Yet another LTSpice Conversion Support Request - TI TPS7A85

QSPICE
1

Mike:

Thanks for all the work here on another Spice Sim! I’m coming up to speed on this simulator and have run into an issue.

I am working on converting a TI LDO Regulator implementation from LTSpice. This is to gain some experience with QSpice and compare performance/capability. TI’s Spice model is 10 years old, is not encrypted (as they like to do), and has only received one revision in that time. Link for your direct download other than what I have included:

TPS7A85 data sheet, product information and support | TI.com

I’ve ported/included the model into the schematic with some very basic R and C elements around the X component to generate 3.3V from 5V. The LTSpice schematic I have implemented is more complicated to perform some component parameterizations for families of curves, and LTSpice doesn’t complain of issues during the simulation runs.

QSpice has several complaints including:

  • Warning: Ignoring unknown instance parameter….
  • Warning: Unexpected number….
  • Fatal error: … Gain was not specified

I’ve narrowed some of the causes down to:

  • Preceding/unnecessary parenthesis combined with spaces – probably for readability in setting up the model
  • Qspice interpreter requiring explicit ‘=’ for an E component in a VALUE based implementation syntax. I’m not sure if the author had sloppy style, or if LTSpice has been modified to accept a missing ‘=’ when the PSPICE syntax requires it.
  • There are other causes that I haven’t been able to track down and resolve.

I’ve corrected the VALUE and ‘=’ items, which has reduced some of the complaints. However, it has not addressed the bulk of the warnings. And certainly not the FATAL crash.

I’ve searched through the forums for hints, and it looks like there has been much effort placed in polishing the ‘garbage in’ syndrome for syntax.

I’ve attached the original 3rd party model from TI for the LDO, and my QSpice schematic. I’ve changed the extension from the TI .LIB to .TXT. Please let me know if there is anything else I need to provide.

Thank you for your time and assistance!

TPS7A85_3V3.qsch (20.2 KB)
TPS7A85_TRANS.txt (9.6 KB)

2

The problem you encountered is not related to TI model file. You changed {} to () in model file for E-source and it actually causing problem, E-source legacy syntax needs {}.

The real problem lies in your .trans 15m startup. In Qspice, its only accept .tran and there is NO startup option in .tran. In short, what actually stopped you to run this simulation is incorrect syntax for .tran. To use something similar to startup, you replace DC source with PWL to give a 20us ramp, and you already have that in Vin. For troubleshooting a library (.subckt), I suggest to use .lib to call that library instead of making it as an embedded subckt symbol, in this way, you can use a text editor to modify the library to see what is going on. But again, I don’t think problem lies in the library.

Here is the modified schematic that can work. Also rename TI .lib file into .txt for easy editing.

TPS7A85_3V3 (modified with .lib).qsch (13.6 KB)
TPS7A85_TRANS.txt (9.6 KB)

You still get warning, but I didn’t go into detail. As they mainly related to shorted resistors (it can happen for poorly written subckt), and diode warning is that if parameter TT is not zero, Qspice need finite VP value in diode. This is automatically fixed by Qspice.

image
image1247×607 44.7 KB

3

Thanks! I see the fixes. The .LIB component had the parentheses implemented instead of braces. I guess that is something that needs to be considered when running through different tool sets.

StevenB