开云体育

Good morning, I have a question about symbols.

Could a symbol be automatically generated from a (.lib) or (.sub) file??..
In this case it would be a comparator.

?

If so, how could I generate it?

Yes, symbols can be automatically generated from any text file containing a valid .subckt. It doesn't matter what the name of the file is. It can be a .lib or .sub file, but it doesn't have to be.

The procedure is simple.

1. Open the file in LTspice. this most easily done by dragging the file from Explorer into LTspice.
2. Right-click with the mouse on the .subckt line.
3. From the drop-down menu, choose Create Symbol.
4. Save.

Whether this is a good idea, or not, is another matter. You will get a rectangular box with the correct pin names, but not necessarily in appropriate places. Nobody will know for sure what kind of component it is. You could delete the box and draw a proper comparator outline, for example, and re-arrange the pin positions. But many people don't bother, and it is often difficult to figure out what a schematic does that uses them.

So, here are some alternatives:

1. Look for an LTspice standard symbol that is appropriate for the type of component.
2. If it also has the correct pin configuration, use it with modification.
3. If it doesn't you can make a copy of the standard symbol, and edit it to have the correct pin configuration.
4. Draw a new symbol from scratch.

--
Regards,
Tony

开云体育

Thanks for answering
That's what I'd like to do..
Find a symbol that looks more like a comparator.
My question is, where do I look for it??' within Ltspice??
And if I find one, how can I associate the appropriate PINS to my comparator?

If your comparator has 5 pins, you can start with the LTspice opamp2 symbol.

The most important thing is for the symbol pin order to match to the order in the .subckt line. The pin names do not have to match. If they match, then you only have to change the opamp2 symbol's value to match the .subckt name, and you're good to go.

But, honestly, if you can draw schematics, you can also draw symbols. It's not hard, and once you have had a little practice, you will never use auto-generated symbols again, and we will all be glad.

Did you look in:

Help > Schematic Capture > Creating New Symbols ?

--
Regards,
Tony

开云体育

Can I remove it from the rectangle and load the symbol for a comparator from a library?

No, the symbol editor lacks many of the features of the schematic editor. You cannot drag items from one symbol into another, like you can with schematics.

--
Regard,
Tony

开云体育

Help?? where?? in this channel?? Or in LTSpice

The LTspice Help. Just hit the F1 key.

Haven't you ever read the Help?

--
Regards,
Tony

开云体育

He abierto la ayuda con F1, pero la ventana que se abre, no contiene nada.

What version of LTspice are you using?

The F1 key works on V17.1, V24.0 and V24.1. If you're using one of those and it doesn't work, your installation may be missing the help file.

--

开云体育

The F1 key does work, a window opens, but nothing of what you're telling me appears
Help > Schematic Capture > Creating New Symbols ?

For V17, the Help has an additional heading:

Help > LTspice > Schematic Capture > Creating New Symbols

If that doesn't work, there is a recent PDF version of the Help in the Files section of the group's website: LTspice Manual. You could download it onto your Desktop.

--
Regards,
Tony

开云体育

If that doesn't work, there is a recent PDF version of the Help in the Files section of the group's website: LTspice Manual. You could download it onto your Desktop.

I mistakenly linked to an older version, but I don't think it had changed much. Newer version: LTSPICE_Manual

--

1. Verify that the comparator model's subcircuit has the same number of pins in the same order: In+ In- V+ V- OUT.
2. Change (edit) the name next to the opamp2 symbol, from "opamp2", to the actual name of the subcircuit of your comparator.? The name of the subcircuit is the name that you see immediately after the command ".SUBCKT", when you examine the contents of the library file.? It is NOT the filename name of the file.
3. Additionally, include the library file into the simulation, by adding this SPICE Directive anywhere on your schematic: ".lib filename.ext" where you use the actual filename.ext of the library file.? If that library file is not already in the same folder with the schematic, nor in one of your Model Library areas that you may have already set up in LTspice's Control Panel, then the filename should also have the relative or absolute path to the library file.

• .lib MyComparator.lib
• .lib models\MyComparator.lib
• .lib ..\models\MyComparator.lib
• .lib \Mymodels\comparators\MyComparator.lib
• .lib "C:\Users\MyName\My Documents\My LTspice Models\comparators\MyComparator.lib"