Two questions about LTSpice

[Marco Trapanese]

Guys, I know most of you are experienced users of spice here
Two short questions, I've already RTM without find the answers.

- I need a TIP 122 model... where I should look for?

- worst-case scenario: I set the tolerances of my resistors. How to run
a simulation to get the worst-case? I'm talking about the maximum span
of selected traces when components reach their end values.

Thanks!
Marco

 

[Vlad]

Hello

For the TIP122, I did a search on Google and I got it within the first hit. As for the worst-case setup, try this link, it has a good explanation: k6jca.blogspot.com/2012/07/monte-carlo-and-worst-case-circuit.html

Good luck,
Vlad

 

[Marco Trapanese]

Il 17/10/2012 08:46, Vlad ha scritto:

For the TIP122, I did a search on Google and I got it within the first hit.

I also got it at the first hit, if you're referring to this page:

http://www.onsemi.com/pub_link/Collateral/TIP122.SP2

but the code inside is quite different than the *.asy files available
into the lib folder of LTSpice. Here my question.

In fact I've already tried to put the file there calling it tip122.asy.
But when I select it from LTSpice I got 'Unknown symbol syntax: ".SUBCKT
Xtip122 1 2 3" '

As for the worst-case setup, try this link, it has a good explanation: k6jca.blogspot.com/2012/07/monte-carlo-and-worst-case-circuit.html

Thanks a lot for the link. I'll give it a try.

Marco

 

[o pere o]

Il 17/10/2012 08:46, Vlad ha scritto:



I also got it at the first hit, if you're referring to this page:

http://www.onsemi.com/pub_link/Collateral/TIP122.SP2

but the code inside is quite different than the *.asy files available
into the lib folder of LTSpice. Here my question.

In fact I've already tried to put the file there calling it tip122.asy.
But when I select it from LTSpice I got 'Unknown symbol syntax: ".SUBCKT
Xtip122 1 2 3" '




Thanks a lot for the link. I'll give it a try.

Marco

The link Vlad provided is a Spice subcircuit file. Perhaps this
http://www.simonbramble.co.uk/lt_spice/ltspice_lt_spice_tutorial_4.htm
may help you inserting it into LTSpice.

Pere

 

[Marco Trapanese]

Il 17/10/2012 09:55, o pere o ha scritto:

The link Vlad provided is a Spice subcircuit file. Perhaps this
http://www.simonbramble.co.uk/lt_spice/ltspice_lt_spice_tutorial_4.htm
may help you inserting it into LTSpice.

Thanks! I wasn't able to find this information in the manual.
It works.

Marco

 

[Robert Macy]

Guys, I know most of you are experienced users of spice here
Two short questions, I've already RTM without find the answers.

- I need a TIP 122 model... where I should look for?

- worst-case scenario: I set the tolerances of my resistors. How to run
a simulation to get the worst-case? I'm talking about the maximum span
of selected traces when components reach their end values.

Thanks!
Marco

Are you certain you want ALL the worst case values at the SAME time?
The statistical likelihood of that is supposed to be extremely small.

We only used the 'worst case box' for milspec designs, where if the
circuit didn't perform to spec, you had to point tothe component that
was out of spec, else...

More likely scenario was for cmmecial designs where we used a Guassian
distribution for the component tolerances, like 'square root of the
sum of the squares' tolerances which was quite a bit more lenient to
design. But even in Production that wasn't realistic - sometimes. We
found the resistor manufacturers made runs of resistors measured what
thy made, which created a flat distribution, but then they culled out
special values which put 'holes' in that distribution! Usually we got
distributions with the centers cut out. In other words likely to get +
values and like to get - values, and rarely got exactly what the label
said.

 

[Marco Trapanese]

Il 17/10/2012 16:04, Robert Macy ha scritto:

Are you certain you want ALL the worst case values at the SAME time?
The statistical likelihood of that is supposed to be extremely small.

Small is not zero, and Murphy's watching me

More likely scenario was for cmmecial designs where we used a Guassian
distribution for the component tolerances, like 'square root of the
sum of the squares' tolerances which was quite a bit more lenient to
design. But even in Production that wasn't realistic - sometimes. We
found the resistor manufacturers made runs of resistors measured what
thy made, which created a flat distribution, but then they culled out
special values which put 'holes' in that distribution! Usually we got
distributions with the centers cut out. In other words likely to get +
values and like to get - values, and rarely got exactly what the label
said.

I'm agree, but sometimes is useful to know where are the bounding
limits, hoping you'll never reach them.

Marco

 

[Marco Trapanese]

Il 17/10/2012 08:46, Vlad ha scritto:

As for the worst-case setup, try this link, it has a good explanation:
k6jca.blogspot.com/2012/07/monte-carlo-and-worst-case-circuit.html

It does the dirty job but in a weird way. I'm going to improve it.
Do you know a way to obtain the tolerance value already put in the
related field (e.g. a resistor) ?

Marco

 

[John S]

Guys, I know most of you are experienced users of spice here
Two short questions, I've already RTM without find the answers.

- I need a TIP 122 model... where I should look for?

- worst-case scenario: I set the tolerances of my resistors. How to run
a simulation to get the worst-case? I'm talking about the maximum span
of selected traces when components reach their end values.

Thanks!
Marco

There is an example simulation that comes with LTSpice called
MonteCarlo.asc in the \LTC\LTspiceIV\examples\Educational folder.

You don't have to do the Monte Carlo, but the example is good to study
to see how to change component values as you wish.

Cheers,
JohnS

 

[Helmut Sennewald]

Since I work primarily at the device level I literally have hundreds
of libraries. Is there a way in LTspice to call a library by its
PATH, rather than requiring it to be in the same folder as the
schematic?

...Jim Thompson
--
| James E.Thompson, CTO | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.

Hello Jim,

You can specify a full path.

Example:

..lib C:\mylib1\mosfet\abc.lib

Best regards,
Helmut

 

[Helmut Sennewald]

Is that put in via the so-called "Spice directive"?

...Jim Thompson

Hello Jim,

A SPICE-directive is simply a SPICE-line.
You can either use a SPICE-directive in the schematic or you specify the
full path in the symbol.

I personally never use a full path name, because I mostly work on chematics
for other users. It's then much more convenient to have all files the folder
of the schemtaic.

Best regards,
Helmut

 

[Robert Macy]

Il 17/10/2012 16:04, Robert Macy ha scritto:


Small is not zero, and Murphy's watching me


I'm agree, but sometimes is useful to know where are the bounding
limits, hoping you'll never reach them.

Marco

Then there are the 'just get by' values. Where you have them in stock,
they're almost the right value, but not quite, but it's 12 weeks to
get the right ones, so you NEED to use these.

Once when designing an IC, after being told to expect beta of 3:1 and
not trusting; I designed the circuit to take a beta range of 5:1
Brother! did THAT pay off!

Once when designing CCD cameras, and being told to expect a
'sensitivity' of such and such and again not trusting; I designed to
accept 50% of the minimum sensitivity. Boy, did THAT pay off.
Especially when you get a lot in that doesn't meet spec, and there are
NO others and you're supposed to be shipping 2,000 units/mo and you
have a room full of workers who will have NOTHING to do if you reject
that lot.


So question goes back to the OP...why do you need to design to milspec
style? Unless your customer is milspec, you have overdesigned for
instrumentation volumes and probably underdesigned for consumer
volumes [10,000,000 per year]

 

[Charlie E.]

Il 17/10/2012 16:04, Robert Macy ha scritto:



Small is not zero, and Murphy's watching me




I'm agree, but sometimes is useful to know where are the bounding
limits, hoping you'll never reach them.

Marco

Not sure in LTSpice, but in PSpice the worst case sim does this.
First, it does a base run, and gets your 'output' value. Then, it
goes to each toleranced part, changes the value a small bit, and runs
a new sim. It notes whether that output value changes plus, or minus.
After testing the sensitivity on all the parts, it takes each part,
adjusts its value in the direction indicated by the sensitivity to its
limit, and runs a final, worst case simulation.

Note that this is not necessarily the absolute worst case. In some
circuits, especially filters, the actual worst case may be a some
point within the tolerances where resonance effects are worse. Also,
if you were not careful in setting your distribution types and values,
you can get wild values for the sim, especially if you have gaussian
distibution parts (PSpice sets the tolerance as the one sigma point,
so worst case is three sigmas...)

Usual practice is to do the worst case high, worst case low, and then
some Monte Carlo runs. Display them all in the same probe window, and
you can see what the distribution of results tends to be.

 

[Marco Trapanese]

Il 17/10/2012 23:57, Charlie E. ha scritto:

Not sure in LTSpice, but in PSpice the worst case sim does this.
First, it does a base run, and gets your 'output' value. Then, it
goes to each toleranced part, changes the value a small bit, and runs
a new sim. It notes whether that output value changes plus, or minus.
After testing the sensitivity on all the parts, it takes each part,
adjusts its value in the direction indicated by the sensitivity to its
limit, and runs a final, worst case simulation.

This is the behavior I was expecting. I'm afraid the DIY solution seen
in the link is not so accurate.

Note that this is not necessarily the absolute worst case. In some
circuits, especially filters, the actual worst case may be a some
point within the tolerances where resonance effects are worse. Also,
if you were not careful in setting your distribution types and values,
you can get wild values for the sim, especially if you have gaussian
distibution parts (PSpice sets the tolerance as the one sigma point,
so worst case is three sigmas...)

You're right.

Usual practice is to do the worst case high, worst case low, and then
some Monte Carlo runs. Display them all in the same probe window, and
you can see what the distribution of results tends to be.

Ok, I got it.
Thanks
Marco

 

[Marco Trapanese]

Il 17/10/2012 21:13, Robert Macy ha scritto:

So question goes back to the OP...why do you need to design to milspec
style? Unless your customer is milspec, you have overdesigned for
instrumentation volumes and probably underdesigned for consumer
volumes [10,000,000 per year]

No milspec at all.
For example, if you followed the thread about the current limiter, I
want know how much will change the limited current in function of the
tolerance of the resistor. It's a protection, so I do need to know if it
will safe with any value I may expect.

It's just an example, but I hope you understand what I'm saying.

Marco

 

[Robert Macy]

Il 17/10/2012 21:13, Robert Macy ha scritto:

So question goes back to the OP...why do you need to design to milspec
style? Unless your customer is milspec, you have overdesigned for
instrumentation volumes and probably underdesigned for consumer
volumes [10,000,000 per year]

No milspec at all.
For example, if you followed the thread about the current limiter, I
want know how much will change the limited current in function of the
tolerance of the resistor. It's a protection, so I do need to know if it
will safe with any value I may expect.

It's just an example, but I hope you understand what I'm saying.

Marco

Yes, being conservative is good. I used the term 'milspec' merely as a
descriptor to make it easy to refer to using the worst case box of
tolerance values. Don't forget to add the tolerances of all the
measuring intrumentation, too.

 

[josephkk]

Yep. Understood.

I work with so many different clients and device libraries that I
extensively use a utility "Clip Path"...

http://download.cnet.com/ClipPath/3000-2094_4-10050927.html

which helps me manage hierarchical schematics (sub-schematics are
often in their own folder, due to pre-testing before incorporation),
and device libraries (I have 93 different foundries/manufacturers, and
49,726 different folders totaling 5.2GB

...Jim Thompson

Poxy hell. I might buy that off you if i could. For obvious reasons it
is not (reasonably) available for sale by you.


BTW is PSpice still available for sale? Is the price not too
unreasonable?

?-)

 

[josephkk]

Il 17/10/2012 08:46, Vlad ha scritto:



It does the dirty job but in a weird way. I'm going to improve it.
Do you know a way to obtain the tolerance value already put in the
related field (e.g. a resistor) ?

Marco

You might look at sensitivity analysis. A .sens card with all the
components you want analyzed listed. Then you could easily pick the ones
you need to sweep. Myself, i can do most of that in my head without any
"heavy lifting" analytically.

?-)

 

[Fred Abse]

I also got it at the first hit, if you're referring to this page:

http://www.onsemi.com/pub_link/Collateral/TIP122.SP2

but the code inside is quite different than the *.asy files available into
the lib folder of LTSpice. Here my question.

In fact I've already tried to put the file there calling it tip122.asy.
But when I select it from LTSpice I got 'Unknown symbol syntax: ".SUBCKT
Xtip122 1 2 3" '

The file referred is a *subcircuit* file.

..asy files are *symbols*, ie. the shape that shows on a schematic.

Put TIP122.sp2 in /lib/sub, and add the LTspice directive ".lib
TIP122.sp2" to your LTspice schematic.

Use the standard NPN symbol, but don't assign a device model. Instead,
control-right-click on it, which will open a dialog box where you can make
it into an "X" subcircuit device, and set the appropriate parameters.

A good read of the manual will make things clear.

If you use a lot of subcircuit devices, it's a good idea to make a
dedicated "subcircuit npn" symbol.