open-source-silicon.dev

Who has a working set of Xyce-compatible models for this technology on hand?

(Not a “theoretically working”, or “should be working” set, but one that has actually demonstrably worked.)

If you are kind enough to volunteer (and especially if you’d be kind enough to share), well, I’ll be grateful.

What level of proven? Goes through Xyce sans error? What level of code coverage if so? Has been silicon validated? Is entirely consistent with some other simulator?

The current open_pdks version should be sufficient for most use cases, but I'm not sure what the level of fidelity is currently. I can confidently say that, at the very least, the following github issue will get you most of the way there. <https://github.com/RTimothyEdwards/open_pdks/issues/124|https://github.com/RTimothyEdwards/open_pdks/issues/124>

Thanks - although there’s one of those “should be’s” I explicitly requested _against_ :slightly_smiling_face:

You didn't define what constituted your level of acceptable fidelity. You're gonna get conditionals if you don't do that. Enjoy.

Aloha Dan and Robert ... I need HELP "characterized Sky130 inductor(s)"... Recommendations for  MyFirst Sky130 characterized inductor project?    Recent "inductors" thread Tim and Amro Tork ... <@U016EM8L91B>   [5:44 AM]
There are no characterized inductors in sky130.  There are several inductor layouts and several inductor models, but it's not clear that they match each other, and all of them may come from a variant of the old foundry process that no longer matches sky130.  Check with Amro Tork, who made some inductor structures on MPW-one that he was going to characterize.

<@U01EMEP553N>:  There is definitely an issue that Xyce does not implement level 3 diodes, whereas all the diode models in SkyWater are level 3.  That does not affect basic transistor simulation, but many of the devices are modeled with diodes, which is a problem.

<@U01EMEP553N>:  I did discover that both ngspice and Xyce will not halt on seeing an unknown "option" statement, so that a good strategy is to add *both* the `.option scale=1e-6` _and_ `.options parser scale=1e-6` to `all.spice`, and each of the simulators will issue a warning, but both will run.  I also found that ngspice does accept `;` as well as `$` for to-end-of-line comments (apparently that got accidentally removed from the documentation, because it was in earlier ngspice documentation but removed from later documentation), so I will need to do that conversion in open_pdks. . . .  Both should be pretty easy to do in open_pdks and should make all the devices both ngspice- and Xyce-compatible except for the level 3 diodes.

Thanks Tim.
FWIW there were two edits I hade to make to get the core-transistor models running:
• The `option scale`, as you described, and 
• The SS corner model-file has an “empty” `.param` statement (e.g. a line which is just “`.param`” with nothing else , which Xyce-input won’t take)