开云体育

When I simulate the following circuit I end
up with 60mv for VOUT when the circuit should be off?
Any ideas why? Not sure where the voltage is coming
from.
6v
47pf Batt BSS84 VOUT
+----+---+------+----+ +-----------+--+
| + + + --- |
| --- --- .-. V .-.
| --- - | | | | |20K
| | | 1M| | | 50K | |
|-+ | === '-' | ___ '-'
+->| | GND +-----+-|___|++ |
| |-+ | | +-| + 47pf
| |----+----------+ 2N7002 |<-+---+
| 2N7002 | +-| | |
| | o | .-. |
|=|> === | | ---
VOff | o GND | | ---
Mom.Switch | '-' |
=== 500K | |
GND === ===
GND GND

Dave Pariseau.

Hello Helmut,

you were faster with your second posting as I could answer your first one. I wanted to recommend the teccor company too.

I really like Teccor SCRs and TRIACs. We use them extensivelly on our company. Very expensive, but they are the best I know.

The field SpiceModel must be empty. That's the only mistake. You only add the TRIAC symbol from the "misc" directory. Then "right click" the mouse over the word TRIAC and change it to Q8025R5.
Shure, the command line with the models must be added to the schematic. Example: .INCLUDE tectriac.lib . Put this file into the lib&#92;sub directory of SwitcherCADIII.

Yes, this was my mistake. Now it's working. I still don't understand very well how to manage the LTSpice libraries, but I'm working on it.

Have you read the datasheet of this high power TRIAC? It needs nearly 100mA gate current to switch on. Just a hint for the circuit in your simulation.

This was just an example. I've imported the tectriac.lib and some triacs from OnSemi.

Thank you *very* much,

Brusque

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

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

Helmut,

Hello Mike or whoever exactly knows about,
...if a model uses the node number 0, is
it then referenced to the common ground
0 of the top schematic or is this a
floating node like any other node inside
the subcircuit?

Yes you are correct, node 0 is global.
Even if used in a subcircuit, it is global
ground. You can't name the pin of a
hierarchical symbol "0" and have that
refer to the node "0" inside that page of
circuitry.

Note that you can specify other nodes to
be globals with the .global dot command.

Hello Mike,
thanks for the answer. I really felt like a beginner when I stumbled
about such a basic question.

Best Rgeards
Helmut

--- In LTspice@..., "brusque.listas@c..."
<brusque.listas@c...> wrote:

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&#92;sub folder. On the
squematic I've put the ".INCLUDE triac.sub" Spice directive.

Hello Brusque,
you were faster with your second posting as I could answer your first
one. I wanted to recommend the teccor company too.

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.

The field SpiceModel must be empty. That's the only mistake.

You only add the TRIAC symbol from the "misc" directory. Then "right
click" the mouse over the word TRIAC and change it to Q8025R5.
Shure, the command line with the models must be added to the
schematic. Example: .INCLUDE tectriac.lib . Put this file into the
lib&#92;sub directory of SwitcherCADIII.

Have you read the datasheet of this high power TRIAC? It needs nearly
100mA gate current to switch on. Just a hint for the circuit in your
simulation.

Have fun with LTSPICE.

Helmut

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

Arnold Esper wrote:

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


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



Your use of Yahoo! Groups is subject to

------------------------------------------------------------------------
Name: Orgelfilter01.jpg
Orgelfilter01.jpg Type: JPEG Image (image/jpeg)
Encoding: Base64

Mike and group:
I'll throw one out. I would like a saved setup file so that when
multiple plot planes are used I don't have to reset them up once I have
closed the file. I think a work around right now is open the schematic
file and the last raw file then rerun with changes, but I haven't tried
it yet. Mike I can't repeat myself enough about how useful the program
is.
Comments welcome
Jim Stockton

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&#92;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.