This thread has been locked.
If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.
Hey team,
I'm trying to simulate the TLV62150ARGT converting a 12V supply down to 5V at 1A. I know this is pushing the maximums outputs, but I think it should be fine. Webench suggested the following build which I reconstructed in ti-spice after having mixed up the FB / PG pins which are conveniently reversed in spice:
Output of the circuit:
I double checked the wiring and values, so I would love to hear your thoughts on this. I am also open to hearing any suggestions on how to decrease run time for the simulations as these are taking quite a while on my laptop.
Do I need to use an analog ground for AGND,PGND, and PAD? Does this affect the spice simulation? I haven't simulated a device yet that needs a different ground.
Cameron,
Must have something to do with initial conditions and convergence. Wiring looks fine to me. Attached file has the same setup that you have and the sims work fine on this one. slvm506a.zip
I added an IC on the output net and also have some parasitics on all the major LC components. You can speed simulation by reducing the sim time overall (change TD, TR, TF, PW. of the load pulse as you already have a pretty fast startup with small SS cap) and also increasing the max time step under simulation profile options but this will come as a compromise to the accuracy of the waveforms.
Thanks,
Amod
Thank you both so much for taking the time to answer my question - I've been running in to such odd problems with ti-pspice on my end that are just baffling. I'll run with this today / tomorrow and see how things go, I'm a little worried that my library might be corrupted. I think I'll test this by deleting the part from the schematic Amod shared and see what happens when I reinsert it from my library.
Kevin, I did get to see the note you left via my email and I appreciate the advice on the simulation speed level setting - I was looking at that and wondering if it affected anything. When I googled it, I only found articles talking about how it helped with simulating different version files.
Sure Cameron, let us know how this testing goes. Apart from the speed level setting that Kevin suggested, you can just directly go into simulation profile and change the maximum time step to a larger value to speed up sims with a little compromise on accuracy.
Thanks,
Amod
Well team I must admit I am quite confused by this - I took Amod's simulation and it ran fine, I then removed the TLV model and placed mine from my library and it again worked properly. I then went back to my project, replaced the tlv model, but got the following result. It seemed to be working until something random happened.. the only difference I can see between our two models is an increased separation of grounds. My simulation profile of course is slightly different, but that should not be causing the aforementioned differences!
Again, I appreciate all the help! I attached my project this time - I was using the transient simulation profile.Power Project-PSpiceFiles.zip
Cameron,
I have requested the PSPICE team to take a look at your project.
Thanks,
Amod
A valid archive? Did I zip the wrong file?
Sorry I haven't shared a pspice project prior to this.
I resaved the project and confirmed this has both the OBJ and DSN file, let me know if there is something missing. I also realize I should mention I have this error when opening up my project, but not Amod's:
This merely tells you that your sim profile contains a model library file that is not inside the same folder where your project is. This is a common reason that zipped up project does not work on someone else's computer. it's a warning, not an error.
-JC
Cameron,
You have 2 pages under your schematic, "page1" and "redesign 5v/1a". Please note that schematics are the minimum entity to be simulated. Every simulation profile name contains the name of the schematic they are set for. So, if you don't need to the circuit on page 1, please delete it and try again.
Let me know if both pages should be included. There might be some undesired interactions.
Regards,
JC
Deleted the additional page, the issue persists Power Project Deleted Page.zip
Cameron,
When I tried to run the simulation, this message showed up in session log:
WARNING(ORNET-1085): Your design does not contain a Ground (0) net. You may not be able to run analog simulation on this design. To run analog simulation, your design must have at least one Ground (0) net. Use at least one PSpice Ground (0) symbol in the design. Ignore this warning, if this is a digital design.
After placing a true zero volt ground (click "Place" - "PSpice component" -> "PSpice ground"), I reset the simulation options and got this:
Hey JC,
I tried replacing my ground with the specific Pspice ground and nothing changed on my side. Did you do something more than simply replace the ground that I had in my simulation? Maybe I'm not sure what you mean by reset the simulation options, I assumed just reran the simulation.
Here's the output from my simulation log:
INFO(ORPROBE-3183): Simulation running...
** Profile: "SCHEMATIC1-Redo_for_JC" [ c:\users\a0234072\documents\mass market rotation\independent study\power\pspice for power\po
Reading and checking circuit
WARNING(ORPSIM-15246): Library index file LMR50410X_TRANS.ind does not have the correct format
INFO(ORPSIM-15422): Making new index file LMR50410X_TRANS.ind for library file LMR50410X_TRANS.LIB.
Making index file for library C:\Users\a0234072\Downloads\LMR50410X_PSPICE_TRANS\LMR50410X_TRANS.LIB
Please be patient. This may take several minutes...
WARNING(ORPSIM-15223): Library file C:\SPB_Data\cdssetup\pspTILibDir\nom_pspti.lib has changed since index file nom_pspti.ind was created.
WARNING(ORPSIM-15227): The timestamp changed from Tue Dec 8 08:32:23 2020 to Mon Dec 14 08:43:53 2020.
INFO(ORPSIM-15422): Making new index file nom_pspti.ind for library file nom_pspti.lib.
Making index file for library C:\SPB_Data\cdssetup\pspTILibDir\nom_pspti.lib
Please be patient. This may take several minutes...
Circuit read in and checked, no errors
Calculating bias point for Transient Analysis
Hey JC,
Why does that fix the problem! I mean I'm not mad that it works, I'm just very confused.
Was something odd happening in the autocorrelation feature due to the loose tolerances?
Hi Cameron,
At each time point the simulator starts from the circuit solution from the previous time point (the first starts from the time zero solution) and iterates to get an accurate answer governed by the the tolerance settings. If these are set too loose like in this case, you spend less time iterating but the accepted solution is pretty far from the reality so the next round of calculation starts off of a bad "initial condition". It is possible that the error accumulates to a point that the solutions start to diverge from what should happen.
Regards,
JC