1
\$\begingroup\$

I am trying to simulate the TI part TPS62808 in LTspice, Pspice for TI, and Tina TI. I managed to easily run the simulation in the latter two simulators, but the models were specifically made for them, there is no available model that is specifically designed for LTspice. Thus, I know that general .lib files contain syntax that can be understood by many spice softwares.

So, I downloaded the Pspice package and located the .lib file in the folder -> I opened it with LTspice and right-clicked on the .SUBCKT line -> chose the create symbol option -> changed it visually to fit all text and saved it in a local folder, where i also have my .asc file and the .lib one.

Now I opened my .asc file and placed the part by going to AutoGenerated, built the rest of my network and had my schematic ready to simulate:

strong text

Once I run the simulation, however, there seem to be some issues within the SUBCKT definition and it makes almost 0 sense to me, since I do not know the synthax that well (I know it goes something like component node1 node2 value, but thats about it):

enter image description here

Does anyone know if this is fixable? Thanks in advance!

EDIT: a helpful suggestion regarding double curly braces eliminated the first wave of errors.

these are the ones left now:

enter image description here

I am not sure if these are errors or just warnings (whether LTspice adjusts these coefficients by default), but I am assuming this as the circuit does not work properly and the output response is incoherent.

EDIT 2: I found diode DD1 and changed its coefficient from 0.01 to 0.1 (it was defined as "n" like in the warnings", so that fixed all errors.

However, why is the output still not working properly? It works in the other simulators..

Here are the outputs and settings:

enter image description here

EDIT 3: Okay, eveything is working now, for some reason, the ideal basic components in LTSpice were just not doing it, and I had to select a part for each of my passive components, and the simulation started working. I faced this problem before with switching converters in LTspice, I guess some parameters are missing in the ideal passive components models and those completely stop the simulator from working?

\$\endgroup\$
4
  • \$\begingroup\$ You will need to provide the exact .SUBCKT. (You can, and probably should, test it out first by simply pasting it into the LTspice schematic rather than saving it into a file. But that's a different problem for a different time.) Also, you need to provide the complete .ASY file for your saved symbol. Don't leave anything out! Everything matters. \$\endgroup\$
    – periblepsis
    Commented Jan 11 at 13:48
  • 1
    \$\begingroup\$ TI’s Pspice models aren’t written very well and have a lot of syntax errors which Pspice ignores/overlooks while LTspice does not. I can’t download the subcircuit right now, but most of what you show in the error log screenshot is due to consecutive curly braces {{ and }} being used. You can manually edit the file to remove one of the curly braces in each instance to fix these errors. I suspect there might be more going on though after you fix these though…so update your post with the new information if that ends up being the case. \$\endgroup\$
    – Ste Kulov
    Commented Jan 11 at 13:57
  • \$\begingroup\$ @SteKulov after meticulously eradication all double curly braces, I managed to remove most warnings/errors, the ones that are left are posted as an edit to the post. Thanks! \$\endgroup\$
    – Yordan Aleksandrov
    Commented Jan 11 at 14:11
  • \$\begingroup\$ The remaining things are just warnings. The N for the diode is just letting you know it's limiting it to 0.1 since that's the minimum it can go (which seems to be a new "feature" never explained in the changelog). The other two are just unused nodes because the author created extra components that apparently don't connect anywhere. Like I said before, these PSpice models aren't written too well for generic SPICE usage. Sometimes .options cshunt=1p helps, but in this case it doesn't. Looks like the extra parasitics added by selecting part#'s for the passives helped stabilize the circuit. \$\endgroup\$
    – Ste Kulov
    Commented Jan 12 at 7:53

0

Reset to default

Browse other questions tagged or ask your own question.