Trouble with importin a component from PSPICE to LTSPICE

[bodzio_stawski]

Hello

I have a problem with importing an IC from PSPICE file to the LTSPICE software.

The part is AMC3330. The steps I did:

1) Copied the downloaded AMC3330.lib (extension of the file does not matter) to my Documents\LTspiceXVII\lib\sub
2) Started LTSpice and opened that file
3) Highlighted the component name besides “.SUBCKT”, then right-click and selected “Create Symbol”.
4) Saved that file and got it in AutoGenerated folder (Documents\LTspiceXVII\lib\sym\AutoGenerated)

Unfortunately, when I insert this exact symbol into the diagram, after clicking Run in LTSpice, the RAW window with waveforms/charts stops opening.
There is probably something wrong in this converted file that I am not seeing that is causing the error in this element. So far there has been no problem with other components converted from PSPICE to LTSpice in the same way, but the AMC3330 is a bit more complex.

This PSPICE file comes from exactly here:
https://www.ti.com/product/AMC3330#design-development##design-tools-simulation

I attached the file I converted to the post.
Is it possible that this type of file is simply not convertible to LTSpice? If so, how to recognize such files? I don't have PSPICE software to verify components.

[RoGeorge]

I am usually place the .lib in the same directory with the .asc of the project, same for the .asy, so I can have them all in one place, and add in the schematic ".include AMC3330.lib".  That will keep all the needed files together, without external dependencies that might not be available on another PC, or later in time.

Please attach the .asc file that didn't work, that's the schematic file.  The .asy file already attached is the auto-generated symbol (that's only a collection of lines on the screen), so it doesn't help much with debugging.

[bodzio_stawski]

Thank you for the reply and your advice! Please check the new attachment.

[RoGeorge]

Try the attached one.  Unzip and open the asc in LTspice.  Then run from the unzipped directory, and it should finish instantly, and should plot 2 random signals I've added as a test.  If you want to get rid of those 2 signals auto-opening after each simulation, delete the .plt file.  The 1 second duration was changed to a much shorter time for debugging purpose.

The fix was adding uic (skip initial conditions) at the end of the .tran, or check the corresponding checkbox in the .tran settings window.

The simulation was stuck in "pseudo-transient analysis" which is a step to calculate DC start conditions before running the .tran, and sometimes there might be convergence problems with it.

[bodzio_stawski]

Thank you very much for your help and commitment!

I admit without hesitation that the cause of this problem turned out to be a bit surprising to me. I'm just trying to read a little into these transition states, but some articles

https://www.analog.com/en/technical-articles/ltspice-speed-up-your-simulations.html

says that the ESC button should just interrupt this state/jump over it. This didn't work for me before, so I can only guess that this command is the final and complete solution. Either way, I'll have to read more about this. Thank you!

EDIT:
PS: I've noticed that "Place .op data label" stops working also - it remains grayed-out and unactive as long as this AMC3330 chip is present on the board. Could there be something inside the imported elements that blocks this functionality?

[RoGeorge]

When a .tran starts, it first tries to find the operating point (the .op), then it goes into calculating the time behavior of the given circuit.  For some reason I don't know, in this AMC3300 model the .op step fails.  The 'uic' option skips the .op and procede to transient simulation directly.  So no .op computing attempt when adding 'uic', no data to place on nodes at right click.

The only way left to see the nodes voltage now, is to left click on a node and see it as a plot.  If you need it printed with the schematic, add it as text.

Alternatively, you can try using TINA-TI (the TI's simulator).  It's free to use, but I don't have TINA-TI.  Tried it once, and found it cumbersome for my needs.  TINA-TI and LTspice have different math solvers, and these models were made for TINA-TI, so maybe it'll all just work if you use the TI's simulator.

[bodzio_stawski]

After many attempts, I gave up, and actually using TINA allowed me to recreate this model. Thank you very much for your suggestion.