开云体育

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

Please post any replies to this question to the list.
I'm interested in vacuum tube modeling.

... and the obvious question: How do I relate the previous info

with

the symbol.

Hello Bill,
you will find the symbol in the "misc" directory.
A short description follows:
1. Load the triode symbol into your schematic.
2. Replace the value 'triode' with the model name used in the model
file. In this case it is '12AX7A'.
3. Put the model text into a file and store it in your working
directory. That is the directory where your schematic is.
4. Add the line .INCLUDE modelfilename in your schematic.
That's it. This procedure will work for any kind of part and you can
put as many models you want into one file.

It is important for any kind of symbol and model that the pin order
is matching. Let's take a look to the triode symbol. The provided
symbol has the pin order P(1), G(2), K(3). The model text
uses .SUBCKT 12AX7A P G K . This means that P is pin-1 G is pin-
2 and K is pin-3. We have luck, the pin order is the same. If it is
different, then we could either change the order in the model text or
in the symbol.

I have the ready to run example files attached.

By the way, the model isn't good at low Vpk voltages. Take a look to
the Ip(Vgk, Vpk) plot to see what I mean.

Best Regards
Helmut




The model file: triode_12ax7a.sub
---------------------------------

* 12AX7A Triode PSpice Model 8/96, Rev. 1.0 (fp)
*
* -------------------------------------------------------------------
* This model is provided "as is", with no warranty of any kind,
* either expressed or implied, about the suitability or fitness
* of this model for any particular purpose. Use of this model
* shall be entirely at the user's own risk.
*
* For a discussion about vacuum tube modeling please refer to:
* W. Marshall Leach, jr: "SPICE Models for Vacuum-Tube Amplifiers";
* J. Audio Eng. Soc., Vol 43, No 3, March 1995.
* -------------------------------------------------------------------
*
* This model is valid for the following tubes:
* 12AX7A/ECC83, 7025, 6EU7, 6681, 6AV6, 12DW7/7247 (Unit #1);
* at the following conditions:
* Plate voltage : 25..400V
* Grid voltage : 0..-3.5V
* Cathode current: 0..8mA
*
*
* Connections: Plate
* | Grid
* | | Cathode
* | | |
.SUBCKT 12AX7A P G K
E1 2 0 VALUE={45+V(P,K)+95.43*V(G,K)}
R1 2 0 1.0K
Gp P K VALUE={1.147E-6*(PWR(V(2),1.5)+PWRS(V(2),1.5))/2}
Cgk G K 1.6P
Cgp G P 1.7P
Cpk P K 0.46P
.ENDS 12AX7A.SUBCKT 12AX7A P G K


The circuit file: triode_test.asc
---------------------------------

Version 4
SHEET 1 1104 692
WIRE 336 384 336 496
WIRE 368 288 368 224
WIRE 368 224 512 224
WIRE 512 336 512 224
WIRE 512 416 512 496
WIRE 512 496 336 496
WIRE 336 496 176 496
WIRE 176 496 176 448
WIRE 176 368 176 336
WIRE 176 336 320 336
WIRE 176 528 176 496
FLAG 176 528 0
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;Misc&#92;triode 368 336 R0
SYMATTR InstName U1
SYMATTR Value 12AX7A
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage 176 352 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value 0
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage 512 320 R0
SYMATTR InstName V2
SYMATTR Value 200V
TEXT 142 136 Left 0 !;dc V2 0 200 0.1 V1 -5 20 5
TEXT 136 176 Left 0 !.INCLUDE triode_12ax7a.sub
TEXT 592 136 Left 0 ;.dc V2 0 200 0.1 V1 -5 20 5 Ip(Vpk, Vgk)
TEXT 144 96 Left 0 !.dc V1 -5 20 0.1
TEXT 592 96 Left 0 ;.dc V1 -5 20 0.1 Ip(Vgk)

kaplounovski wrote:

Hello,
I'm trying to use the National LMC6484A opamp model in LTSpice.
I've downloaded their model and placed it
into ..&#92;LTC&#92;SWCADIII&#92;lib&#92;sub directory under the name LMC6484A.sub.
Then I created a simple test schematic where I used opamp2 symbol with
Prefix = X, Spice Model = LMC6484A.sub, Value = LMC6484A.sub
properties.
I've also added the .inc LMC6484A.sub directive to the netlist.

Running the simulation produces the following error message:
Error: Unknown subckt called in: xu1 ...... lmc6484a.sub lmc 6484a.sub

What am I doing wrong?

Thanks,
Eugene.


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



Your use of Yahoo! Groups is subject to

Try leaving model blank and using value = lmc6484a without the .sub
Good Luck
Jim Stockton

Hello,
I'm trying to use the National LMC6484A opamp model in LTSpice.
I've downloaded their model and placed it
into ..&#92;LTC&#92;SWCADIII&#92;lib&#92;sub directory under the name LMC6484A.sub.
Then I created a simple test schematic where I used opamp2 symbol with
Prefix = X, Spice Model = LMC6484A.sub, Value = LMC6484A.sub
properties.
I've also added the .inc LMC6484A.sub directive to the netlist.

Running the simulation produces the following error message:
Error: Unknown subckt called in: xu1 ...... lmc6484a.sub lmc 6484a.sub

What am I doing wrong?

Thanks,
Eugene.

Please post any replies to this question to the list.
I'm interested in vacuum tube modeling.

Thanks,
Bill

--- guille_bonh <guille_bonh@...> wrote:

I'd appreciate any help on modeling valves.
For example, I copy what I have for the triode 12AX7A:

* 12AX7A Triode PSpice Model 8/96, Rev. 1.0 (fp)
*
* -------------------------------------------------------------------
* This model is provided "as is", with no warranty of any kind,
* either expressed or implied, about the suitability or fitness
* of this model for any particular purpose. Use of this model
* shall be entirely at the user's own risk.
*
* For a discussion about vacuum tube modeling please refer to:
* W. Marshall Leach, jr: "SPICE Models for Vacuum-Tube Amplifiers";
* J. Audio Eng. Soc., Vol 43, No 3, March 1995.
* -------------------------------------------------------------------
*
* This model is valid for the following tubes:
* 12AX7A/ECC83, 7025, 6EU7, 6681, 6AV6, 12DW7/7247 (Unit #1);
* at the following conditions:
* Plate voltage : 25..400V
* Grid voltage : 0..-3.5V
* Cathode current: 0..8mA
*
*
* Connections: Plate
* | Grid
* | | Cathode
* | | |
.SUBCKT 12AX7A P G K
E1 2 0 VALUE={45+V(P,K)+95.43*V(G,K)}
R1 2 0 1.0K
Gp P K VALUE={1.147E-6*(PWR(V(2),1.5)+PWRS(V(2),1.5))/2}
Cgk G K 1.6P
Cgp G P 1.7P
Cpk P K 0.46P
.ENDS 12AX7A.SUBCKT 12AX7A P G K
E1 2 0 VALUE={45+V(P,K)+95.43*V(G,K)}
R1 2 0 1.0K
Gp P K VALUE={1.147E-6*(PWR(V(2),1.5)+PWRS(V(2),1.5))/2}
Cgk G K 1.6P
Cgp G P 1.7P
Cpk P K 0.46P


... and the obvious question: How do I relate the previous info with
the symbol. Thanks in advance,

Guillermo



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



Your use of Yahoo! Groups is subject to

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

I'd appreciate any help on modeling valves.
For example, I copy what I have for the triode 12AX7A:

* 12AX7A Triode PSpice Model 8/96, Rev. 1.0 (fp)
*
* -------------------------------------------------------------------
* This model is provided "as is", with no warranty of any kind,
* either expressed or implied, about the suitability or fitness
* of this model for any particular purpose. Use of this model
* shall be entirely at the user's own risk.
*
* For a discussion about vacuum tube modeling please refer to:
* W. Marshall Leach, jr: "SPICE Models for Vacuum-Tube Amplifiers";
* J. Audio Eng. Soc., Vol 43, No 3, March 1995.
* -------------------------------------------------------------------
*
* This model is valid for the following tubes:
* 12AX7A/ECC83, 7025, 6EU7, 6681, 6AV6, 12DW7/7247 (Unit #1);
* at the following conditions:
* Plate voltage : 25..400V
* Grid voltage : 0..-3.5V
* Cathode current: 0..8mA
*
*
* Connections: Plate
* | Grid
* | | Cathode
* | | |
.SUBCKT 12AX7A P G K
E1 2 0 VALUE={45+V(P,K)+95.43*V(G,K)}
R1 2 0 1.0K
Gp P K VALUE={1.147E-6*(PWR(V(2),1.5)+PWRS(V(2),1.5))/2}
Cgk G K 1.6P
Cgp G P 1.7P
Cpk P K 0.46P
.ENDS 12AX7A.SUBCKT 12AX7A P G K
E1 2 0 VALUE={45+V(P,K)+95.43*V(G,K)}
R1 2 0 1.0K
Gp P K VALUE={1.147E-6*(PWR(V(2),1.5)+PWRS(V(2),1.5))/2}
Cgk G K 1.6P
Cgp G P 1.7P
Cpk P K 0.46P


... and the obvious question: How do I relate the previous info with
the symbol. Thanks in advance,

Guillermo

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

I am trying to run a Burr Brown Op Amp, the OPA336.
The transient analysis "sort of" runs but LTSpice
notes a couple of problems, most notably
unrecognized parameters, jssw and vfb.

I couldn't find this model. Can you send it to me.

--Mike

Here's the link to the TI page. Thanks

genericPartNumber=OPA336&pfsection=models

Steve H

By the way, here's my .ASC file. Sadly,

By the way, I'm including my .ASC version as an attachment. If
that doesn't work in these posts, I'll just add it as text (but
the darned word-wrapping will probably mess it up.)

In this example, what I'd like to do is set up R2 as an equation
so that it is calculated. But I do *not* want to have to
estimate Vbe. I want to use the exact value, computed by LT
Spice, if possible. Since LT Spice must be using matrices to
simulate, I figure it should be able to solve for the necessary
values. But I don't know.

Thanks!

Jon

On Tue, 18 Mar 2003 15:21:56 -0800 (PST), you wrote:

I'm interested in calculating iterative values for
resistors[...]

The .asc file below might get you started there.

--Mike
<snipped file>

Thanks, I took a look at that. But it uses a set Vbe, which I
have to estimate beforehand and then measure and then re-edit
into the .param and then re-run and then re-measure and ...

I was wondering if there was a way to enter into an expression
the equivalent of: V(N001,N003). Or some-such. Possible? Or
am I stuck iterating to a solution, manually?

Jon

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

I am trying to run a Burr Brown Op Amp, the OPA336.
The transient analysis "sort of" runs but LTSpice
notes a couple of problems, most notably
unrecognized parameters, jssw and vfb.

I couldn't find this model. Can you send it to me.

--Mike


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

Jon,

I'm interested in calculating iterative values for
resistors[...]

The .asc file below might get you started there.

--Mike

Version 4
SHEET 1 892 900
WIRE 320 576 320 528
WIRE 320 448 320 400
WIRE 320 304 320 240
WIRE 320 240 128 240
WIRE 128 240 128 256
WIRE 128 336 128 352
WIRE 128 560 128 576
WIRE 128 464 128 480
WIRE 256 352 128 352
WIRE 128 352 128 368
WIRE 64 416 -304 416
WIRE -304 416 -304 448
WIRE -304 528 -304 560
WIRE 464 384 464 352
WIRE 464 272 464 240
WIRE 464 240 320 240
FLAG 128 576 0
FLAG 320 576 0
FLAG -304 560 0
FLAG 464 384 0
SYMBOL npn 64 368 R0
SYMATTR InstName Q1
SYMATTR Value 2N3904
SYMBOL pnp 256 400 M180
WINDOW 0 74 72 Left 0
WINDOW 3 76 34 Left 0
SYMATTR InstName Q2
SYMATTR Value 2N3906
SYMBOL res 112 240 R0
SYMATTR InstName R1
SYMATTR Value {R1}
SYMBOL res 112 464 R0
SYMATTR InstName R2
SYMATTR Value {R2}
SYMBOL voltage -304 432 R0
SYMATTR InstName V1
SYMATTR Value pulse(0 {Vdd} 0 10u 10u .5m 1m)
SYMBOL voltage 464 256 R0
SYMATTR InstName V2
SYMATTR Value {Vcc}
SYMBOL res 304 432 R0
SYMATTR InstName R3
SYMATTR Value {Rload}
TEXT -288 672 Left 0 !.param load=10m R2=500 Vdd=2
Vbe=.7
TEXT -288 736 Left 0 !.param R1=(Vdd -
Vbe)/(load/10+Vbe/R2+Ib)
TEXT -266 604 Left 0 !.tran 3m
TEXT -288 704 Left 0 !.param Ib=10u Rload = Vcc/load
Vcc=5


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

I am trying to run a Burr Brown Op Amp, the OPA336. The transient
analysis "sort of" runs but LTSpice notes a couple of problems, most
notably unrecognized parameters, jssw and vfb.

The AC analysis fails to converge. The comments in the deck offer
some advice with regard to modifyng ITL and gmin via .OPTION which
doesn't seem to help. Are these more PSPICE problems?

Thanks

I'm interested in calculating iterative values for resistors.
For example, an emitter resistor's value may be based on the
emitter voltage divided by some current I need to have.
However, the emitter voltage is, of course, dependent on the
emitter/collector current which will depend on the emitter
resistor value. An iterative process could track down this
value closely, but I don't know how to write the expression.

Here's an example of what I mean:

Vcc
|
,------x
| |
&#92; |
/ R2 |
&#92; |
| |
| |/e Q2
x----| PNP
| |&#92;c
| |
| '-----> to the load
|/c Q1
>-----| NPN
control |&#92;e
signal |
at Vdd |
or 0V, &#92;
not at / R1
Vcc &#92;
|
|
gnd

In this case, R1 needs to be:

R1 = (Vdd - Vbe(Q1))/(I(load)/10+Vbe(Q2)/R2+Ib(Q1))

I want to set up I(load) to some value and have R1 computed from
that.

When I type V(N001,N003) as part of the expression, in order to
get the Vbe(Q1) for example, it's rejected with "Unable to find
definition of model v - default assumed." This isn't what I
want, naturally.

Is there any way to set up the expression for R1, appropriately?

Jon

On Tue, 18 Mar 2003 09:16:19 -0800 (PST), you wrote:

Jon,

...But is it possible to extend the dialog box
list for the NPN transistors, for example, so
that I can simply select from the list rather
than overriding the "Value" on the schematic,
directly?
...
And if there is a way, can it be secure
against the automatic update process, so that
I keep my additions in the face of regular
updates?

The selection dialogs for bipolars, jfets, diodes,
and mosfets use the .model entries in the files
./lib/cmp/standard{.bjt,.jft,.dio,.mos} You can
edit these with a text editor(or LTspice) to add
new components. If you update with the menu item
Tools=>Sync Release, your versions of these files
should be merged with the new ones so you don't loose
your models.

Wonderful! That works better than I'd hoped. Glad you added
the extra code to make that happen during updating.

However, if LT now supplies a model
with the same name as one you've added, you will
loose your version of the model and it will be
replaced with the version from LT.

Okay. So this is a good reason why you might want to keep the
count of your models low -- less likely to kill someone's
personal models that they've added. In particular, I picked up
my own copy of the 2N3391A, for example, which is also in your
standard distribution. So if I placed it there in STANDARD.BJT,
it would be replaced during updating. Luckily, your version is
identical.

I also noticed that if I have a version of 2N3391A in my own
"BJT.LIB," for example, and your STANDARD.BJT also has that
model, as well, then your dialog's list does *not* include the
2N3391A in it, at all. It recognizes that there is a definition
in my own .LIB, so it removes it from its own list. Too bad it
doesn't just give priority to my definitions and compile a
composite list from both the STANDARD.BJT as well as my BJT.LIB,
for example. Then I wouldn't need to modify STANDARD.BJT, at
all.

That's because
the merge routine isn't smart enough to know which
one's you added and which ones are just old versions
from LT.

Makes sense to me. It would be tough to solve, generally. (I
suppose you could add a special parameter which only you'd use
in your models.)

That being said, I would like to recommend that you
keep a version of your own edited standard.* files
for safety.

Will do.

Note that if you don't use the Tools=>sync Release
feature but reinstall, then the standard.* files
will simply be replaced with those in the current
distribution.

Understood.

Or if I should decide to forget about the
standard components included with LT Spice
and start building my own large library
of parts with trusted parameters, can I get
them to be popped into these selection lists?

You'd have to maintain your own versions of
the standard.* files and copy them over into
the ./lib/cmp directory after every update.

Okay.

While I'm at it, it might be nice, someday, if you'd support
user designed .ASY's placed in lib&#92;sym which could have lists of
.SUBCKT attached to them which would be automatically supported
as a selection list for that .ASY. So that I could develop a
small list, for example, for the 2N6027 and 2N6028 or for other
custom X-type circuits I might develop.

(It's still incredible to me that I'm actually using and
learning from a simulator which doesn't eat up my system memory
or crash under WIN98 or otherwise complicate my life. So I'm
glad for everything I'm already using.)

BTW, only .model statements can be put in the
standard.* files. Subcircuits can't be parsed
there.

Thanks! I wouldn't have guessed about that limitation. I'll be
careful, then. (Chances are, and I'm guessing here, that this
probably means that allowing user-created X-type list generation
would be "difficult" under the current architecture. Oh, well.)

Thanks again for the active support. I'm already feeling
guilty.

Jon

Jon,

...But is it possible to extend the dialog box
list for the NPN transistors, for example, so
that I can simply select from the list rather
than overriding the "Value" on the schematic,
directly?
...
And if there is a way, can it be secure
against the automatic update process, so that
I keep my additions in the face of regular
updates?

The selection dialogs for bipolars, jfets, diodes,
and mosfets use the .model entries in the files
./lib/cmp/standard{.bjt,.jft,.dio,.mos} You can
edit these with a text editor(or LTspice) to add
new components. If you update with the menu item
Tools=>Sync Release, your versions of these files
should be merged with the new ones so you don't loose
your models. However, if LT now supplies a model
with the same name as one you've added, you will
loose your version of the model and it will be
replaced with the version from LT. That's because
the merge routine isn't smart enough to know which
one's you added and which ones are just old versions
from LT.

That being said, I would like to recommend that you
keep a version of your own edited standard.* files
for safety.

Note that if you don't use the Tools=>sync Release
feature but reinstall, then the standard.* files
will simply be replaced with those in the current
distribution.

Or if I should decide to forget about the
standard components included with LT Spice
and start building my own large library
of parts with trusted parameters, can I get
them to be popped into these selection lists?

You'd have to maintain your own versions of
the standard.* files and copy them over into
the ./lib/cmp directory after every update.

BTW, only .model statements can be put in the
standard.* files. Subcircuits can't be parsed
there.

--Mike

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

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

John,

I was really puzzled by the complicated G-
source _expression. That all makes sense now.

Yeah. I just put up a version, 2.00l. It lets you
duplicate the leakage of PSpice current sources in
LTspice. Go to Tools=>Control Panel=>SPICE and
check "Add GMIN across current sources" Then you
will see the input bias drop to zero on the -E
models.

There's still a couple differences between PSpice
and LTspice even after checking the box. PSpice
does not report the current's gmin leakage current,
which is just a dumb mistake that I don't
duplicate. Also, in PSpice the current sources
don't leak in the .ac analysis, just .op and .tran.
Which is a complete inconsistency and just another
error I didn't duplicate in LTspice.

There's one other thing to keep in mind when
working with high impedance circuits. You might
want to tighten abstol. That controls the
absolute(vs. relative) acceptable current
error. It defaults to 1pA.

--Mike

_

Mike,

I downloaded the new release this morning and simulated my circuit
again. Sure enough, the input bias current is now reasonable and the
simulation behaves like the actual circuit. Thanks for looking into
this and getting a fix up so quickly.

- John


_________________________________________________

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

desktop!

I know that I can create my own library files and use .include
to specify them. But is it possible to extend the dialog box
list for the NPN transistors, for example, so that I can simply
select from the list rather than overriding the "Value" on the
schematic, directly? It's nice to look over the parameter list,
sometimes, to look for the best of some particular parameter,
without having to print out my library file.

And if there is a way, can it be secure against the automatic
update process, so that I keep my additions in the face of
regular updates?

Or if I should decide to forget about the standard components
included with LT Spice and start building my own large library
of parts with trusted parameters, can I get them to be popped
into these selection lists?

Jon

John,

I was really puzzled by the complicated G-
source _expression. That all makes sense now.

Yeah. I just put up a version, 2.00l. It lets you
duplicate the leakage of PSpice current sources in
LTspice. Go to Tools=>Control Panel=>SPICE and
check "Add GMIN across current sources" Then you
will see the input bias drop to zero on the -E
models.

There's still a couple differences between PSpice
and LTspice even after checking the box. PSpice
does not report the current's gmin leakage current,
which is just a dumb mistake that I don't
duplicate. Also, in PSpice the current sources
don't leak in the .ac analysis, just .op and .tran.
Which is a complete inconsistency and just another
error I didn't duplicate in LTspice.

There's one other thing to keep in mind when
working with high impedance circuits. You might
want to tighten abstol. That controls the
absolute(vs. relative) acceptable current
error. It defaults to 1pA.

--Mike

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

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

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

Mike,

I was really puzzled by the complicated G-source expression. That
all makes sense now.

Thanks,
John

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

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.

The golden rule in analogue design is that n simulators give n different
answers, you have to be able to hand-verify results to some extent.

I tell the engineers here, half-jokingly that simulation tools and models are
for amusement only since both the tool and device vendors don't guarantee the
accuracy of anything.

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.
***

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