I think @bordodynov’s example used the same model as the TI website. Here is the replication of the datasheet Figure 6-5, showing astable operation with the TLC555 model directly downloaded from TI. Without your schematic file, it is hard to determine what is wrong in your model import or setup. Just two things to remind:
- This model consists of different subcircuits. In the auto-generated symbol window, make sure to select “Include Entire File.”
- This model only works with zero initial values; therefore, UIC must be used in the .tran directive.
About the warning in Qspice
If you study this model, there are equations to calculate a parameter VT, but VT is not defined in this model. Therefore, Qspice warns that these values cannot be resolved.
for example, line#321 : .MODEL DZ_18V D( IS={ISz} N={Nz} BV=18.0 IBV=5.0M EG={8*Nz*VT})
For the warning about LAMBDA, the model is a level 3 NMOS, where LAMBDA is not a model parameter.
for example, line#130 : .MODEL TLC55X_NMOSD_HV NMOS LEVEL=3 L=10U W=100U KP={KPN} VTO={VTOHN} LAMBDA=2E-3 THETA=1.8E-01
Parent.TLC555.qsch (16.0 KB)
