I have been given the task of scaling down a 50V lithium ion battery to 24V. I think I have successfully uploaded both schematics and the PWL file in a zip file. The 50V schematic seems to work fine, the battery discharges to 0V after a certain amount of time. I was able to upload the 24V battery specs in the form of a table to a new voltage dependent voltage source, but I did not change any other component values and I did not change the PWL file. I run the simulation and the battery voltage never gets to 0V. I might not understand the function of the PWL file at the independent current source. My end goal is to get the 24V simulation working correctly by seeing the battery discharge to 0V and also understanding the purpose/function of the PWL file at the independent current source. I am not an electrical engineer, but want to try my best to understand my task. Anyone's help is much appreciated.?

I uploaded a new file labeled Paschens-spark_gap. It's a work in progress. And thank you for your help Tony.

开云体育

On 03/07/2023 15:50, Tony Casey wrote:

it always places a comment on the first line (the sub-schematic line)

I mean: it always places a comment on the first line (the sub-schematic name)

开云体育

On 03/07/2023 15:25, Andy I wrote:

That advice only applies to the top-level netlist, not to subcircuits.? Subcircuits usually begin with the ".subckt" command.? Comments are recommended (to document your work), but otherwise they are unnecessary for subcircuits.? The first line of a top-level netlist is ignored (treated like a comment, even if it doesn't start with a "*" character).? The first line of a subcircuit is not ignored.

It's interesting that LTspice text editor still tries to nudge you to have a line above the .subckt definition. The syntax highlighting colour is always green (comment) for the first line, even if that contains the .subckt definition. I suppose syntax highlighting routine doesn't distinguish whether it is a global netlist or a local one. Placing a carriage return on a blank first line is enough to turn the .subckt line to blue.

I noticed that if you use LTspice to create a netlist from a hierarchical schematic, it always places a comment on the first line (the sub-schematic line) followed by a blank line and then the .subckt definition on the third line. Whereas creating a top level netlist omits the blank line, but still places the original schematic file name as a comment on the first line.

Tony wrote, "It is also normal to begin a .subckt definition with a comment, starting with "*". Originally, SPICE assumed the first line was always a comment, but I'm not sure how strictly that is enforced, now. LTspice is quite forgiving of certain things."

That advice only applies to the top-level netlist, not to subcircuits.? Subcircuits usually begin with the ".subckt" command.? Comments are recommended (to document your work), but otherwise they are unnecessary for subcircuits.? The first line of a top-level netlist is ignored (treated like a comment, even if it doesn't start with a "*" character).? The first line of a subcircuit is not ignored.

Andy

Richard,

For some reason, you don't seem to like following advice.? Where is your schematic (.asc) file where this error happened?? Where is the symbol (.asy) file?? I really don't care that someone else could create another (different) new symbol from your subcircuit; where is YOUR symbol file?? Yes, it makes a difference.

Looking at the second subcircuit file that you have uploaded --

I do not know if this has any bearing on the new (singular matrix) error message that you got, but the syntax you used is probably not right.? It's better, but still wrong.? LTspice expects to have a number for its component values, not an expression.? You used a resistor "value" of "1e12 / Vspark", which is not a number.? Perhaps in your mind it should evaluate to a number, but that expression is an expression, not a number.? It must be a number.? I'm guessing that LTspice probably used the "1e12" as the resistor's value and ignored what comes after it, but that is only a guess.

If you wanted that expression to turn into a number, you need to enclose it within curly braces, like this:

? ??Rspark p n {1e12 / Vspark}

Curly braces turn an expression into a number.? Try doing that.? Do the same thing with your capacitor's value:

? ??Cspark p n {8.85e-12 * aa / d}

As I say, it might or might not work, but try it.? Only you have the schematic and the symbol, because you did not bother to include them when you uploaded your model.

What is "aa"?? Is that a parameter that gets passed to this subcircuit?? Same with "d".

The voltage source in your subcircuit still is incorrect.? You have a voltage source named "Vspark" and it's connected between nodes "=" and "(B", and it has a confusing value.? I'm surprised that LTspice accepted it and didn't abort on that.

In the resistor's expression, it refers to the value Vspark.? But Vspark is not defined as a paramater.? Is that supposed to represent a fixed parameter?? Or the voltage on some (yet unknown) node in your subcircuit?? Or the current through the voltage source coincidentally named "Vspark"?? What you wrote does not make sense.

FYI, the subcircuit you uploaded does not have a node "b", so the error message you quoted us could only have come from the schematic file WHICH YOU DID NOT BOTHER TO UPLOAD.? Please.? When we ask you to upload your schematic and symbol files, please follow that advice, and do it.

By the way, I know a pretty good reference to help you with "model cards" and other SPICE syntax.? It's called "Help" and it comes with LTspice.? Run LTspice, then go to its built-in Help.? In fact, much of LTspice's Help about individual component lines and models, happens to be written from the point of view of Netlist syntax, which is exactly where you need when creating a subcircuit.? Admittedly it is somewhat sparse in places, but it is there and it is more useful that you probably think it is.

Andy

开云体育

On 03/07/2023 14:30, Richard Andrews via groups.io wrote:

I uploaded a new file. Now I get that ltspice thinks B is a node. Hello Tony Casey, I'll try your first option later. Thank you.

This is what you uploaded:

.subckt sparkgap p n

* Parameters
* d: Gap distance in meters
* aa: Gap area in sqr meters
* p: Gas pressure in Pascals

* Model constants
?.param A = 5.19e-11
?.param B = 23.8
?.param C = 11.6

* Spark gap voltage
Vspark = (B * p * d) / log(A * p * d) - log(log(1+(1/1.2)))-C

* Capacitance of gap
* Spark gap resistance
Cspark p n 8.85e-12 * aa / d
Rspark p n 1e12 / Vspark

.ends

Yes, I looked at all the spark gap models and none were satisfactory to my needs.

I uploaded a new file. Now I get that ltspice thinks B is a node. Hello Tony Casey, I'll try your first option later. Thank you.

开云体育

On 03/07/2023 13:21, Richard Andrews via groups.io wrote:

I had a reference to help me with model cards, but I seem to have misplaced it.

What I would suggest is that you initially develop your spark gap model as a schematic, without worrying too much about SPICE netlist syntax. You can then extract the netlist and use that as a basis for your .subckt when you have got it working. You're making life much more difficult than it needs to be.

BTW, did you look at all the previous spark gap models in the group's Files section? If not, go to Files and type "spark gap" in the search box. You should get 40 hits, including some complete libraries and some development schematics that help the understanding of how they work.

I had a reference to help me with model cards, but I seem to have misplaced it.

OK, so I uploaded a new file. I get a "singular matrix: check node u2:b" error. Spice thinks my variable is a node.

Richard,

By the way -- I should have said this earlier, but I forgot to --

What you did was the reason for the error message.

You had two capacitors both named "Cspark, inside of the same subcircuit.? LTspice needs to alter that name when it "expands" the subcircuit into the expanded SPICE netlist.? It does that by inserting extra characters into the name.? In your case, it turned "Cspark" into "C:U2:spark".? So what it did was insert? "U2" in the middle of the name, after the first character which must be a "C" to indicate that it is a capacitor.? In your case, it found that Cspark was inside of a subcircuit which had the instance name "U2", so "U2" was the text that it inserted between the "C" and the "spark".? The extra colons are how it separated U2 from the rest of the name.

I am just explaining how "Cspark" got turned into "C:U2:spark".? "CLU2:spark" "C:U2:spark" is LTspice's way of saying "the capacitor you named 'Cspark' which I found inside of the subcircuit instance named 'U2'."

(And I need to proof-read more carefully what I type.? I made careless errors which I didn't catch before clicking the "Send" button.)

Andy

It looks like Richard wanted his comments to define parameters.

Of course they don't.? Having a line like this:

? ??* A = 5.19e-11

makes it a comment, where it does nothing.? It does not define a constant or parameter named "A", so it's invalid to later use "A" within a formula because "A" is not "known".? Maybe Richard intended to write:

? ? .param? A = 5.19e-11

But that's only one of many mistakes he made.

Andy

开云体育

I suppose the algebra could be included as comments also. Maybe Richard thought that the * worked for both lines of text.

Oops, typo alert.

I wrote, "and then another resistor also named Cspark" but that should have been "and then another capacitor also named Cspark".

Andy

In short, every bit of your subcircuit is not SPICE.? It's pretty algebra (if also incorrect), but it is not SPICE and it doesn't belong inside a subcircuit.

The only parts of your subcircuit that make sense, are the .SUBCKT line, the .ENDS line, and the comments.? Everything else should not be there.

Andy

A fresh install rarely helps, especially when the problem is a mistake in your circuit.

By not including your circuit (the .ASY and .ASC files), you aren't helping us help you.? We can't run the same simulation you did, now, can we?

But consider the following lines inside the subcircuit that you did upload:

* Spark gap resistance
Rspark = 1e12 / Vspark

* Capacitance of gap
Cspark = 8.85e-12 * d

* Connect the model to the circuit
Cspark p n
Rspark p n

Look at what you have there.? You have a resistor named Rspark (connected to the nodes "=" and "1e12" with value "/ Vspark" which is obviously ridiculous) and then another resistor also named Rspark connected to nodes "p" and "n" with no value.? You can't do that.? Aside from the ridiculous nodenames and values, there can be only one resistor with the same name.? You violated that rule.

And then you have a capacitor named Cspark (connected to the nodes "=" and "8.85e-12" with another ridiculous value "* d"), and then another resistor capacitor also named Cspark connected to nodes "p" and "n" and no value.? Likewise, you can't ever have two capacitors with the same name.

What you uploaded is not valid SPICE syntax, despite being between .SUBCKT and .ENDS lines.? It's garbage.

? ? "There has to be something wrong with my subckt!?"

You have that right.? It is very wrong.? You need to start over because it is not valid SPICE syntax.? ?What are you to do now?? Start over.

Andy

I already have backups of my stuff, so I did a fresh install and before loading my backups I did an autogeneration of the spark gap and I got the same warning about the multiple instances. What am I to do now? There has to be something wrong with my subckt!?

开云体育

When you autogenerate, the .ASY includes the path to the subcircuit, If you also put an .INC statement on your .ASC, you get the 'multiple instances' error.