Hello,
I created a project to verify the functionality of the REF5025ID precision reference in Kicad v.8.06, using TI’s SPICE model. However when I tried to run the DC operating point simulation, Kicad abruptly shut down with no error message shown. More specifically, when I tried to create a new DC op. analysis tab, shutdown occurred even without clicking the RUN button. This was while using my Windows 11 laptop.
To troubleshoot this, I tried to open the same project on my Windows 10 tower PC, also using Kicad v.8.06. However I received a file already open message (see screenshot), referring to my laptop (“4K-Field-PC”), which was fully powered off (and Kicad not running when I shut the laptop off). Both PC’s use Dropbox as my file repository.
The ZIP file attached also includes a different op amp project, the LMC6484. The simulation for this device works properly on my laptop. Also, I was able to open the same project on my tower PC with no file already open error.
Is something wrong with my REF5025ID project? Thank you for your help.
That is a non existing KiCad version. (Strangely a common and stubborn mistake many people make). I guess you mean V8.0.6. I recommend to start with updating to V8.0.9. Increments in the third number are bug fix updates, and a lot of bugs have been fixed in those three updates.
I see there is a stale lock file in the 5025 project. It looks like: ~REF5025ID.kicad_sch.lck those lock files should be deleted automatically when KiCad closes, but when KiCad crashes these files get left behind. You can also click on the Open Anyway if you’re sure there is no other KiCad instance open with the same project.
Continuing yet again…
While attempting to run the simulator, I get:
I fixed the schematic symbol, so it uses the also provided model, and when I run the simulator then, KiCad also crops out with a segmentation fault / Core dumped. (And this is of course why the lockfile was present in the first place.)
Digging a bit deeper I noticed that the pin assignment in the current project I modified is different from a backup in your zip file:
I’m not sure what it should be. But KiCad should not crash on that I think but either give some error message, or just let the emulator run haywire with faulty results.
Thank you for diving into this. I’ve been using my laptop for my Kicad work, which accesses all the project files directly from the Dropbox directory in its local hard disk. Occasionally I will be also using the tower PC, but I’ll need to be sure that all the project files are mirrored onto that PC’s Dropbox hard disk directory. Perhaps the lock files that didn’t close when the laptop Kicad shut down (and were saved to Dropbox) caused the tower PC Kicad file still open message?
I downloaded Kicad v.8.0.9. Can I uninstall v.8.0.6 and install v.8.0.9 without having to reassociate all the symbols, footprints and SPICE models in my main project? The projects I uploaded here represent just two of the many op amps that my main project uses.
I have checked the files, made a new setup and did the following:
Inspect->Simulator->Edit Analysis Tab-> choose op–>uncheck ‘Save all power dissipations’
Use the correct model of a 5025 (you have attached the model for 5010, which is the 10V reference, and which will not run with 5V input).
The pin assignment is important. The one shown as ‘backup’ above is correct.
Then the simulation is running, the output is 2.50 V.
Thank you, With my project now showing 2.50V output with the correct model file, I’ve attached a screenshot of the pin assignments I used (which were the same as before. I was not sure of the distinction between the numbers in parentheses vs. the preceding numbers).
As you noted, I still needed to disable the power dissipation option for the analysis to run. Should I upgrade to v.8.0.9 to fix this? If I uninstall v.8.0.6 and install v.8.0.9, will all my symbol, footprint and simulation model linkages be preserved?
You don’t have to uninstall V8.0.6. You can just install V8.0.9 over it. All those links you mention are in your project, and upating KiCad does not change anything about that. But sometimes there are small library changes, such as for example a library being renamed of a new library added, and those changes are (I think) not always updated when KiCad is upgraded.
For the latter, a trick you can do is to rename KiCad’s configuration directory. This way KiCad does not see it anymore, and then it creates a new directory with defaults. Renaming also also automatically results in a backup. But of course you should always have backups of any precious data on external drives.
But for the crash, I also had KiCad V8.0.9 crash with your old version (I did not change the "Save all power dissipations) thing), so for you it would probably also not change much.
On Windows, simply running the 8.0.9 “Lite” installer will upgrade all of the executables, fixing hundreds of bugs since 8.0.6 and leave all the libraries alone.
A temporary fix: Use the symbol editor to edit symbol U1: replace the pin name Temp by Tem (or any other than Temp). Then op sim is o.k…
Background: Temp in PSPICE is a reserved word for temperature. In ngspice this is Temper. There is a function to replace Temp by Temper. Then of course here the node is no longer found by the simulator. This only happens as node Temp is unconnected. If connected, its name will be replaced by the connecting node, then nobody does care.
A fix is tricky, as one has to detect this very special situation in (potentially) huge netlists. Let’s see …
