开云体育

I have models for the INA111 from an old Burr-Brown databook (pre-Texas Instruments). They seem to have produced 3 versions: a Basic model, called ".SUBCKT INA111/BB"; an "Enhanced" model, called ".SUBCKT INA111E/BB"; and another enhanced model called ".SUBCKT INA111Z/BB". About 30K bytes (over 500 lines) altogether for the 3. These are probably the same models you will get from TI, but I assembled them into a single file & posted to this group under the "Files>Lib>Sub" heading.

p.s. - You might still find the whole collection of Burr-Brown models at <ftp://nyquist.ee.ualberta.ca/pub/cookbook/spice/> or some other site that actually archives files, rather than linking to the manufacturer's current web pages.

Hao Fu wrote:

--- In LTspice@..., "Hao Fu" <fuhao@y...> wrote:

Hi,

It seems that this device is not among the existing examples in
LTspice. This device is primarily used for medical instrumentation
and data acquisition. Can someone tell me what it takes to make a
custom model for it? What is the minimum number of parameters from
its data sheet that should be taken into account?

Hello Hao,
there is a SPICE model on the TI website. Nobody would do the work on
it a second time.


genericPartNumber=INA111




genericPartNumber=INA111&pfsection=models


The only thing you need now is a symbol for LTSPICE. Take care to
number the value of "Netlist order" according to the parameter order
in the subcircuit definition of the model file.
Now some hints about file organization depending on the value
of "SpiceModel" in the symbol file.
If you reference the "SpiceModel" with a file name without path, then
this model file has to be either in the LTSPICE "...&#92;Lib&#92;Sub"
directory or in the working directory of your schematic file(*.asc).
If you specify a drectory path too("xyz&#92;abc.mod"), then it has to be
in "...&#92;Lib&#92;xyz&#92;abc.mod".

I have added the INA111 symbol, model and a test circuit under this
group's File->Lib directory.

You could read additionally my last posting about the INA103 model
and probably some of my earlier postings which also explain how to
make symbol files.

Overall it was not clear for me whether you have wanted to use the TI-
model or you try to make a model from the data sheet. I hope I could
help you.

Best Regards
Helmut

On Sun, 15 Jun 2003 07:52:24 -0000, you wrote:

It seems that this device is not among the existing examples in
LTspice. This device is primarily used for medical instrumentation
and data acquisition. Can someone tell me what it takes to make a
custom model for it? What is the minimum number of parameters from
its data sheet that should be taken into account?

I'm no expert on this, but it would seem that your needs would
depend on which model you can accept. There are three
Ebers-Moll models I'm familiar with, but the help file for
LTSpice only mentions "the Ebers-Moll." I guess it just depends
on which parameters you want to specify.

EM1 has an injection version, a transport version, and a
nonlinear hybrid-pi version. They use the forward beta (Bf),
reverse beta (Br), saturation current (Is, which is usually just
a hypothetical value designed to minimize errors against a
realistic curve of behavior), the nominal temperature (Tnom),
and the energy gap (Eg.) The energy gap is used to modify Is
over temperature.

For these parameters, you just need to look at a curve trace
which shows the collector current vs the collector-emitter
voltage for a fixed base-current drive. Select the Bf value
found on the desired I(B) curve at the point where I(C) and
V(CE) are at the values you intend to operate the transistor.
Use the DC value, not the AC value. Br can just be set to 1, if
you aren't going to operate it that way or else you can try and
find a curve with the emitter and collector leads interchanged
and pick off the right value for Br. Is is more complex. You
can use a numerical method for this, if you capture some
complete curves. But it is often just set to arbitrary values
like 1E-16 or else measured by considering a simple relationship
when the transistor is in the normal, active region and
zero-biased base-collector junction. In this case, you use the
standard Ebers-Moll equation, I(C)=I(S)*(e^((q*V(BE))/(k*T))-1),
and solve for I(S) (Is.) Eg is typically 1.11eV for silicon but
its often obtained by curve-fitting Is. This would probably
take some effort on your part, as the required information isn't
usually present on a data sheet for this. You might also steal
it from some similar transistor or else ignored if you assume
you will operate the transistor at the specified Is value.

EM2 uses EM1's parameters and adds the emitter ohmic resistance
(Re), the collector ohmic resistance (Rc), the base ohmic
resistance (Rb), the zero-bias emitter-base junction capacitance
(CJEO or CJE) and barrier potential and gradient factor, the
zero-bias collector-base junction capacitance (CJCO or CJC) and
barrier potential and gradient factor, the forward transit time
(Tf), the reverse transit time (Tr), and the substrate
capacitance (Csub). I think you'd need a curve tracer,
capacitance bridge, power supply, pulse generator, and a small
signal measurement system at a minimum. I don't think all these
can be fetched from a typical data sheet.

EM3 adds more, and so does Gummel-Poon. It gets really hairy at
this point.

My guess is that a data sheet is good for EM1, and even that is
only without really getting a good bead on Eg unless you
determine it by fiat. But like I said, I've only played around
with this a little bit with just a couple of unmarked
transistors, for the fun of it. I don't have good experience at
this. I'll be reading to see if someone can wisely point out
some good techniques for better modeling from data sheet curves.

Best of luck,
Jon

Hi,

It seems that this device is not among the existing examples in
LTspice. This device is primarily used for medical instrumentation
and data acquisition. Can someone tell me what it takes to make a
custom model for it? What is the minimum number of parameters from
its data sheet that should be taken into account?


Thanks,

Hao

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

--- In LTspice@..., "Al Williams" <alw@a...> wrote:

I put the ASC file in the Files section. The simulation time is
quite long, but it seemed to stablize around 30uS or so.

Hello Al,
I modified your oscillator circuit and added also some comments.
It is very important to have well defined settings for the

simulator.

Accidentally by far not all paramaters can be controlled from the
schematic or the netlist. This is a very bad drawback of LTSPICE.
I would appreciate to have commands for all simulator settings.

Setup the Simulator:
The points 1 to 4 are the most important actions.
1. Control Panel->Spice->Reset to Default
2. Control Panel->Hacks->Reset to Default
3. Control Panel Hacks->Supply a min. inductor damping->click off
4. Don't use integration method Gear. It tends to let die the
oscillation of this crystal oscillator.
5. Start your simulations with a lower Q of the crystal to reduce
turnaround time during development of your circuit.
Later you can increase Q and simulation time.

My new schematic file is in the Files->Examples->Educational Menu

too.

By the way, this is not the best type of one transistor oscillator
for 12Mhz. There are better suited circuits.

Thanks! I'm not sure where this file came from. I thought it was
installed as part of LTSpice, but maybe I got it somewhere else. It
isn't mine :-) I was simply trying to see if I could simulate it.

--- In LTspice@..., "Al Williams" <alw@a...> wrote:

I put the ASC file in the Files section. The simulation time is
quite long, but it seemed to stablize around 30uS or so.

Hello Al,
I modified your oscillator circuit and added also some comments.
It is very important to have well defined settings for the simulator.
Accidentally by far not all paramaters can be controlled from the
schematic or the netlist. This is a very bad drawback of LTSPICE.
I would appreciate to have commands for all simulator settings.

Setup the Simulator:
The points 1 to 4 are the most important actions.
1. Control Panel->Spice->Reset to Default
2. Control Panel->Hacks->Reset to Default
3. Control Panel Hacks->Supply a min. inductor damping->click off
4. Don't use integration method Gear. It tends to let die the
oscillation of this crystal oscillator.
5. Start your simulations with a lower Q of the crystal to reduce
turnaround time during development of your circuit.
Later you can increase Q and simulation time.

My new schematic file is in the Files->Examples->Educational Menu too.

By the way, this is not the best type of one transistor oscillator
for 12Mhz. There are better suited circuits.

Best Regards
Helmut

Pierce_12Mhz_r.asc:
You have to repair the two broken long lines with a text editor.
.TEXT 728 324 .....
.TEXT 728 524 .....
You can find this file in the Files->Examples->Educational folder too.


Version 4
SHEET 1 2020 1396
WIRE 1248 752 1280 752
WIRE 1344 752 1376 752
WIRE 1136 656 1136 752
WIRE 1328 1040 1136 1040
WIRE 1136 752 1136 1040
WIRE 1392 992 1392 960
WIRE 1392 960 1472 960
WIRE 1920 1232 1920 1344
WIRE 1920 1344 1568 1344
WIRE 1408 1344 1408 1376
WIRE 1440 1200 1440 1232
WIRE 1440 1344 1408 1344
WIRE 1344 1344 1408 1344
WIRE 1440 1136 1440 1104
WIRE 1440 1104 1392 1104
WIRE 1392 1104 1392 1088
WIRE 1344 1344 1136 1344
WIRE 800 960 800 1088
WIRE 640 1344 800 1344
WIRE 800 1344 944 1344
WIRE 944 960 800 960
WIRE 688 960 640 960
WIRE 640 960 640 1056
WIRE 800 1152 800 1344
WIRE 640 1136 640 1344
WIRE 944 1056 944 960
WIRE 944 1344 944 1248
WIRE 944 1136 944 1152
WIRE 1136 1040 1136 1136
WIRE 944 1152 944 1168
WIRE 1344 1216 1344 1344
WIRE 1344 1136 1344 1104
WIRE 1344 1104 1392 1104
WIRE 1232 656 1136 656
WIRE 1472 656 1296 656
WIRE 1136 752 1168 752
WIRE 1456 752 1472 752
WIRE 1472 752 1472 656
WIRE 800 960 768 960
WIRE 1232 960 944 960
WIRE 1312 960 1392 960
WIRE 1344 1056 1328 1056
WIRE 1328 1056 1328 1040
WIRE 1568 992 1568 960
WIRE 1568 960 1472 960
WIRE 1568 1056 1568 1104
WIRE 1568 1344 1440 1344
WIRE 1568 1216 1568 1344
WIRE 1568 1104 1568 1152
WIRE 1920 1104 1568 1104
WIRE 1920 1104 1920 1152
WIRE 1136 1200 1136 1344
WIRE 1136 1344 944 1344
WIRE 992 1152 992 1040
WIRE 992 1152 944 1152
WIRE 992 1040 1136 1040
WIRE 1472 960 1472 752
WIRE 1440 1312 1440 1344
FLAG 1408 1376 GND
FLAG 1920 1104 Output
SYMBOL voltage 640 1040 R0
SYMATTR InstName V1
SYMATTR Value 12
SYMBOL res 784 944 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R1
SYMATTR Value 100
SYMBOL res 960 1152 R180
WINDOW 0 36 76 Left 0
WINDOW 3 36 40 Left 0
SYMATTR InstName R2
SYMATTR Value 10k
SYMBOL res 960 1264 R180
WINDOW 0 36 76 Left 0
WINDOW 3 36 40 Left 0
SYMATTR InstName R3
SYMATTR Value 10k
SYMBOL cap 784 1088 R0
SYMATTR InstName C1
SYMATTR Value 100n
SYMBOL cap 1120 1136 R0
WINDOW 3 25 60 Left 0
SYMATTR InstName C2
SYMATTR Value 33p
SYMBOL res 1904 1136 R0
SYMATTR InstName R4
SYMATTR Value 50
SYMBOL ind 1264 736 R90
WINDOW 0 5 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName L0
SYMATTR Value {L0}
SYMBOL cap 1344 736 R90
WINDOW 0 0 32 VBottom 0
WINDOW 3 32 32 VTop 0
SYMATTR InstName C0
SYMATTR Value {C0}
SYMBOL cap 1296 640 R90
WINDOW 0 0 32 VBottom 0
WINDOW 3 32 32 VTop 0
SYMATTR InstName Cp
SYMATTR Value 5p
SYMBOL res 1472 736 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R0
SYMATTR Value {R0}
SYMBOL cap 1424 1136 R0
SYMATTR InstName C7
SYMATTR Value 10n
SYMBOL res 1328 1120 R0
SYMATTR InstName R6
SYMATTR Value 1k
SYMBOL res 1216 976 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R7
SYMATTR Value 1k
SYMBOL cap 1552 992 R0
SYMATTR InstName C9
SYMATTR Value 33p
SYMBOL cap 1552 1152 R0
SYMATTR InstName C10
SYMATTR Value 2.2n
SYMBOL res 1424 1216 R0
SYMATTR InstName R8
SYMATTR Value 1
SYMBOL npn 1328 992 R0
SYMATTR InstName Q1
SYMATTR Value 2N2369
TEXT 736 736 Left 0 !.tran 0 3m 0 0.005u
TEXT 736 768 Left 0 !.IC I(L0)=1e-24
TEXT 728 384 Left 0 ;Setup the Simulator:&#92;n1. Control Panel->Spice-

Reset to Default&#92;n2. Control Panel->Hacks->Reset to Default&#92;n3.

Control Panel Hacks->Supply a min. inductor damping->click off&#92;n4.
Don't use integartion method Gear. It tends to let die the
oscillation.&#92;n5. Start your simulations with a lower Q of the crystal
to reduce startup simulation time.
TEXT 728 584 Left 0 !.PARAM f0=12e6&#92;n.PARAM Q=50000&#92;n.PARAM R0=60
&#92;n.PARAM L0={Q*R0/(2*pi*f0)}&#92;n.PARAM C0={1/(2*pi*f0*Q*R0)}

That's strange. On my screen the Cs is 1.75fF not 250f and a .1H Ls.
I wonder if I have some file out of sync.

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

Al,

I just looked at the Pierce oscillator under the Educational
directory.

It has a 0.001 Henry series inductor and a 0.25 pF series

capacitor.

2/(2pi sqrt(.001 x .25x10-12)) = 10.07 MHz.

When I simulated the circuit I noticed that the output circuit
doubles the frequency of the oscillator. So twice 10.07 would be
20.14 MHz which is pretty close.

Steve

Al,

I just looked at the Pierce oscillator under the Educational
directory.

It has a 0.001 Henry series inductor and a 0.25 pF series capacitor.


2/(2pi sqrt(.001 x .25x10-12)) = 10.07 MHz.

When I simulated the circuit I noticed that the output circuit
doubles the frequency of the oscillator. So twice 10.07 would be
20.14 MHz which is pretty close.

Steve

Gentlemen,

I have simulated a lot oscillators in my day. I've used Cadence's
Spectre as well as LTSpice. Oscillators tend to be difficult to
simulate because of several factors. Very often, at higher
frequencies, you need to change the maximum time step or they won't
work at all. Also, you can usually speed up the startup of a crystal
oscillator by an order of magnitude by shocking the crystal resonator
with a pulsed current source. I noticed that it seems that the
maximum RAW file size of the LT simulator has been increased which is
important for oscillator simulations. It used to complain if the
simulation went too long and the file went over some limit.

Steve
Sr. Engineering Manager (Ex and looking)
TLSI Inc.

I put the ASC file in the Files section. The simulation time is
quite long, but it seemed to stablize around 30uS or so.

Al W.


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

--- In LTspice@..., "Al Williams" <alw@a...> wrote:

I was playing with pierce.asc -- as far as I can remember, this

was

a sample provided with the program (I think).

Doing a transient analysis on it shows that it oscillates at

21.114

MHz. Why is that? The quasi-crystal has L=.1, Rs=600, Cs=1.75fF,
Cp=5pF.

The series resonance should be 1/(2pi*sqrt(L*Cs))
Parallel resonance should be 1/2pi*sqrt(L*Cx))

where Cx=(Cs*Cp)/(Cs+Cp)

So Cx=1.749fF (almost no difference from Cs) and

Fs=12.031MHz
Fp=12.033MHz

External components might pull the crystal, but not to that

extent.

So is this a spice problem where other components are moving the
resonant frequency even though in real life it would not? Or am

I

missing something obvious?

Hello Al,
please post your circuit *.asc file and the subcircuit models if

any

used. I have simulated crystal oscillators in the past and they

did

run at the crystal frequency. Be aware of very long startup times.

Best Regards
Helmut

Hello D Chisholm,

thank you for data?s and the link. I?ve any other types.

regards,

Guenter


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

Fairchild will email a PSPICE model file for the TIP110. Request

it here:

<

file=TIP110.mod>

Hi Jon,

thanks for your help,

Guenter

--- In LTspice@..., "Al Williams" <alw@a...> wrote:

I was playing with pierce.asc -- as far as I can remember, this was
a sample provided with the program (I think).

Doing a transient analysis on it shows that it oscillates at 21.114
MHz. Why is that? The quasi-crystal has L=.1, Rs=600, Cs=1.75fF,
Cp=5pF.

The series resonance should be 1/(2pi*sqrt(L*Cs))
Parallel resonance should be 1/2pi*sqrt(L*Cx))

where Cx=(Cs*Cp)/(Cs+Cp)

So Cx=1.749fF (almost no difference from Cs) and

Fs=12.031MHz
Fp=12.033MHz

External components might pull the crystal, but not to that extent.
So is this a spice problem where other components are moving the
resonant frequency even though in real life it would not? Or am I
missing something obvious?

Hello Al,
please post your circuit *.asc file and the subcircuit models if any
used. I have simulated crystal oscillators in the past and they did
run at the crystal frequency. Be aware of very long startup times.

Best Regards
Helmut

I was playing with pierce.asc -- as far as I can remember, this was
a sample provided with the program (I think).

Doing a transient analysis on it shows that it oscillates at 21.114
MHz. Why is that? The quasi-crystal has L=.1, Rs=600, Cs=1.75fF,
Cp=5pF.

The series resonance should be 1/(2pi*sqrt(L*Cs))
Parallel resonance should be 1/2pi*sqrt(L*Cx))

where Cx=(Cs*Cp)/(Cs+Cp)

So Cx=1.749fF (almost no difference from Cs) and

Fs=12.031MHz
Fp=12.033MHz

External components might pull the crystal, but not to that extent.
So is this a spice problem where other components are moving the
resonant frequency even though in real life it would not? Or am I
missing something obvious?

What am I doing wrong?

Regards,

Al Williams

Fairchild will email a PSPICE model file for the TIP110. Request it here:
<>

Or try:
.SUBCKT TIP110 1 2 3
* TERMINALS: C B E
* Darlington NPN
Q1 1 2 4 QPWR .1
Q2 1 4 3 QPWR
R1 2 4 8K
R2 4 3 60
D1 3 1 DSUB
.MODEL QPWR NPN (IS=2.4P NF=1 BF=142 VAF=139 IKF=2.4 ISE=168P NE=2 BR=4 NR=1 VAR=20 IKR=3.6 RE=.45 RB=1.8 RC=.18 XTB=1.5 CJE=382P VJE=.74 MJE=.45 CJC=48.7P VJC=1.1 MJC=.24 TF=85.3N TR=3.68U)
.MODEL DSUB D (IS=2.4P N=1 RS=.45 BV=60 IBV=.001 CJO=48.7P TT=3.68U)
.ENDS


.MODEL Q2SC2655 NPN (IS=203F NF=1 BF=195 VAF=127 IKF=1.2 ISE=104P NE=2 BR=4 NR=1 VAR=20 IKR=1.8 RE=35.7M RB=.143 RC=14.3M XTB=1.5 CJE=220P VJE=1.1 MJE=.5 CJC=71P VJC=.3 MJC=.3 TF=1.59N TR=1.1U)

manduur2000 wrote:

On Sat, 14 Jun 2003 14:48:52 -0000, you wrote:

where can I find the spice model?s for these transistors:
2SD2006, 2SC2655, BC516, BC517, TIP110?

I found this:

.MODEL 2SC2655 NPN(
+ IS=8.8111E-15
+ BF=164
+ VAF=100
+ IKF=6.3687
+ XTB=1.5
+ ISE=68.197E-15
+ NE=1.4705
+ BR=10.573
+ VAR=100
+ IKR=91.376E-3
+ ISC=26.265E-12
+ NC=2.0018
+ NK=.4398
+ RC=47.627E-3
+ CJE=2.0000E-12
+ CJC=72.874E-12
+ MJC=.33333
+ TF=437.89E-12
+ XTF=10
+ VTF=10
+ ITF=1
+ TR=190.47E-9)

The others I don't have handy.

Jon

This is not a complaint, since we're all happy to have this tool!

Just an observation of a very minor issue that LT is probably aware
of -

When creating an IC symbol (I was drawing a 64-pin LQFP)and when
inserting pins which are vertically oriented, there are occasionally
trailing graphics when these pins are placed. I notice it usually
happens after 6 or 7 vertically oriented pins have been placed.

Keep up the great work!

Steve

Hello,
where can I find the spice model?s for these transistors:
2SD2006, 2SC2655, BC516, BC517, TIP110?

Thanks,

Guenter Koenig

Thank you very much Helmut for u time.
I am sorry that took too long. I was able to use INA 103 and learning
more. Still having problems in simulation .AC ....but more after i
try more..
Thanks once again
regards
ranga rajan

Besr Regards
Helmut

PS: This was a (too)very time consuming task for me. I hope you can
solve the other models yourself.

My changes:

* CONNECTIONS: NON-INVERTING INPUT
* | INVERTING INPUT
* | | POSITIVE POWER SUPPLY
* | | | NEGATIVE POWER SUPPLY
* | | | | OUTPUT
* | | | | | REFERENCE
* | | | | | | GAIN SENSE 1
* | | | | | | | GAIN SENSE 2
* | | | | | | | |
*.SUBCKT INA103 1 2 3 4 5 8 9 10
*** -RG +RG -GD +GD SNS

G100

.SUBCKT INA103 1 2 3 4 5 8 9 10 109 110 11 12 105

111

*** Change, add resistor for gain = 100, HS 6/8/2003
R910 109 111 60.6

*** Change, seperate connection SENSE, HS 6/8/2003
*R2 13 5 5.9994K
R2 13 105 5.9994K

*** Change, seperate connection -Rg, HS 6/8/2003
*R1FB 9 11 3.0000K
R1FB 109 11 3.0000K

*** Change, seperate connection +Rg, HS 6/8/2003
*R2FB 10 12 3.0000K
R2FB 110 12 3.0000K

I wrote:

...The fix is not yet in the general release
which is still Version 2.03f of May 23, 2003.
It's going to take another week or two before the
MOS3 fix make it into the general release because
that will also include the new sparse matrix solver.

But in the meanwhile, please try out this executable:

This MOS3 fix and the alternate solver with the new
sparse matrix package is now in the general release.
This makes the above mentioned url obsolete and no
longer available.

Version 2.03h implements a major reorganization of
most of the underlying code. Please report any
problems you might encounter as soon as you can.

--Mike

__________________________________
Do you Yahoo!?
Yahoo! Calendar - Free online calendar with sync to Outlook(TM).