A recent article
https://www.allaboutcircuits.com/te...e-operation-of-digital-components-in-ltspice/
described Spiceline parameters for a logic gate: Trise, Tfall, Vhigh, and Vlow. I tried this and it is great. All seem to work. So far so good.

My question is that I cannot figure out where is a list of valid Spiceline parameters? Just as an experiment, I tried "potato" and of course that did not work. But there must be a list somewhere, and I have no idea where it is?

What bugs the heck out of me: I looked in the Help index for "Spiceline". Help had nothing! It seems to me that if "Spiceline" appears in the Component Attribute Editor, then of course the term needs to be listed in the help files index. But....nope!!

Can someone point me to a list of valid Spiceline parameters ?

 

My question is that I cannot figure out where is a list of valid Spiceline parameters?

Try the LTspice Help/Circuit elements/Special functions.

 

There is no single list of "SpiceLine" parameters. Each device has its own list of valid parameters which can appear on "Value", "Value2","SpiceLine", and "SpiceLine2". In the final netlist all four of those fields are concatenated together.

There are some additional rules you should be aware of for how some symbols are handled.

The attributes SpiceModel, Value, Value2, SpiceLine, and SpiceLine2 are all part of the overall value of the component. In terms of the way the component is netlisted for SPICE, the component will generate a line of SPICE that looks like this:​

​

<name> node1 node2 [...] <SpiceModel>
+ <Value> <Value2> <SpiceLine> <SpiceLine2>​

​

The prefix attribute character is prefixed to the reference designator if different than the first character of the reference designator. The Prefix character and InstName will be separated with a '§' character in this case. For example, if you have a Prefix attribute of "M" and an InstName attribute of "Q1", the name in the netlist will be M§Q1. This allows you use reference designators with a leading character different than SPICE uses to identify the type of device.​

​

There are three exceptions to the above rule. There is one special symbol, jumper, that does not translate into a circuit element, but is a directive to the netlist generator that there are two different names for the same electrically identical node. Another exception is a symbol defined to have a prefix of 'X' and both a Value and Value2 attributes defined. Such a component netlists as two lines of SPICE:​

​

.lib <SpiceModel>
<name> node1 node2 [...] <Value2>​

​

This allows symbols to be defined that automatically include the library that contains the definition of the subcircuit called by the component. The netlist compiler removes duplicate .lib statements. Note that such components are not editable on the schematic. The third exception is a symbol that has other exception is a symbol defined to have a prefix of 'X' and a ModelFile attribute defined. Such a component also netlists as two lines of SPICE:​

​

.lib <ModelFile>
<name> node1 node2 [...] <SpiceModel> <Value> <Value2> <SpiceLine> <SpiceLine2>​

​

Use this method when you want to automatically include a library file yet still want to have an instance of this symbol editable. If the symbol attribute SpiceModel exists and is the name of a subcircuit in the file specified as <ModelFile> then a drop list of all subcircuits names will be available when an instance of the symbol is edited on a schematic.​

​

 

Try the LTspice Help/Circuit elements/Special functions.

Try the LTspice Help/Circuit elements/Special functions.

Thanks a lot. That points me to the list of parameters for the devices in question.

It seems reasonable that the parameters depend on the device being described, so that "Spiceline" might not be the best starting point. But I still think that it ought to have lead me to something; some ideas for a second try. Better than just a "nobody home."

FWIW; it seems that HELP (for software in general) is seldom written from the perspective of the person trying to figure it out. I have been designing power supplies since before many co workers were born but I am better with hardware than with software...

 

There is no single list of "SpiceLine" parameters. Each device has its own list of valid parameters which can appear on "Value", "Value2","SpiceLine", and "SpiceLine2". In the final netlist all four of those fields are concatenated together.

Thank you. That is very helpful. I did enter some parameters into what I thought was the wrong field but it seemed to work anyway, so your point explains that. I am studying the rest of your reply as some of it is a bit over my head... This might take me a while!! :-(

 

Thank you. That is very helpful. I did enter some parameters into what I thought was the wrong field but it seemed to work anyway, so your point explains that. I am studying the rest of your reply as some of it is a bit over my head... This might take me a while!! :-(

Never stop asking more questions as you learn more.