Searching \ for '[EE] Can LTspice simulate transformer + spark' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/microchip/ios.htm?key=spi
Search entire site for: 'Can LTspice simulate transformer + spark'.

No exact or substring matches. trying for part
PICList Thread
'[EE] Can LTspice simulate transformer + spark gap?'
2011\11\12@035503 by Electron

flavicon
face

I'm having problems simulating transformer + spark gap with LTspice.

Is it possible?

I find no spark gap and even the transformer, although I can find it, does
not seem to simulate (gives errors, and I can't specify any parameters though).

Is it really a limit of the program/library or is it me? How can I get it to
work?

Thanks,
Mario

2011\11\12@122131 by Sean Breheny

face picon face
Hi Mario,

LTSpice handles transformers by using two inductors with a mutual
inductance (the .M command). You can specify all the usual parameters
of the two inductors and then for the mutual inductance, you specify a
"coupling factor" K.

As for a spark gap - there is no built-in model for that. You will
have to make one yourself out of the other components which are
available. Depending on what you need to simulate, this may be
difficult. You will need to be aware of all the relevant properties of
spark gaps - you can't use LTSpice to "learn" about the properties of
spark gaps - you can only use it as a simulation engine to run your
own model of a spark gap.

Sean


On Sat, Nov 12, 2011 at 3:54 AM, Electron <spam_OUTelectron2k4TakeThisOuTspaminfinito.it> wrote:
{Quote hidden}

>

2011\11\12@131423 by Oli Glaser

flavicon
face

On 12/11/2011 17:21, Sean Breheny wrote:
> Hi Mario,
>
> LTSpice handles transformers by using two inductors with a mutual
> inductance (the .M command). You can specify all the usual parameters
> of the two inductors and then for the mutual inductance, you specify a
> "coupling factor" K.
>
> As for a spark gap - there is no built-in model for that. You will
> have to make one yourself out of the other components which are
> available. Depending on what you need to simulate, this may be
> difficult. You will need to be aware of all the relevant properties of
> spark gaps - you can't use LTSpice to "learn" about the properties of
> spark gaps - you can only use it as a simulation engine to run your
> own model of a spark gap.
>
> Sean
>

I was just about to say much the same as Sean, but his post popped up first.
As mentioned you need to specify a coupling between two inductors to make a transformer.
Add a SPICE directive, for example:
K1 L1 L2 0.99
This will create a coupling between L1 and L2 of 0.99 (factor can be from 0 to 1)
For the spark gap, there isn't one in LTSpice. There are usually only the common components included with SPICEs. Floating around on the web are various SPICE models of the more exotic variety (e.g. motors, valve/tubes, etc)
What you would need to do is make your own based on the breakdown properties of air.
As SPICE is basically a mathematical modelling tool, it can theoretically be used to simulate just about anything (e.g. fluid dynamics, thermal properties, magnetic circuits, etc)
I would search for some info on SPICE commands (all about circuits has a basic intro IIRC) or grab a book that goes into greater detail. Once you know what the various parameters do in the .model file, you can set it up to match whatever function describes a spark gap and add variable parameters for gap length, maybe even humidity and any other factors.
You could probably take a diode as a rough template for a spark gap (e.g. adjust foward/reverse voltage to necessary voltages)
Or maybe a voltage controlled switch might be good enough. Have a look in the LTSpice help under circuit elements for information on the switch and other things.
Whenever I need a model that LTSpice doesn't have, I try Googling "<model> SPICE". I just tried this with "Spark gap SPICE", and came up with the following, hopefully they will help get you started:
www.edn.com/archives/1997/070397/14di_06.htm
http://www.spectrum-soft.com/news/winter99/sparkgap.shtm

2011\11\12@141023 by Electron

flavicon
face

Thank You.

A question, if You don't mind: I always used LTSpice "graphically". It's
easy to create two inductors. Now, how do I enter the coupling factor?

I never created a component in LTSpice, I will google for a spark gap spice
model, and then I will re-google for some tutorial on how to add it to
LTSpice. If I'm out of luck I will ask here again, but I think google will
suffice for this other mission, which would be probably long to explain
here.

Thanks again.

Cheers,
Mario


At 19.13 2011.11.12, you wrote:
{Quote hidden}

>

2011\11\12@145253 by Oli Glaser

flavicon
face
On 12/11/2011 19:09, Electron wrote:
> Thank You.
>
> A question, if You don't mind: I always used LTSpice "graphically". It's
> easy to create two inductors. Now, how do I enter the coupling factor?

On the far right of the LTSpice toolbar there is an icon (the ".op" one) for creating a SPICE directive. CLick on this and add Kn Ln Ln Kf, where n is the number of your components and Kf is the coupling factor.
Example:
You have two inductors, L1 and L2. You want to couple them with a factor of 0.9, so you click on the .op icon and write:
K1 L1 L2 0.9 (K could be any number, e.g K2, K3, etc depending on how many couplings you have in your circuit)
Place the directive on the schematic somewhere and you're done.

2011\11\12@151347 by Sean Breheny

face picon face
Oops, I should have said "K" command/component, not "M". Oli has the
correct version.

On Sat, Nov 12, 2011 at 1:13 PM, Oli Glaser <.....oli.glaserKILLspamspam@spam@talktalk.net> wrote:
{Quote hidden}

>

2011\11\13@052939 by Electron

flavicon
face
At 20.52 2011.11.12, you wrote:
>On 12/11/2011 19:09, Electron wrote:
>> Thank You.
>>
>> A question, if You don't mind: I always used LTSpice "graphically". It's
>> easy to create two inductors. Now, how do I enter the coupling factor?
>
>On the far right of the LTSpice toolbar there is an icon (the ".op" one)
>for creating a SPICE directive. CLick on this and add Kn Ln Ln Kf, where
>n is the number of your components and Kf is the coupling factor.
>Example:
>You have two inductors, L1 and L2. You want to couple them with a factor
>of 0.9, so you click on the .op icon and write:
>K1 L1 L2 0.9 (K could be any number, e.g K2, K3, etc depending on how
>many couplings you have in your circuit)
>Place the directive on the schematic somewhere and you're done.

It worked wonders, thank you! :-)

But what does coupling=0.9 imply? 90% efficiency for the resulting transformer?

Thanks,
Mario

2011\11\13@120728 by Sean Breheny

face picon face
No, it's not efficiency, it's the fraction of the magnetic flux which
the two inductors share. The remaining amount is "leakage". Closer to
0, they act like totally separate inductors (like you didn't even have
the K statement). K=1 makes them into an ideal transformer (not in the
lossless sense but in the sense that it has no extra inductance from
"leakage inductance").

Sean


On Sun, Nov 13, 2011 at 4:56 AM, Electron <electron2k4spamKILLspaminfinito.it> wrote:
{Quote hidden}

>

2011\11\16@223348 by Oli Glaser

flavicon
face
On 13/11/2011 09:56, Electron wrote:
{Quote hidden}

It's one of the factors that contribute to efficiency, but there are others too (core losses, leakage inductance, etc)
It's just the inductive coupling coefficient between windings. To simulate as accurately as possible you would have to add various other parasitic elements. If you google "spice transformer" there are quite  a few helpful links. Here are a couple of helpful ones:
http://ltwiki.org/index.php5?title=Transformers    Reasonably simple and clear
http://www.intusoft.com/articles/satcore.pdf <http://www.intusoft.com/articles/satcore.pdf>    Getting more complex
http://fmtt.com/Transformer%20SPICE%20Model%202-14-08.pdf     Approach with caution...

2011\11\17@150444 by Electron

flavicon
face
At 04.33 2011.11.17, you wrote:
{Quote hidden}

Thank You.. I will read the last one only in the presence of my parents. :D

;)

Cheers,
Mario

More... (looser matching)
- Last day of these posts
- In 2011 , 2012 only
- Today
- New search...