开云体育

Andre,

makes me wonder if there is any way to start a
transient simulation, stop at some predefined
point in time and use that result for the ac
simulation.

No this isn't possible in LTspice. It's pretty
hard to implement. What you can do, to help
with your confidence in the solution from a .ac
analysis, is to do a .step set of runs that
varies some aspect of the dc operating point
and see if the .ac small signal transfer function
looks the same for all those slightly different
.op points.

I had that problem too, but in my
designs i almost only rely on transient
simulation (for the exact same reason that you
mentioned above and because large signals
change the operating point anyways).

Yes, e.g., power amplifier stability is really
difficult to do reliably in small signal .ac
analysis. The open loop gain/phase varies
wildly with output stage operating point.
One method that helps in this situation is to
drive the amp to one end or the other with a DC
input source and insert a floating AC source
in the loop in front of a high impedance
point for an .ac analysis. The open
loop transfer function can be obtained from
the ratio of voltages to either side of the
floating source.

But ultimately, the .tran analysis comes
out at the ultimate SPICE test of stability.

Best Regards,

--Mike

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

Hi Mike,

Helmut,

[...]I have read in a book? that .TRAN analysis
always does converge better.

Hello Mike, is that true?[...]

The .tran solution is always more believable
than the .op solution. SPICE programs are
prone to "false convergence", a numerical
situation in which the error-based checks
accept an answer which is nonsense. This
can happen once and through off a .op
solution, but it *rarely* will happen
repeatably in the .tran solution.

The .ac solution is thereby somewhat suspect
because it is based solely on the .op solution.

But as far as better convergence with respect
to giving up due to convergence errors(not
counting accepting false answers), the .tran
has only one advantage, it can start simulation
without a .op solution while the .ac cannot.
But normally both need the .op solution.
For the .ac analysis, there is basically
no further possibility of convergence failures
after the .op, because everything after that
is an exact solution of the linearized circuit.

--Mike

makes me wonder if there is any way to start a transient simulation,
stop at some predefined point in time and use that result for the ac
simulation. I had that problem too, but in my designs i almost only
rely on transient simulation (for the exact same reason that you
mentioned above and because large signals change the operating point
anyways).

Andre

the latest revision 2.01o now runs my test circuit
for the OPA336 without the 'gmin' hack, but the
line .OPTIONS gmin=1e-10 noopiter=1
is still necessary.

Yes, I was able to reduce gmin to 1e-11, though.

Was this change coming from the missed JFET
parameter?

Apparently so, now the MOSFET's leak more. BTW,
the model, since it uses current sources, should
probably be run with the "Add GMIN across current
sources" hack because the model was written for
PSpice.

From the notes written in the model, it looks
like PSpice had a hard time with it, too.

BTW, I'm thinking of introducing opamp models that
use a different modeling methodology, similar to
that used for LTspice's SMPS products. The result
would be computationally extremely lightweight and
robust models that model noise too(these PSpice-
style opamp models almost never get the noise
modeled). However, the opamps models would not
run in other SPICE simulators and non-LT opamp
models wouldn't be available. Would you folks be
interested in something like that?

--Mike

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

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

Helmut,

[...]I have read in a book? that .TRAN analysis
always does converge better.

Hello Mike, is that true?[...]

The .tran solution is always more believable
than the .op solution. SPICE programs are
prone to "false convergence", a numerical
situation in which the error-based checks
accept an answer which is nonsense. This
can happen once and through off a .op
solution, but it *rarely* will happen
repeatably in the .tran solution.

The .ac solution is thereby somewhat suspect
because it is based solely on the .op solution.

But as far as better convergence with respect
to giving up due to convergence errors(not
counting accepting false answers), the .tran
has only one advantage, it can start simulation
without a .op solution while the .ac cannot.
But normally both need the .op solution.
For the .ac analysis, there is basically
no further possibility of convergence failures
after the .op, because everything after that
is an exact solution of the linearized circuit.

Hello Mike,
the latest revision 2.01o now runs my test circuit for the OPA336
without the 'gmin' hack, but the line
.OPTIONS gmin=1e-10 noopiter=1
is still necessary.

Was this change coming from the missed JFET parameter?

Best Regards
Helmut

I wrote:

[...] I suggest either removing and asking
TI/Burr-Brown why the error is in the model.

but meant:

[...] I suggest either removing vfb=... from
the models or just ignoring the error message
and then asking TI/Burr-Brown why the error is
in the model.

--Mike

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

Helmut,

[...]I have read in a book? that .TRAN analysis
always does converge better.

Hello Mike, is that true?[...]

The .tran solution is always more believable
than the .op solution. SPICE programs are
prone to "false convergence", a numerical
situation in which the error-based checks
accept an answer which is nonsense. This
can happen once and through off a .op
solution, but it *rarely* will happen
repeatably in the .tran solution.

The .ac solution is thereby somewhat suspect
because it is based solely on the .op solution.

But as far as better convergence with respect
to giving up due to convergence errors(not
counting accepting false answers), the .tran
has only one advantage, it can start simulation
without a .op solution while the .ac cannot.
But normally both need the .op solution.
For the .ac analysis, there is basically
no further possibility of convergence failures
after the .op, because everything after that
is an exact solution of the linearized circuit.

--Mike

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

Steve,

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.

Here's the link to the TI page. Thanks

genericPartNumber=OPA336&pfsection=models

Thanks for the link. OK, here's the story.
Jssw is a perimeter-based bulk leakage current
parameter. The MOSFET models in the the macro
model are written such that the bulk leakage is
dominated by the source and drain perimeters,
not that I think that has much to do with the
overall behavior of the macromodel.

I have implemented jssw in LTspice and it is
now available now as version 2.01o. Thank
you very much for the test case that pointed it
out that jssw was missing.

However, Vfb is not a level 3 MOSFET parameter.
PSpice accepts it, but does apparently nothing
with it. LTspice will still complain, which is
okay I think because it is an error in the
model. I suggest either removing and asking
TI/Burr-Brown why the error is in the model.

--Mike

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

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

--- 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

Hello Steve,
the magic trick for the convergence problem in .AC analysis is the
latest 'gnin parallel current source' feature.
That was the only way I found to get convergence in .AC analysis for
this OPAMP.

Enable this feature in the control panel.
Control Panel->Hacks-> Add GMIN across current sorce
But this alone doesn't help. We have to add the command line
.OPTIONS gmin=1e-10 noopiter=1 into the schematic.

I have read in a book? that .TRAN analysis always does converge
better.

Hello Mike,
is that true?
Unfortunately this doesn't help anything when somebody has to make
a .AC analysis.

What's about this error message regarding JFET parameters?
Error on line 61 : .model nch nmos (level=3 tox=30e-9 cgdo=1.55e-10
cgso=1.55e-10 cj=6.300e-4 cjsw=3.83e-10 af=1.05 kf=2.6e-31 js=2.0e-7
jssw=5e-13 rsh=68 mj=.25 mjsw=.11 vfb=-0.784 phi=0.792 vto=.81 ld=34e-
9 wd=17e-9 tpg=-1 gamma=0.6)
Unrecognized parameter "jssw" - ignored
Unrecognized parameter "vfb" - ignored
Error on line 60 : .model pch pmos (level=3 tox=30e-9 cgdo=1.80e-10
cgso=1.80e-10 cj=7.199e-4 cjsw=3.40e-10 af=1.05 kf=1.0e-31 js=4.0e-7
jssw=3.0e-13 rsh=117 mj=.47 mjsw=.16 vfb=-0.34 phi=0.71 vto=-.892
ld=12e-9 wd=43e-9 tpg=+1 gamma=0.6)
Unrecognized parameter "jssw" - ignored
Unrecognized parameter "vfb" - ignored

I have my test files attached.

Best Regards
Helmut

The LTSPICE file for .AC analysis.

Version 4
SHEET 1 1372 1316
WIRE 320 320 320 352
WIRE 320 256 320 224
WIRE -16 368 -16 304
WIRE -16 96 80 96
WIRE 80 304 -16 304
WIRE 160 304 240 304
WIRE 160 96 240 96
WIRE 288 272 240 272
WIRE 240 272 240 96
WIRE 464 96 512 96
WIRE 512 96 512 288
WIRE 512 288 352 288
WIRE -16 480 -16 448
WIRE 240 480 240 512
WIRE 384 480 384 512
WIRE 240 592 240 624
WIRE 384 592 384 624
WIRE 512 288 544 288
WIRE 240 96 384 96
WIRE 240 304 288 304
WIRE 320 976 320 1008
WIRE 320 912 320 880
WIRE -16 752 96 752
WIRE 80 960 -16 960
WIRE 160 960 240 960
WIRE 160 752 240 752
WIRE 288 928 240 928
WIRE 240 928 240 752
WIRE 464 752 512 752
WIRE 512 752 512 944
WIRE 512 944 352 944
WIRE 512 944 544 944
WIRE 240 752 384 752
WIRE 240 960 288 960
WIRE -16 1024 -16 960
WIRE -16 1136 -16 1104
FLAG 320 224 Vcc
FLAG 240 480 Vcc
FLAG 384 480 Vss
FLAG 320 352 Vss
FLAG -16 480 0
FLAG 240 624 0
FLAG 384 624 0
FLAG 544 288 out
FLAG 240 96 in-
FLAG 240 304 in+
FLAG -16 96 0
FLAG 320 880 Vcc
FLAG 320 1008 Vss
FLAG 544 944 out1
FLAG 240 752 in1-
FLAG 240 960 in1+
FLAG -16 752 0
FLAG -16 304 in
FLAG -16 1136 0
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;x_models&#92;xopamp 320 224 R0
SYMATTR InstName U1
SYMATTR Value OPA336
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage 240 496 R0
SYMATTR InstName V1
SYMATTR Value 2.5
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage 384 496 R0
SYMATTR InstName V2
SYMATTR Value -2.5
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage -16 352 R0
WINDOW 123 24 132 Left 0
WINDOW 39 0 0 Left 0
SYMATTR Value2 AC 1
SYMATTR InstName V3
SYMATTR Value 1
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;res 368 112 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R1
SYMATTR Value 1MEG
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;res 64 320 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R2
SYMATTR Value 1MEG
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;res 64 112 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R3
SYMATTR Value 1MEG
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;x_models&#92;xopamp 320 880 R0
SYMATTR InstName U2
SYMATTR Value OPA336
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;res 368 768 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R4
SYMATTR Value 1MEG
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;res 64 976 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R5
SYMATTR Value 1
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;cap 96 768 R270
WINDOW 0 32 32 VTop 0
WINDOW 3 0 32 VBottom 0
SYMATTR InstName C1
SYMATTR Value 1
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage -16 1008 R0
WINDOW 123 24 132 Left 0
WINDOW 39 0 0 Left 0
SYMATTR Value2 AC 1
SYMATTR InstName V4
SYMATTR Value 0
TEXT -432 40 Left 0 ;.op
TEXT -432 -128 Left 0 !.include opa336.mod
TEXT -440 -160 Left 0 !.AC DEC 100 1 100MEG
TEXT -432 -40 Left 0 !.nodeset V(out)=2 V(in-)=1 V(in+)=1
TEXT -400 1256 Left 0 ;.OPTIONS vntol=1e-2 reltol=1e-2 itl1=500
itl2=500 itl6=500 abstol=1e-4 gmin=1e-9 gminsteps=100 noopiter=1
pivtol=1e-6
TEXT -432 -8 Left 0 !.nodeset V(out1)=0 V(in1-)=0 V(in1+)=0
TEXT -432 -88 Left 0 !.OPTIONS gmin=1e-10 noopiter=1
TEXT -400 1288 Left 0 ;.OPTIONS itl1=500 itl2=500 itl6=500 vntol=1e-
3 abstol=1e-12 reltol=1e-3 trtol=1 pivtol=1e-13 pivrel=1e-3 gmin=1e-
12 gminsteps=100 noopiter=1







The model OPA336.mod:
Be carefully with the broken lines I see in this awful YAHOO-editor.


* -------------------------------------------------------------------
-----
* | NOTICE: THE INFORMATION PROVIDED HEREIN IS BELIEVED TO BE
RELIABLE; |
* | HOWEVER; BURR-BROWN ASSUMES NO RESPONSIBILITY FOR INACCURACIES
OR |
* | OMISSIONS. BURR-BROWN ASSUMES NO RESPONSIBILITY FOR THE USE OF
THIS |
* | INFORMATION, AND ALL USE OF SUCH INFORMATION SHALL BE ENTIRELY
AT |
* | THE USER'S OWN RISK. NO PATENT RIGHTS OR LICENSES TO ANY OF
THE |
* | CIRCUITS DESCRIBED HEREIN ARE IMPLIED OR GRANTED TO ANY THIRD
PARTY. |
* | BURR-BROWN DOES NOT AUTHORIZE OR WARRANT ANY BURR-BROWN PRODUCT
FOR |
* | USE IN LIFE-SUPPORT DEVICES AND/OR
SYSTEMS. |
* -------------------------------------------------------------------
-----
*
*
*
* SUBCIRCUIT MACROMODEL OPA336
* PSpice ver. 6.3
* REV A. CREATED Wednesday, June 18, 1997 RH
* REV B. 25 JUNE 97 NPA: COMPILED INTO OPA336.MOD
* REV C. 26 JUNE 97 NPA: EDITED NODE SYNTAX AND ADDED .OPTION NOTES
*
* Notes concerning using macromodel to simulate OPA336:
* 1) Model is actually a simplified schematic of OPA336.
* 2) Model was created with PSpice ver. 6.3, level 3 device models.
* 3) Operation of the circuit is assumed to be single supply
*

* Example: X_U1 1 2 3 0 5 OPA336
*

* Where U is the subcircuit name and
* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
* .subckt OPA336 1 2 3 4 5
*
* Note that node "4" may be connected to ground "0", i.e., single
supply operation.
*
* 4) ADD .OPTION ITL=40 AND .OPTION GMIN=10p TO NET LIST IF
SIMULATION DOES NOT
* CONVERGE
* 5) ADDING .NODESET STATEMENT (BELOW) TO NET LIST MAY HELP
CONVERGENCE IS CASES
* WHERE V+=5V AND V-=0V ; SINGLE SUPPLY OPERATION. ASSUMES
SUBCIRCUIT IS "U1".
*
* .NODESET
* +V(2) = 2.5 V(1) = 2.5 V(5) = 2.5 V(3) = 5.0
* +V(X_U1.20)= 3.8 V(X_U1.23)= 3.8 V(X_U1.25)= .834 V(X_U1.27)
= .833 V(X_U1.29)= .834
* +V(X_U1.32)= 2.03 V(X_U1.34)= 2.03 V(X_U1.43)= 4.065 V(X_U1.44)=
2.51 V(X_U1.45)= 1.93
* +V(X_U1.47)= 1.93 V(X_U1.51)= .848 V(X_U1.53)= 4.07 V(X_U1.54)=
1.58 V(X_U1.55)= 4.02
* +V(X_U1.60)= 1.94 V(X_U1.62)= .855 V(X_U1.64)= 3.17 V(X_U1.67)=
4.98 V(X_U1.76)= 2.51
* +V(X_U1.GNDS)= 0.0 V(0)= 0.0
*
*
* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
.subckt OPA336 1 2 3 4 5
*
M61 4 64 55 55 PCH W=20U L=0.8U M=1
M59 55 53 3 3 PCH W=15U L=5U M=4
M55 55 60 51 GNDS NCH W=5U L=0.8U M=1
M53 53 45 51 GNDS NCH W=5U L=0.8U M=1
M57 53 53 3 3 PCH W=15U L=5U M=2
C55 55 60 CP1P2 2P
M67 55 55 67 3 PCH W=5U L=5U M=1
M74 45 51 62 GNDS NCH W=5U L=1U M=1
R67 3 67 RNW 200K
R47 45 47 RPO2 2K
ITAIL 3 23 DC 6U AC 0
ITAIL2 27 4 DC 1.6U AC 0
ITAIL3 51 4 DC 0.8U AC 0
I60 3 60 DC 0.4U AC 0
RGNDS GNDS 4 0.01
M24 29 1 23 3 PCH W=90U L=2U AD=2560P PD=3328U AS=2688P
PS=3494U M=1
M26 29 27 4 GNDS NCH W=500U L=2U AD=1142P PD=1670U AS=1142P
PS=1670U M=1
I20 20 4 DC 1U AC 0
R20 3 20 1.2MEG
M20 4 20 23 3 PCH W=5U L=2U M=1
R32 32 25 1.2MEG
R34 34 29 1.2MEG
I34 3 34 DC 1U AC 0
I32 3 32 DC 1U AC 0
V64 3 64 DC 1.8302
V60 60 62 DC 1.0897
V62 62 4 DC .8547
M23 25 2 23 3 PCH W=90U L=2U AD=2560P PD=3328U AS=2688P
PS=3494U M=1
M47 43 43 3 3 PCH W=60U L=4U M=1
M43 43 34 27 GNDS NCH W=4U L=4U M=1
M45 45 32 27 GNDS NCH W=4U L=4U M=1
M73 76 51 4 GNDS NCH W=5U L=0.8U M=20
M25 25 27 4 GNDS NCH W=500U L=2U AD=1142P PD=1670U AS=1142P
PS=1670U M=1
M71 76 55 3 3 PCH W=20U L=0.8U M=20
M49 45 43 3 3 PCH W=60U L=4U M=1
RC1 44 76 RPO2 10K
R76 76 5 RPO2 100
CM1 29 44 CP1P2 200P
C45 47 76 CP1P2 22P
RC2 54 4 RPO2 10K
CM2 25 54 CP1P2 200P
.ENDS
* MODELS for LEVEL 3 PSpice
*
.MODEL PCH PMOS (LEVEL=3 TOX=30E-9 CGDO=1.80e-10 CGSO=1.80e-10
CJ=7.199E-4 CJSW=3.40E-10
+AF=1.05 KF=1.0e-31 JS=4.0e-7 JSSW=3.0e-13 RSH=117 MJ=.47 MJSW=.16
VFB=-0.34 PHI=0.71 VTO=-.892
+LD=12E-9 WD=43E-9 TPG=+1 GAMMA=0.6)

.MODEL NCH NMOS (LEVEL=3 TOX=30E-9 CGDO=1.55e-10 CGSO=1.55e-10
CJ=6.300E-4 CJSW=3.83E-10
+AF=1.05 KF=2.6e-31 JS=2.0e-7 JSSW=5e-13 RSH=68 MJ=.25 MJSW=.11 VFB=-
0.784 PHI=0.792 VTO=.81
+LD=34E-9 WD=17E-9 TPG=-1 GAMMA=0.6)

.MODEL RPO2 RES (R=1 TC1=6.3e-4 TC2= 1.1e-6)
.MODEL RNW RES (R=1 TC1=5.5e-3 TC2=-1.3e-5)
.MODEL CP1P2 CAP (C=1)
*.ENDS
*.ENDS OPA336
*

--- 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