开云体育

John,

Are there any special considerations with using
P-spice op-amp macro models with LTspice? I'm
trying to simulate a circuit that uses a Burr
Brown/TI electrometer op-amp (OPA128 or OPA129)
and I'm getting incorrect results...

As has been pointed out, the non-E version of
the models do leak much more than the product.
That's the model. The E versions are supposed
model input bias current and it still leaked
too much in LTspice.

I just found out why the E models have large
bias currents in LTspice. It turns out that
all current sources in PSpice are shorted out
with a very small conductivity equal to GMIN
which defaults to 1e-12.

All versions of the models have use JFETs for
the input stage. The JFET supplies GMIN
conductivity between gate-source and gate-
drain. With +/-15V supply voltage this leads
to an input bias current of 15pA. In LTspice
you can set GMIN to zero, so you an turn off
this leakage. But PSpice can't converge with
GMIN=0.

So the -E versions of the models add a current
source to cancel the JFET leakage. So far
so good. Unfortunately, all current sources
in PSpice also supply their own additional GMIN
of conductivity. That is, PSpice shorts out
all current sources with a resistivity of 1e12
Ohms. There's no reason for this, it's just
bad SPICE design as far as I can tell. So the
additional current source to cancel the JFET
leakage has to cancel it's own leakage, too.
That's what makes the expression of the G-
sources so complicated. Also, when you run
the -E version in LTspice, the bias current
doesn't go to zero where if you run it in
PSpice, it will. I will probably and an
option in the control panel of LTspice to
duplicate this leakage as an option in the
near future.

Thanks to Helmut for help in isolating the
problem.

Below is a deck that shows the PSpice vs LTspice
leakage of currents. In LTspice you will get
the correct answer, but in PSpice, you will
get an error because the current sources don't
have infinite impedance.

--Mike

*
* V(y) should be 100KV
R1 Y 0 1e11
G1 0 Y N001 0 1
Vin3 N001 0 1u

* V(x) should be -100KV
R2 X 0 1e11
G2 X 0 value = { 1u }

* V(z) should be -100KV
I1 Z 0 1u
R3 Z 0 1e11
.tran 1m 1
.options gmin=1e-10
.probe
.end


__________________________________________________
Do you Yahoo!?
Yahoo! Web Hosting - establish your business online

--- In LTspice@..., brian.howie@b... wrote:

Are there any special considerations with using P-spice op-amp

macro

models with LTspice? I'm trying to simulate a circuit that uses a
Burr Brown/TI electrometer op-amp (OPA128 or OPA129) and I'm

getting

incorrect results. I downloaded the models from TI's website.

The

circuit's been built and thoroughly debugged, so I'm confident in

the

design.

When I couldn't get the circuit to operate correctly, I entered a
simple test circuit to verify some of the basic op-amp
characteristics. I found that the input bias current was way to

high

(about 12nA instead of 100fA), and the gain-bandwidth of the

OPA129

was high by about a factor of 10. I suspect that the models are

just

screwed up, but since I'm new to LTspice I'm not completely

confident

with my conclusion. Any help would be greatly appreciated.

I get similar problems with the OP27A, although in my case it is

the noise that

is reported about 2 orders more than the data sheet and hand

calculations

suggest. The bias currents look right. Other vendors opamps seem to

behave.

I ran a test circuit on Accusim II (Eldo SPICE-like kernal) and

the OP27A gave

sensible answers. I ported the netlist back to LTSPICE and although

the AC

analysis ran, the noise analysis gave up . I put the Accusim OP27A

model into

LTSPICE library and it gave the same wrong noise on my test

circuit.

Brian



--
Brian Howie | Tel: 0131 343 5590
BAE SYSTEMS | Fax: 0131 343 5050
Sensor Systems Division | Email brian.howie@b...
Silverknowes | bhowie@i...
Edinburgh EH4 4AD | Web site www.baesystems.com


***
This email and any attachments are confidential to the intended
recipient and may also be privileged. If you are not the intended
recipient please delete it from your system and notify the sender.
You should not copy it or use it for any purpose nor disclose or
distribute its contents to any other person.
***

Brain,

On one hand, I'm frustrated to learn there are so many issues with
vendor supplied models. This sort of problem can send you down a rat
hole for quite some time, and leave you worrying about the soundness
of your design. On the other hand, I know that I'm going to only use
simulation to validate my initial design and analysis, and not use it
as a substitute for other analytical methods. This experience only
supports my convictions and helps keep me honest.

- John

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

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

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

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

wrote:

Are there any special considerations with using P-spice op-

amp

macro

models with LTspice? I'm trying to simulate a circuit that

uses

a

Burr Brown/TI electrometer op-amp (OPA128 or OPA129) and I'm

getting

incorrect results. I downloaded the models from TI's

website.

The

circuit's been built and thoroughly debugged, so I'm

confident

in

the

design.

When I couldn't get the circuit to operate correctly, I

entered

a

simple test circuit to verify some of the basic op-amp
characteristics. I found that the input bias current was way

to

high

(about 12nA instead of 100fA), and the gain-bandwidth of the

OPA129

was high by about a factor of 10. I suspect that the models

are

just

screwed up, but since I'm new to LTspice I'm not completely

confident

with my conclusion. Any help would be greatly appreciated.

Hello John,
I tried to verify your results and the bias currents are indeed

a

lot

higher than expected. I looked around in the LTSPICE settings

for

possible leakage currents and other precision important

parameters.

Finally I have found that we need the command line

.OPTIONS gmin=0 (or at least <1e-18)

It defines the minimum conductance added to every node.
The simulated input bias current is then 40pA for the OPA128

and

OPA129.
The AC-gain results are really by a factor of ten too high for

the

OPA129/OPA129E.

I still don't know why the enhanced models OPA128E and OPA129E

still

shows bias currents of about 30pA instead of 40fA.
I tried the OPA129E with the PSPICE 8.0 demo.
Surprise, surprise! Even with the OPA129E, the bias current has

been

40fA. Something seems to go wrong in LTSPICE with this enhanced

model

in the .OP calculation.

The .AC simulation shows exactly the same results in PSPICE as

in

LTSPICE.

Best Regards
Helmut

Helmut,

Thanks for looking into this and going to the trouble of

duplicating

my results. I've also had problems with the enhanced model for

the

INA128 instrumentation amplifier. The standard model seems to

work

OK although it does have a little trouble converging. One thing

for

sure, it's definitely worth the effort of proving the model in a
simple circuit against data sheet specs, particularly when second
order effects are critical.

Hello John,
I have to take back my statement that LTSPICE was wrong with the
OPA129E input bias current. I further investigated the enhanced(E)
model and it is obvious that it isn't modelled correctly for bias
current. Now it seems the PSPICE simulation has been wrong with the
OPA129E.

These are the two critical lines of the enhanced model.

g11 2 4 poly(4) (10,2) (11,2) (4,2) (66,0) 0 1E-12 1E-12 1E-12
100E-9

g21 1 4 poly(4) (10,1) (12,1) (4,1) (68,0) 0 1E-12 1E-12 1E-12
100E-9

Node 1 and 2 are the input pins. g11 and g21 should simulate input
currents proportional to the negative supply voltage(4), the common
source point(10) the drain(11 close to V-) and node 66 which is

close

to (0). Assuming 15V for the negative supply gives bias currents of
15V*1e-12 = 15pA.

Finally I am wondering how PSPICE can calculate 40fA bias current.

Best Regards
Helmut

Helmut,

Thanks again for looking so thoroughly into this. I'm surprised that
they use such a complicated expression for bias current, unless the
terms help implement the bias current temperature coefficient.
According to the data sheet, the bias current is relatively constant
over a wide range of common mode voltage, implying that the
difference between the inputs and the negative supply should have
little effect on this parameter. Like any JFET op-amp, bias current
increases exponentially with temperature, so temperature is by far
the dominant variable. I do find it surprising that such a critical
characteristic would be modeled incorrectly, as there is no reason to
use this op-amp other than for it's extremely low bias current.

Thanks,
John

Are there any special considerations with using P-spice op-amp macro
models with LTspice? I'm trying to simulate a circuit that uses a
Burr Brown/TI electrometer op-amp (OPA128 or OPA129) and I'm getting
incorrect results. I downloaded the models from TI's website. The
circuit's been built and thoroughly debugged, so I'm confident in the
design.

When I couldn't get the circuit to operate correctly, I entered a
simple test circuit to verify some of the basic op-amp
characteristics. I found that the input bias current was way to high
(about 12nA instead of 100fA), and the gain-bandwidth of the OPA129
was high by about a factor of 10. I suspect that the models are just
screwed up, but since I'm new to LTspice I'm not completely confident
with my conclusion. Any help would be greatly appreciated.

I get similar problems with the OP27A, although in my case it is the noise that
is reported about 2 orders more than the data sheet and hand calculations
suggest. The bias currents look right. Other vendors opamps seem to behave.

I ran a test circuit on Accusim II (Eldo SPICE-like kernal) and the OP27A gave
sensible answers. I ported the netlist back to LTSPICE and although the AC
analysis ran, the noise analysis gave up . I put the Accusim OP27A model into
LTSPICE library and it gave the same wrong noise on my test circuit.

Brian



--
Brian Howie | Tel: 0131 343 5590
BAE SYSTEMS | Fax: 0131 343 5050
Sensor Systems Division | Email brian.howie@...
Silverknowes | bhowie@...
Edinburgh EH4 4AD | Web site www.baesystems.com


***
This email and any attachments are confidential to the intended
recipient and may also be privileged. If you are not the intended
recipient please delete it from your system and notify the sender.
You should not copy it or use it for any purpose nor disclose or
distribute its contents to any other person.
***

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

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

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

wrote:

Are there any special considerations with using P-spice op-amp

macro

models with LTspice? I'm trying to simulate a circuit that

uses

a

Burr Brown/TI electrometer op-amp (OPA128 or OPA129) and I'm

getting

incorrect results. I downloaded the models from TI's

website.

The

circuit's been built and thoroughly debugged, so I'm confident

in

the

design.

When I couldn't get the circuit to operate correctly, I entered

a

simple test circuit to verify some of the basic op-amp
characteristics. I found that the input bias current was way

to

high

(about 12nA instead of 100fA), and the gain-bandwidth of the

OPA129

was high by about a factor of 10. I suspect that the models

are

just

screwed up, but since I'm new to LTspice I'm not completely

confident

with my conclusion. Any help would be greatly appreciated.

Hello John,
I tried to verify your results and the bias currents are indeed a

lot

higher than expected. I looked around in the LTSPICE settings for
possible leakage currents and other precision important

parameters.

Finally I have found that we need the command line

.OPTIONS gmin=0 (or at least <1e-18)

It defines the minimum conductance added to every node.
The simulated input bias current is then 40pA for the OPA128 and
OPA129.
The AC-gain results are really by a factor of ten too high for

the

OPA129/OPA129E.

I still don't know why the enhanced models OPA128E and OPA129E

still

shows bias currents of about 30pA instead of 40fA.
I tried the OPA129E with the PSPICE 8.0 demo.
Surprise, surprise! Even with the OPA129E, the bias current has

been

40fA. Something seems to go wrong in LTSPICE with this enhanced

model

in the .OP calculation.

The .AC simulation shows exactly the same results in PSPICE as in
LTSPICE.

Best Regards
Helmut

Helmut,

Thanks for looking into this and going to the trouble of

duplicating

my results. I've also had problems with the enhanced model for the
INA128 instrumentation amplifier. The standard model seems to work
OK although it does have a little trouble converging. One thing

for

sure, it's definitely worth the effort of proving the model in a
simple circuit against data sheet specs, particularly when second
order effects are critical.

Hello John,
I have to take back my statement that LTSPICE was wrong with the
OPA129E input bias current. I further investigated the enhanced(E)
model and it is obvious that it isn't modelled correctly for bias
current. Now it seems the PSPICE simulation has been wrong with the
OPA129E.

These are the two critical lines of the enhanced model.

g11 2 4 poly(4) (10,2) (11,2) (4,2) (66,0) 0 1E-12 1E-12 1E-12
100E-9

g21 1 4 poly(4) (10,1) (12,1) (4,1) (68,0) 0 1E-12 1E-12 1E-12
100E-9

Node 1 and 2 are the input pins. g11 and g21 should simulate input
currents proportional to the negative supply voltage(4), the common
source point(10) the drain(11 close to V-) and node 66 which is close
to (0). Assuming 15V for the negative supply gives bias currents of
15V*1e-12 = 15pA.

Finally I am wondering how PSPICE can calculate 40fA bias current.

Best Regards
Helmut

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

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

Are there any special considerations with using P-spice op-amp

macro

models with LTspice? I'm trying to simulate a circuit that uses

a

Burr Brown/TI electrometer op-amp (OPA128 or OPA129) and I'm

getting

incorrect results. I downloaded the models from TI's website.

The

circuit's been built and thoroughly debugged, so I'm confident in

the

design.

When I couldn't get the circuit to operate correctly, I entered a
simple test circuit to verify some of the basic op-amp
characteristics. I found that the input bias current was way to

high

(about 12nA instead of 100fA), and the gain-bandwidth of the

OPA129

was high by about a factor of 10. I suspect that the models are

just

screwed up, but since I'm new to LTspice I'm not completely

confident

with my conclusion. Any help would be greatly appreciated.

Hello John,
I tried to verify your results and the bias currents are indeed a

lot

higher than expected. I looked around in the LTSPICE settings for
possible leakage currents and other precision important parameters.
Finally I have found that we need the command line

.OPTIONS gmin=0 (or at least <1e-18)

It defines the minimum conductance added to every node.
The simulated input bias current is then 40pA for the OPA128 and
OPA129.
The AC-gain results are really by a factor of ten too high for the
OPA129/OPA129E.

I still don't know why the enhanced models OPA128E and OPA129E

still

shows bias currents of about 30pA instead of 40fA.
I tried the OPA129E with the PSPICE 8.0 demo.
Surprise, surprise! Even with the OPA129E, the bias current has

been

40fA. Something seems to go wrong in LTSPICE with this enhanced

model

in the .OP calculation.

The .AC simulation shows exactly the same results in PSPICE as in
LTSPICE.

Best Regards
Helmut

Helmut,

Thanks for looking into this and going to the trouble of duplicating
my results. I've also had problems with the enhanced model for the
INA128 instrumentation amplifier. The standard model seems to work
OK although it does have a little trouble converging. One thing for
sure, it's definitely worth the effort of proving the model in a
simple circuit against data sheet specs, particularly when second
order effects are critical.

Thanks,
John

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

Are there any special considerations with using P-spice op-amp

macro

models with LTspice? I'm trying to simulate a circuit that uses a
Burr Brown/TI electrometer op-amp (OPA128 or OPA129) and I'm

getting

incorrect results. I downloaded the models from TI's website.

The

circuit's been built and thoroughly debugged, so I'm confident in

the

design.

When I couldn't get the circuit to operate correctly, I entered a
simple test circuit to verify some of the basic op-amp
characteristics. I found that the input bias current was way to

high

(about 12nA instead of 100fA), and the gain-bandwidth of the OPA129
was high by about a factor of 10. I suspect that the models are

just

screwed up, but since I'm new to LTspice I'm not completely

confident

with my conclusion. Any help would be greatly appreciated.

Hello John,
I tried to verify your results and the bias currents are indeed a lot
higher than expected. I looked around in the LTSPICE settings for
possible leakage currents and other precision important parameters.
Finally I have found that we need the command line

.OPTIONS gmin=0 (or at least <1e-18)

It defines the minimum conductance added to every node.
The simulated input bias current is then 40pA for the OPA128 and
OPA129.
The AC-gain results are really by a factor of ten too high for the
OPA129/OPA129E.

I still don't know why the enhanced models OPA128E and OPA129E still
shows bias currents of about 30pA instead of 40fA.
I tried the OPA129E with the PSPICE 8.0 demo.
Surprise, surprise! Even with the OPA129E, the bias current has been
40fA. Something seems to go wrong in LTSPICE with this enhanced model
in the .OP calculation.

The .AC simulation shows exactly the same results in PSPICE as in
LTSPICE.

Best Regards
Helmut

Are there any special considerations with using P-spice op-amp macro
models with LTspice? I'm trying to simulate a circuit that uses a
Burr Brown/TI electrometer op-amp (OPA128 or OPA129) and I'm getting
incorrect results. I downloaded the models from TI's website. The
circuit's been built and thoroughly debugged, so I'm confident in the
design.

When I couldn't get the circuit to operate correctly, I entered a
simple test circuit to verify some of the basic op-amp
characteristics. I found that the input bias current was way to high
(about 12nA instead of 100fA), and the gain-bandwidth of the OPA129
was high by about a factor of 10. I suspect that the models are just
screwed up, but since I'm new to LTspice I'm not completely confident
with my conclusion. Any help would be greatly appreciated.

Thanks,
John

--- In LTspice@..., D Chisholm <dchishol@c...> wrote:

You may have to download the complete package and re-install from
scratch under Wine. I had this problem (sync release didn't work) when
I had LTSpice on my machine at work behind a corporate firewall.

It wasn't a really big deal on my NT station. I just downloaded the
latest release every couple of weeks, and the new version always
installed smoothly over the old version. The only glitch is that the
standard component library files get clobbered by the new installation.
(These are the files called "standard.bjt", "standard.dio", etc in
"..&#92;SwCADIII&#92;lib&#92;cmp".) If you've added any transistors, capacitors,
etc to these databases you'll lose the data. (The Sync Release tool
merges your additions to the old database, with the new database

files -

which I find rather impressive!) To work around this, I created a
parallel structure of files called "additions.bjt", "additions.dio",
etc to hold info for the the components I added then I used a text
editor to append my "additions.xxx" on the end of the "standard.xxx"
files after every re-installation. A DOS macro of about 3 lines could
probably do the same thing with the "copy <file1>+<file2>" command if I
was too lazy to open the text editor.

Maybe this summer Mike (Englehardt) will get a student intern who can
re-work the installation package so the user can specify either a
complete installation or simply update an existing installation . . .

Dale

Thank You for the advice.
I tried to re-install from scratch under Wine but I have the same
problem. I think I will follow the procedure that You use under NT.

Thank You again

Stefano

Jon,

Is there way to get the peak-to-peak over a specific
time range? One simple calculation I'd like to do
is to get a close estimate of the gain figure by,
say, dividing the output p-p by the input p-p.
But I want this figure computed, based on the time
range of, say, t0=100ms to t1=200ms?

No really, but the cursors are helpful. You can get
a quick idea by dragging a box as if you were going
to zoom that just touches the peak and valley points
and looking at the dy value on the status bar. You
can read differences on the waveforms in this manner
and skip the zoom by either pressing the right button
before releasing the left or pressing ECS.

Another method is to attach both attachable cursors
to the same trace.(Right click on the trace label
use the "Attached Cursor:" list of possibilities.
Drag one cursor to the peak and the other to the
valley and then you can read off the difference
on the attached cursor readout.

I'm also going to have to figure out a simple way
to look at effects of temperature variation and
component variation on gain and DC quiescent point,
again only over a specified time range.

See .step and .temp in the help. Also check out
the examples with the word step in the file name.

What about computing group delay through a
filter or amplifier?

Do a .AC analysis. Then move the mouse to the right
of the plot. The mouse cursor will turn into a
ruler trying to indicate that you are pointing
at that axis' attributes. Pick group delay
instead of phase in the representation group.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - forms, calculators, tips, more

You may have to download the complete package and re-install from scratch under Wine. I had this problem (sync release didn't work) when I had LTSpice on my machine at work behind a corporate firewall.

It wasn't a really big deal on my NT station. I just downloaded the latest release every couple of weeks, and the new version always installed smoothly over the old version. The only glitch is that the standard component library files get clobbered by the new installation. (These are the files called "standard.bjt", "standard.dio", etc in "..&#92;SwCADIII&#92;lib&#92;cmp".) If you've added any transistors, capacitors, etc to these databases you'll lose the data. (The Sync Release tool merges your additions to the old database, with the new database files - which I find rather impressive!) To work around this, I created a parallel structure of files called "additions.bjt", "additions.dio", etc to hold info for the the components I added then I used a text editor to append my "additions.xxx" on the end of the "standard.xxx" files after every re-installation. A DOS macro of about 3 lines could probably do the same thing with the "copy <file1>+<file2>" command if I was too lazy to open the text editor.

Maybe this summer Mike (Englehardt) will get a student intern who can re-work the installation package so the user can specify either a complete installation or simply update an existing installation . . .

Dale

stefanodel wrote:

In my PC running Linux (SuSe 8.1) I installed wine, then I installed
SwitcherCADIII. The program seems to work well, I have only a little
problem, I am not able to update the program using internet.If I try
to sync release I get the the message "could not access web ..."
I have the connection to internet active, but I get this message. I
dont know if using wine it is possible to update the program.
Someone can help me ?

Stefano Delfiore

On Sat, 8 Mar 2003 13:58:35 -0800 (PST), you wrote:

Thanks for that wonderful letter you wrote. I
forwarded it to the Chief Technical Officer at
Linear. Hope that's okay.

Hehe. Sure! I want folks at Linear to realize it's all
appreciated.

For your question, it might help you to know that
you can see what your {} expressions evaluated to
in this manner:

1. Go to Tools=>Control Panel=>Operation.
2. Check "Generate Expanded Listing"
3. Then, after you run the simulation, make the
schematic the active window and use the menu
command View=>SPICE Error Log. In the listing
you will see how the {} expressions were
evaluated.

Anyway, that's how I do it.

Works for me. Looks good. Thanks!

...

Is there way to get the peak-to-peak over a specific time range?
One simple calculation I'd like to do is to get a close estimate
of the gain figure by, say, dividing the output p-p by the input
p-p. But I want this figure computed, based on the time range
of, say, t0=100ms to t1=200ms?

I'm also going to have to figure out a simple way to look at
effects of temperature variation and component variation on gain
and DC quiescent point, again only over a specified time range.

What about computing group delay through a filter or amplifier?

And can LT Spice conserve or account for charge in the
calculations?

Sorry, I keep wondering about all the possibilities, now.

Jon

Jon,

Thanks for that wonderful letter you wrote. I
forwarded it to the Chief Technical Officer at
Linear. Hope that's okay.

For your question, it might help you to know that
you can see what your {} expressions evaluated to
in this manner:

1. Go to Tools=>Control Panel=>Operation.
2. Check "Generate Expanded Listing"
3. Then, after you run the simulation, make the
schematic the active window and use the menu
command View=>SPICE Error Log. In the listing
you will see how the {} expressions were
evaluated.

Anyway, that's how I do it.

Regards,

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - forms, calculators, tips, more

I want to start out by saying that I'm a hobbyist, not an
electronics professional.

When I first heard of SwitcherCAD III/LT Spice perhaps a year
ago, I went to the Linear web site with the intent to download
the program and completely failed to understand what I almost
had in hand. From the descriptions, it looked like some kind of
specialized program for switcher-based power supplies and that
was far too limited to be very interesting at the time. It
wasn't until later reading of comments by one of the active
members of the LT Spice team (Mike) that I began to realize my
mistake and attempted to download LT Spice in January. Boy, was
that a good decision.

In the past, I've tried, and actually purchased, a few other
programs claiming to provide electronics simulations. I've had
a crashed Windows, substantial memory leaks, and overly complex
setup for simulation and overly complex arrangements to observe
the signal values I'm interested in (in some cases, having to
manually wire up a "meter" in order to get those results, and
even then with difficulty.) By comparison, and this isn't
simply a false impression because of my building on prior
experience, LT Spice was a dream to use. Once I set down to
seriously confront a simple circuit, it took me no time at all
(and without reading any help files) to create it and get
results I was interested in seeing. This stands in stark
contrast to past experience.

As I've spent a little more time in LT Spice, every moment has
been well paid back by discovery of still more useful and
interesting features. It's actually such a joy, that I've gone
out and purchased an original Spice II PhD thesis from 1975,
recommended by Mike, and another similar book and have found all
of it very useful. Every minute has been well-paid and I can
barely imagine a tool which is easier to use.

Of course, I'm still too much a neophyte, both in electronics
knowledge as well as in simulation depth, to know whether or not
this program provides simulations which are incorrect in some
important details and which will lead me into very wrong
impressions which will be hard to unlearn. But I'm pretty
confortable in my current belief, tested in a few cases I've
actually built and used, that it's providing good results. And
comforted aslo by the active support of this program.

All that is by way of introduction for a question I have:

I've taken advantage of .param in order to allow me to specify
certain important values for a basic degenerative amplifier
design. The components used in this model design are all
specified with expressions using the set signs, {}. Simulation
results look encouraging to me, now, but I'd like to see what
the results of the calculations for these expressions were, in
simulation, so that I can now specify real values and build one
for testing. I could go use my calculator, of course, and
figure these out. But I'd like LT Spice to display the results
of its own calculations without my having to use a calculator,
by hand. Is this easily doable?

My guess is that I could write an expression into the graphical
display as another trace and just see the value of the straight
line, but that's not a good way to do this. What I'm
considering as "nice" would be to right-click over the
expression on the schematic and call up a dialog box for
extering the expression, but where this dialog box would *also*
show the current result of the existing expression.

Anyway, that's my question for now. Thanks to all!

Jon

--- In LTspice@..., "Helmut Sennewald
<helmutsennewald@y...>" <helmutsennewald@y...> wrote:

--- In LTspice@..., "polapart <sahawley@m...>"
<sahawley@m...> wrote:

I was looking around for a model of a low voltage MUX like the
74lv4051. I found a a 6 pin fragment in the Philips LV library
() called SWI1. I wired

it

up and it ran fine with DC control input, but when I attempted to
toggle the switch with a square wave, once it turned off it never
turned on again.

Any ideas what's going on here and or pointers to a fully

functional

part model.

Hello,
unfortunately I don't know any other source of SPICE model for this
part. The behaviour looked indeed strange. It was ok with static
driven control input, but failed with a pulse source. I already
speculated about a problem of LTSpice.
The last resort was to sketch the circuit from the netlist through
all levels of subcircuits. That was a hard work and I wouldn't have
done it, if I hadn't feared a problem of the LTSpice simulator.
I found an inverter output connected to no other stage in the used
subcircuit LLCN. The subcircuit levels are SWI1 -> LLCN. This
circuit contains a first inverter, a two stage level shifter and

two

more following inverters. The output of the first inverter was
connected to no other circuit. Obviously this is wrong. Either MP1

or

MP2 has to be connected to node '4'. I supposed MP2. The simulation
now runs with pulse sources as expected.

Conclusion: There is a bug in this Philips model. This is really a
pain and now I have low confidence about the quality of this

library.

It is in zhree files: Lvnomi.cir, lvfast.cir, lvslow.cir .
I suppose to change the line in the .subckt LLCN ...

MP2 6 2 50 50 MLVPEN W=135U .......

to

MP2 6 4 50 50 MLVPEN W=135U .......

The interested reader can draw the schematic from the netlist.

Hope that helps and please next time an easier problem.

Hello,
I reported this bug to Philips. Today I have got feedback that my
correction of this model has been correct. They promised to fix it in
their library until mid of March.

Best Regards
Helmut

--- In LTspice@..., "Helmut Sennewald
<helmutsennewald@y...>" <helmutsennewald@y...> wrote:

--- In LTspice@..., Bill Lewis <wrljet@y...> wrote:

Thanks! I'm checking it out now.

Hello Bill,
I forgot to mention that the symbols for the triode, tetrode and
pentode are all in the "misc" directory of LTSpice. I am not shure
you were aware of that.

And again some more information.

The model in my example file is from this link:


Another source is:


Best Regards
Helmut

--- In LTspice@..., Bill Lewis <wrljet@y...> wrote:

Thanks! I'm checking it out now.

Hello Bill,
I forgot to mention that the symbols for the triode, tetrode and
pentode are all in the "misc" directory of LTSpice. I am not shure
you were aware of that.

Best Regards
Helmut

Thanks! I'm checking it out now.

Bill

--- "Helmut Sennewald <helmutsennewald@...>" <helmutsennewald@...>
wrote:

--- In LTspice@..., "Bill Lewis <wrljet@y...>"
<wrljet@y...> wrote:

Has anyone migrated any of the vacuum tube models floating
around on the 'net to LTspice?

Hello Bill,
I did it once for a pentode. The model is included in the schematic,
but this can be changed using a library file valve.lib.
Then add instead .include valve.lib in the schematic.
It is very important to look on the used pin order. Everybody
has another pin order used in his library. It have to be changed
according to the pin order of your symbol or you make your own symbol
with the appropriate pin order. I couldn't attach it, because the
lines will be split by this awful YAHOO reader. I put it into this
group's Files->examples->apps folder. It is the file "pentode.asc".

Best Regards
Helmut





To unsubscribe from this group, send an email to:
LTspice-unsubscribe@...



Your use of Yahoo! Groups is subject to

__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - forms, calculators, tips, more

--- In LTspice@..., "Bill Lewis <wrljet@y...>"
<wrljet@y...> wrote:

Has anyone migrated any of the vacuum tube models floating
around on the 'net to LTspice?

Hello Bill,
I did it once for a pentode. The model is included in the schematic,
but this can be changed using a library file valve.lib.
Then add instead .include valve.lib in the schematic.
It is very important to look on the used pin order. Everybody
has another pin order used in his library. It have to be changed
according to the pin order of your symbol or you make your own symbol
with the appropriate pin order. I couldn't attach it, because the
lines will be split by this awful YAHOO reader. I put it into this
group's Files->examples->apps folder. It is the file "pentode.asc".

Best Regards
Helmut