Dosent seem to give logicale result or maybe this function is not
doing what I think it it should.

So what does it represent? -- not much different than normal data
apart that it is shifted around.

??I'm juts probably lost??

Mike,

Would it be possible to add the capability to do an efficiency
analysis on a circuit that doesn't use an LT switching regulator IC?
I've found this function to be very useful, but not all designs have
a switching regulator controller in them. It seems that all that is
needed is the ability to set a start and end time for the analysis.

This capability would also be helpful for circuits that use an LT
controller. Often the efficiency analysis requires the circuit to
settle for much longer than is really necessary. This isn't a
problem if the simulation takes less than a minute or so, but it's a
problem when it takes a half hour or more. Also, it would be useful
to be able to get power dissipation info during transient conditions
since many of the small parts I use heat up quite quickly.

Thanks,
John

Another issue I have is that some transistors are modelled as a
subcircuit rather than a plain model statement.
How -and where- do I add these?

There's different ways to handle this, but the cleanest way is
barely documented. What you can do is make a symbol that tells
the netlister which file to include whenever you place the
symbol on a schematic. Also, when you edit an instance of the
the symbol on the schematic you want to get a list of possible
models(subcircuits) from that file.

What you do is make a symbol with the symbol attribute "ModelFile"
set to the name of the file to include whenever you use the symbol.
Give this symbol an attribute of Prefix equal to "X". You should
also initialize the symbol attribute SpiceModel to be the name
of a subcircuit in the file. Attached are three files:

mybjtsubcircuits.lib: The file containing subcircuits that can
all be represented with the same symbol.

xpnpdarlings.asy: The symbol that knows about this library.

example.asc: A schematic uses the symbol.

You can put these files all in the same directory or put
the symbol with the usual symbol directory and the .lib
file in the /lib/sub directory. If you use an absolute
path name in the symbol for the library, you can put the
library whereever you wish.

Then open the example schematic and right click on the body
of the symbol. Then click on SpiceModel and the editor
is becomes a selection box of possible subcircuits from
the library.

--Mike

--- xpnpdarlings.asy ---
Version 4
SymbolType CELL
LINE Normal -25 0 -32 0
LINE Normal -25 16 -25 -16
LINE Normal -7 -22 -25 -8
LINE Normal -6 24 -25 9
LINE Normal -17 -17 -25 -8
LINE Normal -14 -13 -17 -17
LINE Normal -25 -8 -14 -13
LINE Normal -2 -22 -7 -22
LINE Normal -2 -6 -2 -38
LINE Normal 16 -44 -2 -30
LINE Normal 16 1 -2 -13
LINE Normal 6 -39 -2 -30
LINE Normal 9 -35 6 -39
LINE Normal -2 -30 9 -35
LINE Normal 16 32 16 1
LINE Normal 16 24 -6 24
LINE Normal 16 -48 16 -44
WINDOW 0 23 -32 Left 0
WINDOW 38 24 10 Left 0
SYMATTR Prefix X
SYMATTR Description Example of a symybol that automaticall includes a file and helps you select a
subcircuit in that file.
SYMATTR ModelFile mybjtsubcircuits.lib
SYMATTR SpiceModel 2N6042
PIN 16 32 NONE 0
PINATTR PinName C
PINATTR SpiceOrder 1
PIN -32 0 NONE 0
PINATTR PinName B
PINATTR SpiceOrder 2
PIN 16 -48 NONE 0
PINATTR PinName E
PINATTR SpiceOrder 3

--- mybjtsubcircuits.lib ---
*100V 8A PNP Darlington Transistor
.SUBCKT 2N6042 1 2 3
Q1 1 2 4 QMOD .1
Q2 1 4 3 QMOD
R1 2 4 8K
R2 4 3 120
D1 1 3 DMOD
.MODEL QMOD PNP(IS=9.6E-12 BF=96.6 VAF=180 IKF=4 ISE=6.41E-10 NE=2
+ BR=4 VAR=20 IKR=6 RB=0.2 RE=0.085 RC=0.063 CJE=1.65E-9 VJE=0.74 MJE=0.45
+ TF=1.4E-8 CJC=2.38E-10 VJC=1.1 MJC=0.24 TR=7E-7 VJS=0.75 XTB=1.5 )
.MODEL DMOD D(IS=9.6E-12 RS=0.05 TT=7E-7 CJO=2.38E-10 BV=100 )
.ENDS 2N6042

; dummy entry, you'd want ot put other PNP darlingtons
; with the same pin out here
.SUBCKT transistor2 1 2 3
Q1 1 2 4 QMOD .1
Q2 1 4 3 QMOD
R1 2 4 8K
R2 4 3 120
D1 1 3 DMOD
.MODEL QMOD PNP(IS=9.6E-12 BF=96.6 VAF=180 IKF=4 ISE=6.41E-10 NE=2
+ BR=4 VAR=20 IKR=6 RB=0.2 RE=0.085 RC=0.063 CJE=1.65E-9 VJE=0.74 MJE=0.45
+ TF=1.4E-8 CJC=2.38E-10 VJC=1.1 MJC=0.24 TR=7E-7 VJS=0.75 XTB=1.5 )
.MODEL DMOD D(IS=9.6E-12 RS=0.05 TT=7E-7 CJO=2.38E-10 BV=100 )
.ENDS 2N6042

.SUBCKT transistor3 1 2 3
Q1 1 2 4 QMOD .1
Q2 1 4 3 QMOD
R1 2 4 8K
R2 4 3 120
D1 1 3 DMOD
.MODEL QMOD PNP(IS=9.6E-12 BF=96.6 VAF=180 IKF=4 ISE=6.41E-10 NE=2
+ BR=4 VAR=20 IKR=6 RB=0.2 RE=0.085 RC=0.063 CJE=1.65E-9 VJE=0.74 MJE=0.45
+ TF=1.4E-8 CJC=2.38E-10 VJC=1.1 MJC=0.24 TR=7E-7 VJS=0.75 XTB=1.5 )
.MODEL DMOD D(IS=9.6E-12 RS=0.05 TT=7E-7 CJO=2.38E-10 BV=100 )
.ENDS 2N6042

--- example.asc ---

Version 4
SHEET 1 880 680
WIRE 144 336 144 320
WIRE 144 240 144 208
WIRE 144 208 304 208
WIRE 304 208 304 240
WIRE 32 400 32 384
WIRE 32 304 32 272
WIRE 32 272 96 272
WIRE 304 320 304 336
FLAG 304 336 0
FLAG 144 336 0
FLAG 32 400 0
SYMBOL xpnpdarlings 128 272 M180
WINDOW 0 31 8 Left 0
WINDOW 38 34 -20 Left 0
SYMATTR InstName U1
SYMBOL current 32 384 M180
WINDOW 0 24 88 Left 0
WINDOW 3 24 0 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName I1
SYMATTR Value 0
SYMBOL voltage 304 224 R0
SYMATTR InstName V1
SYMATTR Value 0
TEXT 32 448 Left 0 !.dc V1 0 -5 1m I1 0 -100u -10u


--- mathias.borcke@... wrote:

Meanwhile I found a couple of collections of Spice Models and I also
feel the need to organize them in some sort of user defined folder
structure.
The standard.bjt etc. to my opinion could remain untouched to allow the
web-update of the standard installation.
Big compliment to Mike Engelhardt regarding the update tool at this
point: I was completely stunned to figure out that those entries I had
added were still in there !!!

Another issue I have is that some transistors are modelled as a
subcircuit rather than a plain model statement.
How -and where- do I add these?

For example:

*100V 8A PNP Darlington Transistor
.SUBCKT 2N6042 1 2 3
Q1 1 2 4 QMOD .1
Q2 1 4 3 QMOD
R1 2 4 8K
R2 4 3 120
D1 1 3 DMOD
.MODEL QMOD PNP(IS=9.6E-12 BF=96.6 VAF=180 IKF=4 ISE=6.41E-10 NE=2
+ BR=4 VAR=20 IKR=6 RB=0.2 RE=0.085 RC=0.063 CJE=1.65E-9 VJE=0.74
MJE=0.45
+ TF=1.4E-8 CJC=2.38E-10 VJC=1.1 MJC=0.24 TR=7E-7 VJS=0.75 XTB=1.5 )
.MODEL DMOD D(IS=9.6E-12 RS=0.05 TT=7E-7 CJO=2.38E-10 BV=100 )
.ENDS 2N6042

* Origin: Mcebjt.lib



Or an IGBT:

**** Copyright Intusoft 1992 ****
* All Rights Reserved
* NL26 - IGBT Library
* 9/14/92
* Contents: 2 IGBT Models (Toshiba), 1 P-Channel, 1 N-Channel

*SYM=IGBT
.SUBCKT GT20D101 71 72 74
* TERMINALS: C G E
* 250 Volt 20 Amp 17.2NS N-Channel IGBT 09-15-1992
Q1 83 81 85 QOUT
M1 81 82 83 83 MFIN L=1U W=1U
DSD 83 81 DO
DBE 85 81 DE
RC 85 71 66.5M
RE 83 73 6.65M
RG 72 82 23.2
CGE 82 83 1.33N
CGC 82 71 1P
EGD 91 0 82 81 1
VFB 93 0 0
FFB 82 81 VFB 1
CGD 92 93 457P
R1 92 0 1
D1 91 92 DLIM
DHV 94 93 DR
R2 91 94 1
D2 94 0 DLIM
LE 73 74 7.5N
.MODEL QOUT PNP (IS=10.1F NF=1.2 BF=5.1 CJE=2.25N TF=17.2N XTB=1.3)
.MODEL MFIN NMOS (LEVEL=3 VMAX=221K THETA=80M ETA=4.81M VTO=3 KP=1.29)
.MODEL DR D (IS=1.01F CJO=457P VJ=1 M=.82)
.MODEL DO D (IS=1.01F BV=250 CJO=1.79N VJ=1 M=.7)
.MODEL DE D (IS=1.01F BV=14.3 N=2)
.MODEL DLIM D (IS=100N)
.ENDS

* Origin: IGBT.SUB



-----Ursprngliche Nachricht-----
Von: Jonathan Kirwan [mailto:jkirwan@...]
Gesendet: Donnerstag, 24. April 2003 19:47
An: LTspice@...
Betreff: Re: AW: [LTspice] Using ORCAD .lib files


On Thu, 24 Apr 2003 19:09:46 +0200, Mathias wrote:

No idea whether LTspice can handle this.

It's almost as though there may need to be a sub-folder
structure to allow some user-determined organization to the
"pick/select new transistor" dialog box. In other words, not a
flat list, but one which allows folders as well which can be
opened, as desired.

I personally think about importing models once I need these.

Yes, it's just a nifty resource at this point, where I can pull
what I need when I need it. On the other hand, if there is some
nice way to organize so many, I'd be happier to have them all at
my fingertips without having to exit, edit, save, and re-enter
LT Spice.

There's currently no folder structure possible for models in LTspice

and

therefore I'm concerned that I might loose the overview scrolling

through

thousands of files.

Yes. Hehe. But LT Spice does allow re-sorting on certain
criteria, though sadly not on the detailed spice parameters.

Can you be so kind to forward this link to me?

The one I found is:



e/PSPICE/
<
re/PSPICE/>

Jon



Yahoo! Groups Sponsor




<
pmail/S=:HM/A=1482387/rand=990924111>

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



Your use of Yahoo! Groups is subject to the Yahoo! Terms of Service
<> .

__________________________________
Do you Yahoo!?
The New Yahoo! Search - Faster. Easier. Bingo.

开云体育

开云体育

Thanks Mike

It's a useful facility to have so quickly! I'll try it out.

Regards,

Norbert.

How do you use the eye diagram function in swcad?

Add a SPICE directive like, ".options baudrate=250 delay=1.5m"
to the schematic. The eye diagram period will be 1/baudrate and the
phasing of the bits in the diagram will be shifted per the delay.
The delay can be changed after the simulation in the waveform
viewer, but the baudrate must be specified in the simulation.

--Mike


__________________________________
Do you Yahoo!?
The New Yahoo! Search - Faster. Easier. Bingo.

Hi,

How do you use the eye diagram function in swcad?

Norbert,

Some Spices print out a table of device operating
point information (e.g. device gm , gds, capacitances)
for things like mosfets and bipolar devices.

OK, I just released version 2.03b which starts to do
this. After running a .op simulation, do View=>SPICE
Error Log to see the results.

--Mike


__________________________________
Do you Yahoo!?
The New Yahoo! Search - Faster. Easier. Bingo.

Thanks for help on both topics,

Regards.

Norbert,

Does anybody have suggestions of how to use LTSpice in a
'batch' way, either from Windows or from Linux?

You can run a netlist in batch mode like this:

scad3.exe -b myfilename.cir

The waveform data will be in the file myfilename.raw
and the .log file will be in the file myfilename.log.

--Mike

__________________________________
Do you Yahoo!?
The New Yahoo! Search - Faster. Easier. Bingo.

Norbert,

Some Spices print out a table of device operating point
information (e.g. device gm , gds, capacitances) for
things like mosfets and bipolar devices.

Is this available in LTSpice?

Not at this time, but the request comes up now and again,
so I'll add it when I have time.

--Mike

__________________________________
Do you Yahoo!?
The New Yahoo! Search - Faster. Easier. Bingo.

Does anybody have suggestions of how to use LTSpice in a
'batch' way, either from Windows or from Linux?

I want to write a program loop to build an input netlist
file, submit it to LTSpice as a batch job, and pick out
results from the raw file.

Thanks in advance for any reply.

Some Spices print out a table of device operating point
information (e.g. device gm , gds, capacitances) for
things like mosfets and bipolar devices.

Is this available in LTSpice?

Regards,

Norbert.

Great, thanks!

Bill

--- Panama Mike <panamatex@...> wrote:

There's some new circuit topology checking in
version 2.02w to help diagnose these types of
problems. Floating nodes are now listed as
warnings in the .log file. Note not all floating
nodes listed are fatal LTspice errors. For
example, if you don't give a DC path to the gate
of a JFET, it will be listed as a floating node,
even though LTspice has no trouble computing the
voltage on the gate since it's not perfectly
floating.

The new error checking will also detect a loop of
voltage sources and/or inductors when there's
no Rser in the loop.

--Mike

--- Bill Lewis <wrljet@...> wrote:

Thank you so much.

How did you determine that? Or is this something I
should just know -- to leave nothing floating?

Bill

--- Panama Mike <panamatex@...> wrote:

Bill,

<snip>

The problem was that the filment supply was floating,
that is, its potential wasn't defined. The following
circuit fixed this:

__________________________________
Do you Yahoo!?
The New Yahoo! Search - Faster. Easier. Bingo.

There's some new circuit topology checking in
version 2.02w to help diagnose these types of
problems. Floating nodes are now listed as
warnings in the .log file. Note not all floating
nodes listed are fatal LTspice errors. For
example, if you don't give a DC path to the gate
of a JFET, it will be listed as a floating node,
even though LTspice has no trouble computing the
voltage on the gate since it's not perfectly
floating.

The new error checking will also detect a loop of
voltage sources and/or inductors when there's
no Rser in the loop.

--Mike

--- Bill Lewis <wrljet@...> wrote:

Thank you so much.

How did you determine that? Or is this something I
should just know -- to leave nothing floating?

Bill

--- Panama Mike <panamatex@...> wrote:

Bill,

<snip>

The problem was that the filment supply was floating,
that is, its potential wasn't defined. The following
circuit fixed this:

--- .asc file ---

Version 4
SHEET 1 892 692
WIRE -144 304 -144 336
WIRE 512 288 512 304
WIRE 304 160 304 112
WIRE 304 64 512 64
WIRE 512 64 512 96
WIRE 512 176 512 208
WIRE 384 112 304 112
WIRE 112 176 112 208
WIRE 112 208 256 208
WIRE 112 208 112 224
WIRE 112 304 112 336
WIRE 336 432 336 416
WIRE 304 112 304 64
WIRE 272 256 240 256
WIRE 240 256 240 272
WIRE 272 304 272 416
WIRE 288 272 288 304
WIRE 288 304 272 304
WIRE 320 272 320 304
WIRE 320 304 336 304
WIRE 336 304 336 320
WIRE 272 416 336 416
WIRE 336 416 336 400
WIRE -144 224 -144 208
WIRE -144 208 112 208
FLAG -144 336 0
FLAG 240 272 0
FLAG 512 304 0
FLAG 384 112 p
FLAG 112 176 g
FLAG 112 336 0
FLAG 336 432 0
SYMBOL voltage -144 208 R0
WINDOW 123 24 132 Left 0
WINDOW 39 0 0 Left 0
WINDOW 0 31 32 Left 0
WINDOW 3 28 93 Left 0
SYMATTR InstName V1
SYMATTR Value SINE(-10 5 1000)
SYMBOL voltage 512 192 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V4
SYMATTR Value 300
SYMBOL res 496 80 R0
SYMATTR InstName R1
SYMATTR Value 1
SYMBOL res 96 208 R0
SYMATTR InstName R2
SYMATTR Value 1Meg
SYMBOL voltage 336 304 R0
WINDOW 123 24 132 Left 0
WINDOW 39 24 71 Left 0
WINDOW 3 27 91 Left 0
SYMATTR Value SINE(0 6.3 60)
SYMATTR InstName V2
SYMBOL triodeh 304 208 R0
WINDOW 3 27 61 Left 0
SYMATTR InstName U1
SYMATTR Value 12AU7
TEXT -40 528 Left 0 !;op
TEXT -40 424 Left 0 !.include triodeh_DM.sub
TEXT -40 456 Left 0 !.tran 1s


__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - File online, calculators, forms, and more



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



Your use of Yahoo! Groups is subject to

__________________________________________________
Do you Yahoo!?
Yahoo! Tax Center - File online, calculators, forms, and more

__________________________________
Do you Yahoo!?
The New Yahoo! Search - Faster. Easier. Bingo.

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

I ran a sim with start time=0 and zoomed in on a portion of the
waveforms near the end of the sim. I then re-ran the sim with

Tstart

and Tstop specified as the beginning and end, respectively, of the
zoomed waveforms view. For example, let's say I zoomed in so that

my

time scale started at 895 usec and ended at 927 usec. I then set
Tstart=895u and Tstop=927u. To my surprise (and dismay), the

results

were different! Has anyone else noticed this problem?

Hello Ron,
sorry that nobody has answered you up to now.
Could you send Mike Engelhardt(alias Panama Mike) and/or me your
circuit file(s) (name.asc) to take a look at.
May be your time step was too coarse and just around the window you
looked there was too much interpolation.

Best Regards
Helmut

My better e-mail: HelmutSennewald@...

PS: I am not an employee of Linear Technology if that matters.

Thanks for the book recomendation. I'll keep my eyes open for a used
copy.

Dale

Bernhard,

As I changed the value of a resistor, I saw that it is possible
to give the "power rating" of

The power rating is only used for the Bill of Material. You can
ignore it as LTspice otherwise does. Note you don't have to
use that editor to change the value either, just move the mouse
to the old value, notice it turns into a text caret cursor,
and right click to edit that text.

--Mike

__________________________________
Do you Yahoo!?
The New Yahoo! Search - Faster. Easier. Bingo.

Hello,

Thank You very much, Helmut. Your help was helpful! I now can use the TL071-OpAmp in my circuits - perfect.

But one thing astonished me:
As I changed the value of a resistor, I saw that it is possible to give the "power rating" of the resistor. So I tried it and gave the resistor a power rating of 0.25 Watt. Then I simulated the circuit and "burned" my resistor with a power of 1.5 Watt. That was possible without a problem. Instead I expected an error message by LTSpice like "The resistor R1 was driven by 1.5 Watt instead of 0.25 Watt and is now smoking". So what serves the power rating for? And how can I use it?

Yours,

Bernhard
______________________________________________________________________________
UNICEF bittet um Spenden fur die Kinder im Irak! Hier online an
UNICEF spenden: