and V(out) will
be selected and you can select other quantities by
clicking on the nodes/devices in the schematic.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!

Is there any way to limit the number of voltages and currents that
are saved during a transient analysis? Over the weekend I ran a
simulation of a poly-phase voltage regulator. The resulting data
file was nearly 5G! It took about 20 minutes this morning just to
load up 7 or 8 traces to view. I've noticed that the time to load a
trace grows with the number of nodes, not just the simulation period,
so I'm thinking that I could save a lot of time if I could be
selective about what data I save.

Also, is there a way to selectively export plot data? It would be
really nice to be able to bring particular traces into Mathcad, for
example, for more detailed analysis. It would also be very
beneficial to be able to e-mail data to plot a few traces.

Thanks,
John

--- In LTspice@..., Panama Mike <panamatex@y...> wrote:

Dale wrote:

Mike, this sounds like something I'd like to
dissuade you from.

Helmult wrote:
I fully agree with you. The biggest advantage
of all the opamp models
[...]
The provided SPICE models should be also optimized
for good convergence in the simulation. If a model
doesn't provide some features like noise modeling
(.AC), it should behave more like an ideal
component in such a type of simulation.

The problem is that the PSpice models often don't
converge very well and don't model noise correctly.
That has nothing to do with Linear's opamp models,
it's common to most Boyle style models.

Hello Mike,
I have never said here that it is specific for LT models. My
statement has been a general one for all vendor's models.
If it is true that the Boyle model is so weak, why not starting with
another SPICE model? I am shure that LT has the right people(you for
example) to make excellent models.

They don't
converge well in PSpice either. It's just a really
lame modeling methodology. Sometimes I honestly
get the impression that SPICE macromodeling
engineers tweak a model until it doesn't run anymore
and pronounce it done at that point, blaming any
convergence problems are due to the simulator.

I have experimented with my own generic opamp model and indeed it
converges very different depending on the choosen circuit.

LTSPICE has been greatly improved over the last year regarding
convergence problems. Most of the problems seem to be history.

Of course the advantage of being able to run
them in PSpice is important.

There are even more SPICE simulators around. Some of them are
specific SPICE simulators like ICAP and others are part of PCB-CAD
packages. All these users need/want SPICE models of LT opamps.
Finally I hope that LT always provide opamp models for the whole
SPICE "family" too.

Best Regards
Helmut

Dale wrote:

Mike, this sounds like something I'd like to
dissuade you from.

Helmult wrote:
I fully agree with you. The biggest advantage
of all the opamp models
[...]
The provided SPICE models should be also optimized
for good convergence in the simulation. If a model
doesn't provide some features like noise modeling
(.AC), it should behave more like an ideal
component in such a type of simulation.

The problem is that the PSpice models often don't
converge very well and don't model noise correctly.
That has nothing to do with Linear's opamp models,
it's common to most Boyle style models. They don't
converge well in PSpice either. It's just a really
lame modeling methodology. Sometimes I honestly
get the impression that SPICE macromodeling
engineers tweak a model until it doesn't run anymore
and pronounce it done at that point, blaming any
convergence problems are due to the simulator.

Essentially all customer-reported SwCADIII
convergence problems reported deal with using
these opamp models. But inside the mixed-mode
simulator in LTspice is the ability to model
an opamp model like I described. Few convergence
problems, one or two internal nodes, good noise
modeling and almost no load on the simulation
run time. The technology already exists in
LTspice and is used in the SMPS products' error
amps.

Another problem I have is there's some newer
Linear opamps that don't have any SPICE models.
If I go to this new method, then I can make a
model in less than an hour that will be more
accurate than the former PSpice models. It's
much cheaper and it's hard to justify these
expensive PSpice models that don't work well.
Of course the advantage of being able to run
them in PSpice is important.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!