Hello everyone. i have been tinkering in LTspice with TI's flagship op-amps like OPA1612 and LME49860. I have used the TI models in LTspice with no problem. Except for the new OPA891. Does anyone know how to use the model in LTspice?
maybe it has something to do with the additional pins for adjusting the offset voltage?
maybe it has something to do with the additional pins for adjusting the offset voltage?
The TI SPICE model for the OPA891 has a different pin order than most op amps: In+ In- Out V+ V-, instead of the more common In+ In- V+ V- Out. So you will need a different symbol file for the OPA891.
Attached is a symbol that should work with the TI OPA891 SPICE model. Rename the file to OPA891.asy before using it.
Attached is a symbol that should work with the TI OPA891 SPICE model. Rename the file to OPA891.asy before using it.
I'm glad to help.
There is another way to deal with models that use different pin orders, and that is to create an alias model that remaps the pins to match the symbol that you are using. I don't like maintaining "special" symbols for models that don't conform to usual conventions, so remapping the pin order lets me use a single symbol and store all models compatible with that symbol in a single library file.
If you would like to try this, change the following line in the original OPA891 model file as follows:
Original line:
.subckt OPA891 IN+ IN- OUT V+ V-
Edited line:
.subckt OPA891_ORIG IN+ IN- OUT V+ V-
This just gives the subcircuit a unique name that you aren't likely to actually use (OPA891_ORIG in this case).
Then, add the following lines to the end of the model file:
This will let you use the subcircuit OPA891 with LTspice's built-in opamp2.asy symbol, just like most other opamp SPICE models.
IMPORTANT CAVEAT: the original Texas Instruments OPA891 model file contains an .END statement at the very end of the file. This, as the line suggests, is an end-of-file marker and LTspice will ignore everything after that line. So either delete the .END statement, or make any additions to the file above that line.
I hope this is useful
There is another way to deal with models that use different pin orders, and that is to create an alias model that remaps the pins to match the symbol that you are using. I don't like maintaining "special" symbols for models that don't conform to usual conventions, so remapping the pin order lets me use a single symbol and store all models compatible with that symbol in a single library file.
If you would like to try this, change the following line in the original OPA891 model file as follows:
Original line:
.subckt OPA891 IN+ IN- OUT V+ V-
Edited line:
.subckt OPA891_ORIG IN+ IN- OUT V+ V-
This just gives the subcircuit a unique name that you aren't likely to actually use (OPA891_ORIG in this case).
Then, add the following lines to the end of the model file:
Code:
* Create alias for OPA891_ORIG to reorder pins to conventional In+ In- V+ V- Out
.SUBCKT OPA891 In+ In- V+ V- Out
X1 In+ In- Out V+ V- OPA891_ORIG
.ENDS OPA891
*This will let you use the subcircuit OPA891 with LTspice's built-in opamp2.asy symbol, just like most other opamp SPICE models.
IMPORTANT CAVEAT: the original Texas Instruments OPA891 model file contains an .END statement at the very end of the file. This, as the line suggests, is an end-of-file marker and LTspice will ignore everything after that line. So either delete the .END statement, or make any additions to the file above that line.
I hope this is useful