I am working on a "cantilever model" flyback

transformer with 4 windings. I elected to rip 

off one of the contrib/Wurth transformer 

symbols because they were nice and pretty

while I can't seem to get the hang of stick-

building with the "arc" object.

 

So that worked out, except now right-click

delivers a popup that's still all about Wurth

symbol.

 

"attachments are not allowed in this group"

 

This seems to be some "hidden junk", "Attributes" 

has none of this visible. Down in the symbol ASCII

I see this bit that appears in the popup, but nothing 

that looks like "why?".

 

"attachments are not allowed in this group"

 

If I remove that line the popup goes away, but

I can't hierarchy-descend by right click, as the

Help claims - this only works on some subset 

of symbols, no idea why.  Also cannot get to 

symbol attributes list by control-right-click

(as Help claims with no qualification).

 

What I want, is to add a "turns ratio" property

so that I can square-scale the secondary winding

inductance by that, squared. 

 

But I see nothing about how to add or remove

attributes from a symbol. Only change visibility.

I'm looking to add a named property and use

it (with math) in the netlist line or pass it in and

use the (well behaved in this regard) ind primitive

to (hopefully) carry it (the param*value) to the

netlist. I would like this param to appear at

placement-time, just like the primitives, and

used in a math expression in the value attribute

fields of ind instances (like I want to see 

"TurnsRatio" as a field to fill, and I want the L

(inductance) value of L1 to be "10m*TurnsRatio"

(or its syntax-correct equivalent, so that the

inductor in question is "modified from above"

(symbol instance property flows to SPICE 

value, not a SPICE .param or a {} evaluation of

one).

 

For that matter I find nothing about flexible

definition of netlisting either. Seems "baked 

in". But I know there's a lot of undocumented

features, so I'm asking.

It's not entirely clear what you are trying to do. You mention:

..but I can't hierarchy-descend by right click, as the Help claims

Are you trying make a hierarchical block, whereby you can right-click on the IdealXfmr symbol in the schematic editor, and you get an option to "Open Schematic"? If so, did you already create its schematic? You don't mention that.

To get that option, several things must already be in place:

1. The schematic must exist, preferably in the same folder as the symbol.
2. The schematic must have the same name as the symbol.
3. The symbol must be of type "Block".
   
4. The created symbol should have no values for any of the attributes. (Actually, you can add some after you have placed the symbol, but critically, the "Prefix" attribute must have remain empty.)

- this only works on some subset of symbols, no idea why.

Did you look inside any hierarchical symbols to see how they differ from your symbol?

Once you are able to get the "Open Schematic" option by right-clicking on the symbol, you will also get the "PARAMS" field. It is there that you can add "TurnsRatio" parameter. However, that won't do anything unless the "TurnsRatio" parameter exists in your lower level schematic.

The syntax for putting anything in the PARAMS field is:

ParameterName=<NumericValue>

..or

ParameterName={AnotherParameterName}

In the second case, "AnotherParameterName" must resolve to a numeric value in the top level schematic.

I don't know what you mean by:

flexible definition of netlisting

Netlists are not flexible. They must obey syntax rules just like any other language.

If you don't want a hierarchical block with a lower level schematic, you have two options:

1. Your component is a SPICE intrinsic component like a resistor, inductor, or transistor
   
2. You component is defined in a .subckt (like the Würth 750310471 that you used as the basis for your edited symbol).

Do you have a .subckt that defines your basic component? As a minimum, it should contain two inductors, each with an inductance value that resolves to a numeric value. It must also contain a coupling directive in order to behave as a transformer. The coupling directive looks something like this:

K1 L1 L2 0.99

The value of "0.99" can be replaced with a parameter:

K1 L1 L2 {Kval}

.. where "Kval" resolves to a numeric value defined elsewhere.

This is described in:

Help > LTspice > LTspice® > Circuit Elements > K. Mutual Inductance

This seems to be some "hidden junk", "Attributes" 

has none of this visible. Down in the symbol ASCII

I see this bit that appears in the popup, but nothing 

that looks like "why?".

This "junk" is not hidden at all, but as Andy says, it cannot be edited from within the schematic editor because the specific arrangement of the attributes prohibits it. You need to open the IdealXfmr symbol directly in the symbol editor. From there, press ctrl-A to edit the symbol's attributes. There, you will find listed:

attribute     Value
Prefix        X
SpiceModel    Contrib/Wurth/WE-FB.lib
Value
Value2        750310471
SpiceLine
SpiceLine2
Description   WE-FB Flyback Transformer\n25uH, ... \nPlease note the disclaimer in lib/sub/Contrib/Wurth/WE-FB.lib.
Modelfile

.. just as it was in the original Würth symbol.

--
Regards,
Tony

Did you consider uploading the rejected material as the group's directions specify. We can't help if we can't see what you have.

This is an incredibly helpful group - it just abhors the disorder and security problems that random uploads and message attachments create.

Donald.