On Sat, Dec 21, 2024 at 12:49 AM, <info@...> wrote:

It gives the same error every time:

" Unknown subcircuit called in:
xu1 0 n002 n003 v+ v- tss/opa891_model_v1p1.lib opa891"

There are multiple problems with that line, pointing to a few mistakes.

 

The pin-order is all messed up.  It seems to have connected the input pins to net N002 and ground, the power pins to nets N003 and V+, and the output goes to net V-.  That can't be right.  Did you alter the pin-order of the symbol?  Don't do that.  Did you mistakenly use package pin numbers, thinking that the ORDER of pins is the same as the package pin number?  Don't do that either.  SPICE/LTspice does not want to know what the package pin numbers are.

 

The name "tss/opa891_model_v1p1.lib" is stuck in there where it does not belong.  That might cause LTspice to try to find a subcircuit by that name.  Of course it does not exist.  Furthermore, I believe that the model file itself was never being loaded at all.  That would surely cause problems because LTspice would be totally unaware of that subcircuit, so it would indeed be "unknown".

 

I strongly suggest deleting the SpiceModel attribute, and use the ModelFile attribute instead.  The SpiceModel attribute does not necessarily refer to a filename that you want to be loaded.  It does in the unique case where both the Value and Value2 attributes are defined, but I think not otherwise.  You probably did not use it that way with both Value and Value2.

 

People can get themselves in trouble by trying to use LTspice in ways it was not supposed to be used.  And then they waste time trying to fix problems that they made for themselves.

 

Andy