Spectre error when simulating with extracted view

I'm not sure what would cause this in a Cadence extracted view flow. My guess is that maybe you are using extracted views from a tool other than QRC? Or maybe including a SPICE or DSPF definition of the extracted layout.

If something is defined in SPICE or included as a case-insensitive netlist, then maybe it could clash with another instance which is case sensitive. I tried a simple case and couldn't reproduce it and could find no record of this error message anywhere.

So I'd like to understand how the data was produced, and ideally to see the netlist that is giving the error. Can you log a support request with customer support so that you can share the netlist (if you can't share it here), and then post the case number so I can take a look?

Thanks,

Andrew.

Thank you for the reply Andrew. I don't have any problem in sharing the netlist. How would you prefer? Through the forum, or I can send you the netlist on a private message? I think that posting it here would be a bit bad because the netlist is huge.

Allow me to warning you that I can't go to the customer support because to make the registration I must have  the Cadence License Server Host ID and because I am using Cadence at the university I can't provide that - I don't have access to the ID, as you might understand.

Regards.

EDIT: I forgt to tell you that I took a look at the netlist and there is in fact a 'c2', with this description: c2 (\1939\:gnd_bg \857\:net52) capacitor c2.169e-17.

Another thing is that, even with that error, the simulation keeps running and finishes without problem (not counting with that error).

I don't know if this can tell you something.

I tried to change the capacitor instance name in the schematic but the error persists. Don't know what to do.

OK, I should have searched for the text of the message, not the SFE-400 bit. I've reproduced it with the model files you're using (or a very similar version). I think you must have cut-and-pasted that incorrectly (it was SFE-404 in the log file you sent me too).

It turns out that the error message was actually SFE-404 (I tried a variety of versions and they were all SFE-404):

    ERROR (SFE-404): Multiple case sensitive symbols have been created which match the case insensitive symbol `C1'.

This is covered in solution 11540588 (I know you won't be able to see this), and is related to the fact that the model files have insensitive=yes enabled. The issue is that there is currently a limitation where hierarchical names can't have a mixture of case sensisitive and insensitive components. It is happening because you have the option in your netlist:

saveOptions options save=allpub pwr=all currents=all useprobes=yes

This is causing it to attempt to save the currents for both capacitors and this causes the message. If you rename one of the capacitors, or don't save all currents, this won't be a problem. I don't believe it will affect the circuit though.

It's on the list of things to be fixed - it's just not trivial to fix so hasn't happened yet. CCR 1375493 is one such CCR about this.

Kind Regards,

Andrew.

You have a momcap called C1 and a parasitic called c1. The parasitic you can't control but if you rename the momcap in the schematic to something suitably unique it should then get called the same in the extracted view too. Or you could turn off saving of currents. Or you could just ignore the error!

Hi Andrew. I see. That's what I have been distrusting. So I can change the name of the MOM capacitor to something like C8000 and then go through all the process of LVS and Parasitic Extraction and then try to simulate again the extracted view.

I will try that and give the feedback.

Regards.

Hi Andrew. I have changed the capacitor instance name and then I have ran the LVS and the parasitic extraction and everything is now OK. I can't remove the "save currents" because I need to look at them. That could be a solution though. Thanks for your quick help.