TLV313: No such Fatal error: No such subcircuit: VOS_DRIFT_TLV313

[sleimam]

I am getting error “Fatal error: No such subcircuit: VOS_DRIFT_TLV313” when I am run the simulation for the TLV313 imported model in QSPICE.
1- Imported from: https://www.ti.com/lit/zip/sboma12
2- copied and pasted all from tlv313.lib

what am I missing?

[KSKelvin]

Any chance you didn’t select “Include Entire File” in autogenerate symbol window? For a netlist with multiple .subckt and their calls each other, you can have following method to deal with that.

How to import third-part model of an IGBT with multiple subcircuits?

You have two ways to include all subcircuits In autogenerate symbol window, it has an option “Include Entire File”, select that and all subcircuits will be included in that one line netlist syntax in embedded symbol Or you just take advantage of using autogenerate symbol for generating symbol and pin. After symbol is generated, right click > symbol properties. In library, delete one line netlist and put your library file name there (e.g. Mylibrary.lib)

[sleimam]

I tried both (Include Entire File) and without that option check. it didn’t work

you mean replace this line with tlv313.lib? it did not work either

[KSKelvin]

Does the warning or error message change?

[KSKelvin]

I tested TLV313 Pspice model from TI, there was an illegal character in subcircuit and Mike fixed how Qspice handling, please update Qspice to latest version.

Here is an example to use TLV313 Pspice model to simulate in Qspice.
Circuit follow your setup with a single supply operation. For simulation to run better, .option trtol=7 is required, this is the trtol value that used in Pspice. Without that, simulation may have difficulty when simulate to 2ms. For dual supply simulation, with and without that doesn’t make a difference. Sometime, simulation option play a very important role in dealing with Pspice model.

Parent.TLV313-sboma12d.qsch (12.2 KB)

[sleimam]

Thanks @KSKelvin. it works like a charm!