I am working on IC614 with the techonology IBM7RF. After extracting models from layout by Assura QRC, I tried to do the post-simulation with that extraction. However, a long list of errors (SFE-23) come out in ADE with Spectre simulator. I couldn't find "input.scs" in the model folder of the technology. Could anyone help to locate this file? Or other ideas to fix this error? Thanks in advance.
The input.scs will be in the netlist directory used by ADE, not in the models from the technology. If you do Simulation->Netlist->Display in ADE it should show you the full path to the input.scs in the banner of the window.
Wherever ADE has it's project directory, on Setup->Simulator/Directory/Host , you'll then find under there cellName/simulator/viewName/netlist - it will be in there.
Thanks for your quick reply. I found "input.scs" in the directory you mentioned, and included it in ADE model libraries. Now turns to a new error:
FATAL (SFE-879): Recursive file include or library call: `/home/zheng072/simulation/NOT_test/spectre/schematic/netlist/input.scs'.
Any idea about this error please?
Adding the netlist as a model file makes no sense at all. When you set up a model file, it will add include statements to the input.scs into the input.scs - and so you'll get a recursive include, as you've found - hardly surprising.
You didn't really give much detail as to your original problem, but presumably you need to include the model files from your technology/PDK - and exactly what you need to include is probably documented in the PDK documentation.
I checked the content of input.scs and compared it with the extracted cellview. It seems that all undefined models come from analogLib. For example, undefined model "cmodel" is actually "pcapacitor" in the extraction. I don't know why the input.scs messes up the model name. Then I replaced the word "cmodel" with "pcapacitor" in input.scs, but same error said "pcapacitor" is also undefined model. At this point I am confused, since the schematic simulation with models from analogLib worked just fine, but fails to be defined here. Do I need to include a specific model file of analogLib in input.scs? So far I cannot find any .scs file in analogLib folder. Thanks for your time.
On the QRC Extraction form, go to the Netlisting tab, and ensure that you have Parasitic Capacitor Models and Parasitic Resistor Models set to either "Include As Comment" or "Do not include". You must have had it set to "Include Model".
That's useful if you want to provide a model to (say) scale the capacitance or resistance, but if you don't have such a model, you're best to leave them so that no model name is given. In this case, they'll get netlisted as resistor and capacitor in spectre.
Because I was reading on a handheld device I missed the end of the subject line - I might have realised that was what your problem was (your original posting was a bit confusing) - so my apologies for missing that.