开云体育

Hello,

I'm trying to have a working TRIAC model on LTSpice.

From www.teccor.com I got the following model that I saved to a file called triac.sub. I've put this file on lib\sub folder. On the squematic I've put the ".INCLUDE triac.sub" Spice directive.


*=========================*
* TECCOR TRIACS *
* Triac pinout: MT2 G MT1 *
*=========================*

*SRC=Q8025R5;Q8025R5;TRIACS;TECCOR;800V 25A
*SYM=TRIAC
.SUBCKT Q8025R5 1 2 3
* TERMINALS: MT2 G MT1
QN1 5 4 3 NOUT OFF
QN2 11 6 7 NOUT OFF
QP1 6 11 3 POUT OFF
QP2 4 5 7 POUT OFF
DF 4 5 DZ OFF
DR 6 11 DZ OFF
RF 4 6 8MEG
RT2 1 7 25.4M
RH 7 6 5.25
RGP 8 3 12
RG 2 8 5.8
RS 8 4 1.2
DN 9 2 DIN OFF
RN 9 3 6.12
GNN 6 7 9 3 0.554
GNP 4 5 9 3 0.705
DP 2 10 DIP OFF
RP 10 3 3.56
GP 7 6 10 3 0.373
.MODEL DIN D (IS=764F)
.MODEL DIP D (IS=764F N=1.19)
.MODEL DZ D (IS=764F N=1.5 IBV=100U BV=800)
.MODEL POUT PNP (IS=764F BF=5 CJE=1.12N TF=102U)
.MODEL NOUT NPN (IS=764F BF=20 CJE=1.12N CJC=223P TF=6.8U)
.ENDS



But everytime I try to start the simulation I got the message:
SPICE Error
Too many parameters for subcircuit type "q8025r5"(instance: xu1)

On the "Component Attribute Editor" I have:
Prefix X
InstName U1
SpiceModel triac
Value Q8025R5
Value2 <none>
SpiceLine <none>
SliceLine2 <none>

Please, I need help.

Thanks,

Brusque
--
-----------------------------------------------------------------
Edson Brusque C.I.Tronics Lighting Designers Ltda
Research and Development Blumenau - SC - Brazil
Say NO to HTML mail www.citronics.com.br
-----------------------------------------------------------------

You are correct, The simulation is extremely slow. I would better

say

LTSPICE fails here with its default settings.

Two things are necessary with this circuit.

1.
Add the option .OPTIONS abstol=1e-10 or higher.
This reduces the numerical conergence effort for the simulator.

2. Add a load resistor of 1MOhm or less(e.g. 100k) from your output
VOUT to ground.

Only both changes together allow a useful simulation of this

circuit

with LTSPICE. I needed 1 hour to fix it even as a frequently SPICE
user. I have not further investigated which of the models in your
circuit was the trouble maker. The models used are MOSFET 2N7002,
MOSFET FDN304P and the battery switch LTC4412.
I tried a lot of the other options too, but only "abstol" and the
circuit enhancement(load resistor) were really important.


Best Regards
Helmut

Thanks Helmut!!!

What do you think about the display of the .step
Parameters in the Viewer? Or did I miss something
here, too?

This is a known problem that I want to fix. It's
not the top priority because there isn't much in
house interest in it. The IC designers using the
program tell me they feel they have no trouble
keeping the step values straight in their heads.
God bless them is all I can say. Anyway, right
now the only thing that helps here at all is that
you can use the attached cursor and navigate
sequentially from run to run in the .step with
the up/down cursor keys. Also, the .step values
used are in the .log file.

--Mike

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

--- In LTspice@..., "David Pariseau"
<david.pariseau@s...> wrote:

....
I added this and commented out the Diode line and there are no

errors

now in simulation, but the simulation is glacially slow and I'm not
sure correct.

Hello Dave,
thanks for the circuit file.
When I opened it, the resistor R1 wasn't connected correctly to the
4th pin of the FDN304p. I corrected that myself.

You are correct, The simulation is extremely slow. I would better say
LTSPICE fails here with its default settings.

Two things are necessary with this circuit.

1.
Add the option .OPTIONS abstol=1e-10 or higher.
This reduces the numerical conergence effort for the simulator.

2. Add a load resistor of 1MOhm or less(e.g. 100k) from your output
VOUT to ground.

Only both changes together allow a useful simulation of this circuit
with LTSPICE. I needed 1 hour to fix it even as a frequently SPICE
user. I have not further investigated which of the models in your
circuit was the trouble maker. The models used are MOSFET 2N7002,
MOSFET FDN304P and the battery switch LTC4412.
I tried a lot of the other options too, but only "abstol" and the
circuit enhancement(load resistor) were really important.


Best Regards
Helmut

Jon,

...Edit=>Attributes=>Edit Window...

However, it's really:

Edit=>Attributes=>Attribute Window

Thank you very much for pointing this out.

Also, as I discovered, there are some items
not present in the attribute window which
appears, using ctrl-W:

2 RefName
5 QArea
8 Width
9 Length
10 Multi

Are there others I've missed? Are these
documented? Is there a reason why these
do not appear in the ctrl-W list?

There are a couple hundred symbol attributes.
There's even an undocumented attribute
compiler. These attributes are used when
LTspice reads some other EDA formats used
inhouse. However, these formats are non-
standard, customized versions of commercial
syntaxs and have no usage outside of LT.
I only document what I think is useful(and
feel I can let people rely on.) While
there are useful undocumented features
that come out in formums like this user
group, I'm afraid those symbol attributes
will be a red herring for you and could
cause erratic program operation.

--Mike

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

Note that the background color is not printed. That

is, you can set it to black in the color preferences

dialog but it will still be white when you print it

on white paper becuase it's the background and is not

printed. So if you also what a bitmap that is on a

white background, so a print preview and capture that

bitmap with Alt-Print Screen.

Hope this helps,

Thanks for this hint. That's absolutely sufficient.




What do you think about the display of the .step Parameters in the
Viewer? Or did I miss something here, too?




Regards




Peter

On Wed, 26 Mar 2003 11:12:51 -0800 (PST), you wrote:

...So I looked at the ASCII text of PUT.ASY and
noticed these lines:

WINDOW 0 24 0 Left 0
WINDOW 3 24 72 Left 0
...

I'd recommend using the graphical symbol editor.
Attribute visibility is covered in help in
Schematic Capture=>Creating New Symbols=>
Attribute Visibility.

Yes, I thought I'd already tried that but apparently I hadn't.
Sorry about that -- defective user, I guess.

By the way, your help file describes this as:

"You can edit the visibility of attributes using the menu
command Edit=>Attributes=>Edit Window. After you select an
attribute with this dialog you will then be able to position it
as you wish with respect to the symbol."

However, it's really:

Edit=>Attributes=>Attribute Window

There is no "Edit Window" selection there, I believe.

Also, as I discovered, there are some items not present in the
attribute window which appears, using ctrl-W:

2 RefName
5 QArea
8 Width
9 Length
10 Multi

Are there others I've missed? Are these documented? Is there a
reason why these do not appear in the ctrl-W list?

Jon

Various people are writing:

Yes, it's a good Idea to allow white background to
the graphik Window, in order to save printing-color
or some extra work for inverting it for other
programs.

Note that the background color is not printed. That
is, you can set it to black in the color preferences
dialog but it will still be white when you print it
on white paper becuase it's the background and is not
printed. So if you also what a bitmap that is on a
white background, so a print preview and capture that
bitmap with Alt-Print Screen.

Hope this helps,

--Mike

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

Jon,

...So I looked at the ASCII text of PUT.ASY and
noticed these lines:

WINDOW 0 24 0 Left 0
WINDOW 3 24 72 Left 0
...

I'd recommend using the graphical symbol editor.
Attribute visibility is covered in help in
Schematic Capture=>Creating New Symbols=>
Attribute Visibility.

--Mike

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

Mike,

Place a gate on a schematic. Right mouse click
on the body. Click on Value, Value2, SpiceLine,
or SpiceLine2. Type Vhigh=5 in the box above
the grid thing that looks like a spread sheet
of the component's attributes.

Thanks, that did the trick.

Dave.

> Hi there,
>
>
> LTSpice is really fun to work with. Assuming that Mike likes to get
> feedback, I would like to make some suggestions for enhancements of the
> waveform viewer, mainly for documentation purposes:
>
> * If any parameter of the circuit is stepped with the .step command, it
> should be possible in the waveform viewer to see what value the

parameter

> has in the respective curve. (see example stempodelparam.asc)

Preferably

> on a legend that can be switched on or off.
>
> * the number of the cursor should always be displayed, not only on
> mouseover.
>
> * maybe it should be possible to add some draw elements for

documentation

>
> * add a second color profile for the use of the results (via clipboard
> copy) in other documents with white background and different colors for
> grid, cursors and axis (cursor color is currently not customizable).

There

> is no doubt that black background is good for working on the screen but
> white background is good for documentation.
>
> What are your thoughts?
>
> Regards
>
> Peter Schaich

Yes, it's a good Idea to allow white background to the graphik Window, in
order to save printing-color or some extra work for inverting it for other
programs. The black background reminds me my analog oszilloscope, earlier used
every day. But nowadays I'm almost afraid to touch it's knobs, because of the
huge dust on it.
Maybe a good Idea too, to allow some differnt styles of drawing lines like
dotted, hatched .... for black and white coying machines. Adding the unit
behind every number can make it difficult to read at high line-densities. The
Windows could have a look similar to the picture below, I made with an early
Version of Spice2 (years ago).
.
Thanks, Arnold

On Wed, 26 Mar 2003 08:30:09 -0800 (PST), you wrote:

You probably want to make the Model and Instance name
visible in the .asy file and nothing else. THE VALUE
SHOULD BE LEFT BLANK in both the .asy and instance,
unless you want to add parameters to pass to the
subckt. These should be of the form "eta=5.3"

Attached is a .asy file and .sub file that work
together
to demonstate being able to use the drop list to
to select a subckt in the .sub file. You will have
to fix line wrap.

Okay, thanks. I'm beginning to get some of it. However, now
this leads me to some more questions...

First, I went back to look at a symbol you provided me, some
time ago, for the PUJT (called PUT.ASY.) It included two text
attribute elements, InstName and Value, which I could see by
right-clicking on them. However, I noticed that I could not
change the attribute element type for them.

So I went and tried creating a new symbol. (I've avoiding doing
this, so far.) Then I looked around through the menus for a way
to add those same attributes, InstName and Value, to my new
symbol. I couldn't find them anywhere. Nada.

So I looked in the help for InstName. Nothing. I tried ctrl-W
and ctrl-A and played around with those. Nope, nothing I could
figure out there, either. I just couldn't figure out how you
added those two attributes to the visible part of the diagram.

So I looked at the ASCII text of PUT.ASY and noticed these
lines:

WINDOW 0 24 0 Left 0
WINDOW 3 24 72 Left 0

What's interesting to me is that I had *NO IDEA* what these are
for and I couldn't find any documentation on them, either. So I
just guessed that the first number might relate to type of
attribute and played around by changing it. I got the following
list, working the numbers up to about 40:

0 InstName
1 Type
2 RefName
3 Value
4
5 QArea
6
7
8 Width
9 Length
10 Multi
11
.
.
.
37
38 SpiceModel
39 SpiceLine
40 SpiceLine2
41
.
.
.

Then I went and looked at your newly posted example and noticed
this:

WINDOW 0 16 -32 Left 0
WINDOW 38 47 28 Center 0

Ah hah!! "38" is there, exactly what you were referring to.

Mike!? How do I add that, using the symbol editor GUI? Do I
have to hand-edit those things into the .ASY file? Or am I just
being an ignorant user who should know better?

Jon

David,

There's some special things you need to know
about the gates. The gates don't need external
power. If you want a gate to switch between
0 and 5 volts, give the gate a value of
"Vhigh=5" Vlow defaults to 0V.

I figured it was something like this. How do I
set Vhigh=5 for a particular gate???

Place a gate on a schematic. Right mouse click
on the body. Click on Value, Value2, SpiceLine,
or SpiceLine2. Type Vhigh=5 in the box above
the grid thing that looks like a spread sheet
of the component's attributes.

--Mike

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

An: "'LTspice@...'" <LTspice@...>

Von: "Schaich, Peter" <schaich.peter@...>
Datum: Wed, 26 Mar 2003 08:01:58 +0100
Betreff:[LTspice] Suggestions for waveform viewer



> Hi there,
>
>
> LTSpice is really fun to work with. Assuming that Mike likes to get
> feedback, I would like to make some suggestions for enhancements of the
> waveform viewer, mainly for documentation purposes:
>
> * If any parameter of the circuit is stepped with the .step command, it
> should be possible in the waveform viewer to see what value the parameter
> has in the respective curve. (see example stempodelparam.asc) Preferably
> on a legend that can be switched on or off.
>
> * the number of the cursor should always be displayed, not only on
> mouseover.
>
> * maybe it should be possible to add some draw elements for documentation
>
> * add a second color profile for the use of the results (via clipboard
> copy) in other documents with white background and different colors for
> grid, cursors and axis (cursor color is currently not customizable). There
> is no doubt that black background is good for working on the screen but
> white background is good for documentation.
>
> What are your thoughts?
>
> Regards
>
> Peter Schaich

Yes, it's a good Idea to allow white background to the graphik Window, in order
to save printing-color or some extra work for inverting it for other programs.
The black background reminds me my analog oszilloscope, earlier used every day.
But nowadays I'm almost afraid to touch it's knobs, because of the huge dust on
it.
Maybe a good Idea too, to allow some differnt styles of drawing lines like
dotted, hatched .... for black and white coying machines. Adding the unit behind
every number can make it difficult to read at high line-densities. The Windows
could have a look similar to the picture below, I made with an early Version of
Spice2.
.
Thanks, Arnold

Mike,

There's some special things you need to know
about the gates. The gates don't need external
power. If you want a gate to switch between
0 and 5 volts, give the gate a value of
"Vhigh=5" Vlow defaults to 0V.

I figured it was something like this. How do I
set Vhigh=5 for a particular gate??? I was looking
for something like this. It would have to be in a
particular instance right, not at the component level.

Also, all unconnected inputs are connected to
the gate's common node(that extra pin that is
tied to ground in the examples).

Fair enough, that makes things easier. Are the
PRE and CLR inputs active high? Can you tell this
by looking at the component? I wasn't able to find
any documentation on the flip-flop via help, etc...

Thanks for the help,
Dave Pariseau.

David,

I'm trying to use the dflop part in a simple
circuit and am having difficulty getting it
to work.

+-----------+
0-6v square wave --------|>CLK Q |--- 1v solid
out??
GND----| D Q'|
+-----------+

Both the CLR and the PRE inputs are floating
though I've tried tieing them up and down.

There doesn't seem to be anywhere to attach
power to the device? There is a common pin
(COM?) on the corner, but leaving it open or
tieing it to ground has the same effect.

I'm looking for a 5-6v output. The 160 example
has dflops in it and seems to work fine, which
is beyond me.

Any ideas?

There's some special things you need to know
about the gates.

The gates don't need external power. If you
want a gate to switch between 0 and 5 volts,
give the gate a value of "Vhigh=5" Vlow
defaults to 0V.

Also, all unconnected inputs are connected to
the gate's common node(that extra pin that is
tied to ground in the examples). This
connection flags that pin as unused and is
removed from the simulation. Note that the
common pin will be connected to ground by the
netlister if it is left floating. So, say you
place an AND gate on the schematic, connect one
of it's input to a signal, one input to ground
and leave the other 3 inputs floating. The
AND's output will follow the signal because
all the other pins aren't floating or grounded,
but flagged as not part of the simulation.

--Mike

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

I'm trying to use the dflop part in a simple
circuit and am having difficulty getting it
to work.

+-----------+
0-6v square wave --------|>CLK Q |--- 1v solid out??
GND----| D Q'|
+-----------+

Both the CLR and the PRE inputs are floating
though I've tried tieing them up and down.

There doesn't seem to be anywhere to attach
power to the device? There is a common pin
(COM?) on the corner, but leaving it open or
tieing it to ground has the same effect.

I'm looking for a 5-6v output. The 160 example
has dflops in it and seems to work fine, which
is beyond me.

Any ideas?
Thanks,
David Pariseau.

Jon,

...For example, if I select 2N6028 in the drop-down
for SpiceModel *and* then manually change the Value
attribute to match, everything works well...

You probably want to make the Model and Instance name
visible in the .asy file and nothing else. THE VALUE
SHOULD BE LEFT BLANK in both the .asy and instance,
unless you want to add parameters to pass to the
subckt. These should be of the form "eta=5.3"

Attached is a .asy file and .sub file that work
together
to demonstate being able to use the drop list to
to select a subckt in the .sub file. You will have
to fix line wrap.

--- .asy ---
Version 4
SymbolType CELL
LINE Normal -32 -32 32 0
LINE Normal -32 32 32 0
LINE Normal -32 -32 -32 32
LINE Normal -28 -16 -20 -16
LINE Normal -28 16 -20 16
LINE Normal -24 20 -24 12
LINE Normal 0 -32 0 -16
LINE Normal 0 32 0 16
LINE Normal 4 -20 12 -20
LINE Normal 8 -24 8 -16
LINE Normal 4 20 12 20
WINDOW 0 16 -32 Left 0
WINDOW 38 47 28 Center 0
SYMATTR Prefix X
SYMATTR Description Parameterized Single Pole Opamp.
En and in are equivalent voltage and current noises.
Enk and ink are the respective corner frequencies.
SYMATTR Value2 Avol=10Meg GBW=10Meg Slew=10Meg
SYMATTR SpiceLine ilimit=25m rail=0 Vos=0
SYMATTR SpiceLine2 en=0 enk=0 in=0 ink=0
SYMATTR ModelFile genopamp.sub
SYMATTR SpiceModel 1pole
PIN -32 16 NONE 0
PINATTR PinName In+
PINATTR SpiceOrder 1
PIN -32 -16 NONE 0
PINATTR PinName In-
PINATTR SpiceOrder 2
PIN 0 -32 NONE 0
PINATTR PinName V+
PINATTR SpiceOrder 3
PIN 0 32 NONE 0
PINATTR PinName V-
PINATTR SpiceOrder 4
PIN 32 0 NONE 0
PINATTR PinName OUT
PINATTR SpiceOrder 5

--- .sub ---
* Copyright Linear Technology Corp. 1998, 1999,
2000, 2001, 2002, 2003. All rights reserved.
*
.subckt 1pole 1 2 3 4 5
S1 5 3 N002 5 Q
S2 4 5 5 N002 Q
A1 2 1 0 0 0 0 N002 0 OTA G={Avol/Rout} ref={Vos}
Iout={slew*Cout} Cout={Cout} en={en} enk={enk} in={in}
ink={ink} Vhigh=1e308 Vlow=-1e308
C3 5 4 1p
C4 3 5 1p
S3 N002 0 4 N002 C
S4 0 N002 N002 3 C
R2 N002 4 {2*Rout} noiseless
R1 3 N002 {2*Rout} noiseless
R3 3 1 1G noiseless
R4 3 2 1G noiseless
R5 2 4 1G noiseless
R6 1 4 1G noiseless
.model C SW(Ron=100 Roff=1T Vt=0 Vh=-1 noiseless)
.param Rout=100Meg
.param Cout={Avol/GBW/2/pi/Rout}
.model Q SW(Ron=10 Roff=10Meg Vt=0 Vh=-.1 Vser={Rail}
ilimit={Ilimit} noiseless)
.param Avol=10Meg GBW=10Meg Slew=10Meg ilimit=25m
rail=0 Vos=0
.param en=0 enk=0 in=0 ink=0
.ends 1pole

.subckt 2pole 1 2 3 4 5
S1 5 3 N002 5 Q
S2 4 5 5 N002 Q
A1 2 1 0 0 0 0 N003 0 OTA G={Avol/Rout} ref={Vos}
Iout={slew*Cout} Cout={Cout} en={en} enk={enk} in={in}
ink={ink} Vhigh=1e308 Vlow=-1e308 Rout={Rout}
C3 5 4 1p
C4 3 5 1p
S3 N002 0 4 N002 C
S4 0 N002 N002 3 C
R3 3 2 1G noiseless
G1 0 N002 N003 0 {1/Rout}
R1 3 N002 {2*Rout} noiseless
R2 N002 4 {2*Rout} noiseless
C1 N002 0 {X*Cout/Avol}
S5 0 N003 N003 3 C
S6 N003 0 4 N003 C
R4 3 1 1G noiseless
R5 1 4 1G noiseless
R6 2 4 1G noiseless
.model C SW(Ron=100 Roff=1T Vt=0 Vh=-1 noiseless)
.param Rout=100Meg
.param Cout={Avol/GBW/2/pi/Rout}
.model Q SW(Ron=10 Roff=10Meg Vt=0 Vh=-.1 Vser={Rail}
ilimit={Ilimit} noiseless)
.param Avol=10Meg GBW=10Meg Slew=10Meg rail=0 Vos=0
ilimit=25m
.param en=0 enk=0 in=0 ink=0 phimargin=45
.param X
table(phimargin,29.4,3.5,32.1,2.9,33.8,2.6,35.8,2.3,38.1,2,40.9,1.7,43.2,1.5,45.9,1.3,49.2,1.1,53.2,0.9,58.2,0.7,64.7,0.5,73,0.3,86.1,0.05)
.ends 2pole


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

On Wed, 26 Mar 2003 00:49:55 -0800, you wrote:

Thanks. Just tested and it seems to work okay. Now what I'm
wondering about is what is displayed on the schematic. Should I
remove "visibility" for the Value attribute and add "visibility"
for the SpiceModel attribute on the underlying .ASY symbol?

I guess I'm asking this because the .ASY I currently use
automatically displays the Value attribute. But the new
drop-down for the SpiceModel only changes the SpiceModel
attribute (perhaps, as it should.) Since this isn't normally
displayed on the schematic, so far as I've seen anyway,
selecting a new model doesn't change what appears on the
schematic. So I have to manually change the Value attribute, as
well, in order to match (so it appears.)

For example, if I select 2N6028 in the drop-down for SpiceModel
*and* then manually change the Value attribute to match,
everything works well. If I then set the Value attribute to
"junk," leaving the SpiceModel to 2N6028, I get "Error: Unknown
subckt called in: xu1 n001 n002 n003 2N6028 junk" If I then try
and change the Value attribute to 2N6027 (which is also present
in the .LIB file I have, but which is *not* a match for the
current SpiceModel, which is 2N6028), then I get the error, "Too
many parameters for subcircuit type "2n6027" (instance: xu1)"

Just to let you know.

Jon

On Tue, 25 Mar 2003 15:19:26 -0800 (PST), you wrote:

Jon,

In the above case, it would be nice if LT Spice
would put a "Select Subcircuit" button on the
dialog box which comes up when I right-click on
the symbol (if the .ASY symbol is an X type)
and provide me a list of .SUBCKT entries it
found in the specified library file. In that
case, the PUJT.LIB case, this means it would pop
up 2N6027 and 2N6028, for example, and offer
those as options.

Yes, this is something that's been needed for a
long time. So I implemented it today. To use
it make a symbol with prefix 'X'. Make ModelFile
point to a library contianing subcircuits. Give
the symbol a SpiceModel that coincides with the
name of a subcircuit in ModelFile. Those
conditions will cause the editor for the
SpiceModel to be replaced with a drop list of
subcircuits in the file pointed to by ModelFile.

I modified the symbols 1pole.asy and 2pole.asy
to put the subcircuit names as the SpiceModel
attribute instead of the value so that you can
see it work(Though there's only one subcircuit
in the list to choose from). It's possible
that old schematics drafted with yesterday's
version don't work, just delete and replace the
1pole and 2pole instances to fix.

Thanks. Just tested and it seems to work okay. Now what I'm
wondering about is what is displayed on the schematic. Should I
remove "visibility" for the Value attribute and add "visibility"
for the SpiceModel attribute on the underlying .ASY symbol?

Jon