¿ªÔÆÌåÓý

Date

Re: Opamp models from Texas Instruments

 

Sven,

The simulation ( transient analysis )with the AD8009
works as expected. But the THS4271 produces just junk.
After some 500 ps the output will be some Megavolts.
The AC analysis on the other hand looks ok.
It looks like the problem is in the model. I ran the
model in PSpice 9.2.3, the most recent version of the
target simulator of the model, and got the same results.
Here is a netlist based on your circuit that you can run
in either LTspice or PSpice. I removed the power source
impedances because PSpice doesn't handle those as part of
voltage sources.

You'll have to pick a different opamp or contact TI
about the error in the model. Good luck.

* THS4271.asc
R1 N001 0 100
R2 out N001 100
V1 N005 0 PULSE(0 1 0 0.1n 0.1n 10n 20n)
V2 0 N003 5
V3 N002 0 5
R3 N004 N005 0.1
XU1 N004 N001 N002 N003 out THS4271
.tran 0 20n 0
.inc TI.lib
.probe
.end

--Mike

__________________________________
Do you Yahoo!?
SBC Yahoo! DSL - Now only $29.95 per month!


No files were attached

 

Hello,

my attached files did't appear, so I try to add then
to this post.

Thank you again for any help.

Sven Hegewisch




The library:

AD8009 SPICE model Rev B SMR/ADI 8-21-97

* Copyright 1997 by Analog Devices, Inc.

* Node assignments
* non-inverting input
* | inverting input
* | | positive supply
* | | | negative supply
* | | | | output
* | | | | |
.SUBCKT AD8009 1 2 99 50 28

* input stage *

q1 50 3 5 qp1
q2 99 5 4 qn1
q3 99 3 6 qn2
q4 50 6 4 qp2
i1 99 5 1.625e-3
i2 6 50 1.625e-3
cin1 1 98 2.6e-12
cin2 2 98 1e-12
v1 4 2 0

* input error sources *

eos 3 1 poly(1) 20 98 2e-3 1
fbn 2 98 poly(1) vnoise3 50e-6 1e-3
fbp 1 98 poly(1) vnoise3 50e-6 1e-3

* slew limiting stage *

fsl 98 16 v1 1
dsl1 98 16 d1
dsl2 16 98 d1
dsl3 16 17 d1
dsl4 17 16 d1
rsl 17 18 0.22
vsl 18 98 0

* gain stage *

f1 98 7 vsl 2
rgain 7 98 2.5e5
cgain 7 98 1.25e-12
dcl1 7 8 d1
dcl2 9 7 d1
vcl1 99 8 1.83
vcl2 9 50 1.83

gcm 98 7 poly(2) 98 0 30 0 0 1e-5 1e-5

* second pole *

epole 14 98 7 98 1
rpole 14 15 1
cpole 15 98 2e-10

* reference stage *

eref 98 0 poly(2) 99 0 50 0 0 0.5 0.5

ecmref 30 0 poly(2) 1 0 2 0 0 0.5 0.5

* vnoise stage *

rnoise1 19 98 4.6e-3
vnoise1 19 98 0
vnoise2 21 98 0.53
dnoise1 21 19 dn

fnoise1 20 98 vnoise1 1
rnoise2 20 98 1

* inoise stage *

rnoise3 22 98 8.18e-6
vnoise3 22 98 0
vnoise4 24 98 0.575
dnoise2 24 22 dn

fnoise2 23 98 vnoise3 1
rnoise4 23 98 1

* buffer stage *

gbuf 98 13 15 98 1e-2
rbuf 98 13 1e2

* output current reflected to supplies *

fcurr 98 40 voc 1
vcur1 26 98 0
vcur2 98 27 0
dcur1 40 26 d1
dcur2 27 40 d1

* output stage *

vo1 99 90 0
vo2 91 50 0
fout1 0 99 poly(2) vo1 vcur1 -9.27e-3 1 -1
fout2 50 0 poly(2) vo2 vcur2 -9.27e-3 1 -1
gout1 90 10 13 99 0.5
gout2 91 10 13 50 0.5
rout1 10 90 2
rout2 10 91 2
voc 10 28 0
rout3 28 98 1e6
dcl3 13 11 d1
dcl4 12 13 d1
vcl3 11 10 -0.445
vcl4 10 12 -0.445

.model qp1 pnp()
.model qp2 pnp()
.model qn1 npn()
.model qn2 npn()
.model d1 d()
.model dn d(af=1 kf=1e-8)
.ends

* [Disclaimer] (C) Copyright Texas Instruments
Incorporated 1999 All rights reserved
*
* THS4271 High Speed amplifier "macromodel" subcircuit
* updated using Model Editor release 9.2 on 11/05/02
at 13:11
* The Model Editor is a PSpice product.
*
* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
*$
.subckt THS4271 1 2 3 4 5

*Offset and CMRR
Vos 1a 9 .005
Ios 1 2 .5u

* upper Vic range limit
drc1 16 17 dx
drc2 16 18 dx
Vcp 3 16 dc -0.4

* input stage
rc1 17 11 176.8
rc2 18 12 176.8
L- 2 2a .8n
q1 11 2a 13 qx1
L+ 1 1a .8n
q2 12 9 14 qx1
re1 13 10 159.07
re2 14 10 159.07
Cdif 1 1c 0.8p
Rcdf 1c 2 50
Ccm 2 2b 0.4p
Rccm 2b 99 50

* lower Vic range limit
d10 15 10 dx
v10 15 4 dc 1.2
Iee 10 4 dc 3e-3
Icc 3 4 15m
Rcc 3 4 2500

* gain stage and dominant pole
Ga 21 99 value =
{(limit(V(11,12),-.447,.447))*-35.6m}
ra 21 99 158k
ca 21 99 15.9E-12

* GAIN STAGE SWING LIMIT
DPC 21 23 dx
VPC 3 23 1.7
DNC 24 21 dx
VNC 24 4 1.74

* zero
ez 26 99 21 99 10
rz1 26 27 -900
cz 26 27 .2p
rz2 27 99 -100

* phase shift stage
gps 25 99 27 99 -100.0E-6
rps 25 99 10.0E3
cps 25 99 10E-15

Egnd 99 0 poly(2) 3 0 4 0 0 .5 .5
X_OP 25 99 3 4 5a THS4271_OP
Ro 5a 5b .1
Lo 5b 5 .2n
Rco 5c 99 10
Co 5 5c .8p

.ends
*$

* Output stage
* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
.subckt THS4271_OP 1 2 3 4 5
* GAIN STAGE SWING LIMIT
DOPC 1 38 dx
VOPC 3 38 1.
DONC 48 1 dx
VONC 48 4 1.

* UPPER DRIVE STAGE
ROP 3 34 8.5
HLP2 34 33 VLP 30
VOP 33 32 0
HLP1 35 0 VOP 8
RLP 35 36 8
DLP 36 37 dx
VLP 37 0 0
EOP 32 31 Poly(2) 2 1 3 4 -.8 1 .5
DOP 31 5 dx

* LOWER DRIVE STAGE
DON 5 41 dx
EON 41 42 Poly(2) 1 2 3 4 -.8 1 .5
VON 42 43 0
HLN1 45 0 VON 15
RLN 45 46 8
DLN 46 47 dx
VLN 47 0 0
HLN2 43 44 VLN 45
RON 44 4 12

.ends
*$
*DIODE MODELS
.model dx D(Is=800.00E-18)
*$
.model qx1 NPN(Is=800.00E-18 Bf=272.73 af=0 kf=9e-22)
*.model qx1 NPN(Is=800.00E-18 Bf=272.73 af=2 kf=8e-8)
*$

Please note that the disclaimers and copyright notices
are shorted!


The circuit with AD8009:

Version 4
SHEET 1 880 680
WIRE -320 176 -80 176
WIRE -80 80 -80 176
WIRE -80 176 0 176
WIRE 0 80 144 80
WIRE 144 80 144 192
WIRE 144 192 64 192
WIRE 144 192 240 192
WIRE 32 160 32 144
WIRE 32 352 32 336
WIRE 240 192 288 192
WIRE -80 208 0 208
WIRE -224 288 -224 208
WIRE -224 208 -160 208
WIRE 192 336 192 320
WIRE 192 432 192 416
WIRE 32 240 32 224
FLAG -320 256 0
FLAG -224 368 0
FLAG 32 432 0
FLAG 192 320 0
FLAG 240 192 out
FLAG 32 144 v+
FLAG 192 432 v+
FLAG 32 240 v-
FLAG 32 336 v-
SYMBOL res -336 160 R0
SYMATTR InstName R1
SYMATTR Value 100
SYMBOL res 16 64 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R2
SYMATTR Value 100
SYMBOL voltage -224 272 R0
WINDOW 123 24 132 Left 0
WINDOW 39 0 0 Left 0
WINDOW 3 -402 89 Left 0
SYMATTR Value2 AC 0.1
SYMATTR Value PULSE(0 1 0 0.1n 0.1n 10n 20n 1)
SYMATTR InstName V1
SYMBOL voltage 32 448 R180
WINDOW 0 24 104 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 24 -12 Left 0
SYMATTR InstName V2
SYMATTR Value 5
SYMATTR SpiceLine Rser=0.1
SYMBOL voltage 192 432 R180
WINDOW 0 24 104 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 24 76 Left 0
SYMATTR InstName V3
SYMATTR Value 5
SYMATTR SpiceLine Rser=0.1
SYMBOL res -64 192 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R3
SYMATTR Value 0.1
SYMBOL Opamps\\AD8009 32 128 R0
SYMATTR InstName U1
TEXT -226 506 Left 0 !.tran 0 20n 0


The circuit with THS4271:


Version 4
SHEET 1 880 680
WIRE -320 176 -80 176
WIRE -80 80 -80 176
WIRE -80 176 0 176
WIRE 0 80 144 80
WIRE 144 80 144 192
WIRE 144 192 64 192
WIRE 144 192 240 192
WIRE 32 160 32 144
WIRE 32 352 32 336
WIRE 240 192 288 192
WIRE -80 208 0 208
WIRE -224 288 -224 208
WIRE -224 208 -160 208
WIRE 192 336 192 320
WIRE 192 432 192 416
WIRE 32 240 32 224
FLAG -320 256 0
FLAG -224 368 0
FLAG 32 432 0
FLAG 192 320 0
FLAG 240 192 out
FLAG 32 144 v+
FLAG 192 432 v+
FLAG 32 240 v-
FLAG 32 336 v-
SYMBOL res -336 160 R0
SYMATTR InstName R1
SYMATTR Value 100
SYMBOL res 16 64 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R2
SYMATTR Value 100
SYMBOL voltage -224 272 R0
WINDOW 123 24 132 Left 0
WINDOW 39 0 0 Left 0
WINDOW 3 -402 89 Left 0
SYMATTR Value2 AC 0.1
SYMATTR Value PULSE(0 1 0 0.1n 0.1n 10n 20n 1)
SYMATTR InstName V1
SYMBOL voltage 32 448 R180
WINDOW 0 24 104 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 24 -12 Left 0
SYMATTR InstName V2
SYMATTR Value 5
SYMATTR SpiceLine Rser=.1
SYMBOL voltage 192 432 R180
WINDOW 0 24 104 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 24 76 Left 0
SYMATTR InstName V3
SYMATTR Value 5
SYMATTR SpiceLine Rser=.1
SYMBOL res -64 192 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R3
SYMATTR Value 0.1
SYMBOL Opamps\\THS4271 32 128 R0
SYMATTR InstName U1
TEXT -226 506 Left 0 !.tran 0 20n 0


________________________________________________________________________
Send free SMS using the Yahoo! Messenger. Go to


Opamp models from Texas Instruments

 

Hello,

first let me than you for this nice program.

I am rather new to simulation programs so I ran into
some
difficulties.

I try to simulate a small circuit with two different
opamps, the AD8009 from Analog Devices and the THS4271
from Texas Instruments. I downdloaded both models from
the net and made a library with them which I put in
the
standard library folder.

The simulation ( transient analysis )with the AD8009
works as expected.
But the THS4271 produces just junk. After some 500 ps
the output will be some Megavolts.
The AC analysis on the other hand looks ok.

After several days of try and still error I don't know
what I am doing wrong.

Every help will be appreciated.

The circuits have the filenames THS4271t.asc and
AD8009t.asc
and the library has the name opa.lib.
They are attached to this post.

Thank you

Sven Hegewisch


________________________________________________________________________
Send free SMS using the Yahoo! Messenger. Go to


Re: Rotating components when placing in schematic

Howie, Brian (UK)
 

In Eagle (by CadSoft) I can rotate components by clicking the right
mouse button before placing. Would be a nice feature in LTSpice, too.

Greeting from Germany

Michael

Control R does it.

Brian

***
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.
***


Rotating components when placing in schematic

telyn_de
 

Hello,

my name is Michael and I'm designing stage control systems for
theaters, opera houses etc.

I've been using LTSpice only for a few days by now (after been
completely unsatisfied with CircuitMaker 5 schematic editor).

Now my question:
Is there any easy way (other than clicking the Rotate Button) to
rotate components when placing ?

In Eagle (by CadSoft) I can rotate components by clicking the right
mouse button before placing. Would be a nice feature in LTSpice, too.

Greeting from Germany

Michael


Re: What does 'Fatal Error: doAnalyses: Iteration limit reached' mean?

 

Massimo,

Please can you report some additional information about the alternate
solver? Which are the main differences between the two solvers?

Is it possible to understand why you have added this new solver? Are
there some limitations in the old one? Which are the circuits in which
the new solvers is more accurate?
The alternate solver uses a sparse matrix package that
accumulates much less internal round-off error. The new
sparse solver uses (what I call) a vertical solution method.
It runs at about half the simulation speed but 1000x more
accurately as far as the matrix solution goes in the test
cases that caused the investigation.

For practical circuits, there's no need for it. But some
opamp macro models use unphysical components that lead to a
difficult-to-solve linearized circuit matrix. I found three
ways to solve the problem, but only released the method to
use a more accurate sparse matrix solver that has less round-
off error because (i) it was of the most general use and (ii)
it's the hardest for other SPICE programs to duplicate. This
also gives a nice diagnostic that allows one to check if
numerical round-off is an issue by switching between solvers.
I think it's an interesting, very high-power means to solve
the problem and I don't know of any other SPICE in academia
or commerce that uses this vertical solution technology.
Intellectual property concerns don't allow me to feel
comfortable revealing the theory behind the implementation,
but you should find the operation to be exactly as I describe.

Besides the sparse matrix solver, there is no other intended
difference between the two SPICE solvers in the current
release. There's basically two copies of LTspice in the
executable because the new matrix solver is not compatible
with the old one so a copy of LTspice had to be modified to
work with it.

Anyway, I recommend only using the normal solver unless you
run into singular matrix issues. The normal solver usually
will be just as accurate as the alternate solver since round-
off error in the sparse matrix is rarely the limiting factor
to the accuracy of your circuit's solution. If you develop
macro models for others to use in possibly other simulators,
I definately recommend that you use the normal solver, or
could end up with a model that only LTspice can solve.

But of course I appreciate people testing both solvers and
reporting any un-intended differences between them. It was
a huge reorganization of the code to have two versions of
LTspice in the same executable. I find the feedback I
get from this, other groups, and individually extremely
valuable to the quality of the program.

--Mike

__________________________________
Do you Yahoo!?
SBC Yahoo! DSL - Now only $29.95 per month!


Re: What does 'Fatal Error: doAnalyses: Iteration limit reached' mean?

 

Dear Mike,

Please can you report some additional information about the alternate solver? Which are the main differences between the two solvers?

Is it possible to understand why you have added this new solver? Are there some limitations in the old one? Which are the circuits in which
the new solvers is more accurate?

Thanks

Massimo

Panama Mike wrote:

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.
--

''~``
( o o )
+------------------.oooO--(_)--Oooo.------------------+
| |
| e-mail: gaspari@... |
| |
| ICQ # = 166939207 |
| |
| PGP fingerprint16: |
| 76 80 F2 F9 8D 70 F3 D1 42 2B CD 80 29 49 CB 25 |
| |
| .oooO |
| ( ) Oooo. |
+---------------------\ (----( )--------------------+
\_) ) /
(_/


Re: Symbol Creation

Steve Steckler
 

Thanks Mike

Panama Mike wrote:
Steve,

> 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.

Thank you very much for reporting this.? The fix will be availible
when the next minor update is released.

--Mike

__________________________________
Do you Yahoo!?
SBC Yahoo! DSL - Now only $29.95 per month!



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



Your use of Yahoo! Groups is subject to the .


Do you Yahoo!?
- Now only $29.95 per month!


Re: Symbol Creation

 

Steve,

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.
Thank you very much for reporting this. The fix will be availible
when the next minor update is released.

--Mike

__________________________________
Do you Yahoo!?
SBC Yahoo! DSL - Now only $29.95 per month!


Re: Models for BB INA111AP

D Chisholm
 

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:

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


Re: Models for BB INA111AP

 

--- 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


Re: Models for BB INA111AP

Jonathan Kirwan
 

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


Models for BB INA111AP

 

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


Re: Oscillator

Al Williams
 

--- 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.


Re: Oscillator

 

--- 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)}


Re: Pierce Oscillator

Al Williams
 

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


Pierce Oscillator

leckerts
 

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


Oscillators

leckerts
 

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.


Re: Oscillator

Al Williams
 

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


Re: Spice model for 2SD2006, .......

manduur2000
 

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>