The difference of extracted view and analog_extracted view

analog_extracted

Hi, all

I am wondering about the difference of extracted view and analog_extracted view, at very beginning, I used the extracted view for post-simulation, and now, somebody told me that I should use the later one. However, nobody can tell me the reason, and also I can not see any difference from the simulation results.
So, what's the difference between them, and the reason for using analog_extracted for post-simulation?

Thanks a lot in advance

extracted view

extracted_view is generated either by Diva or Assura which includes all the extracted devices and parasitics.

You can run a simulation directly from the extracted_view.

The analog_extracted_view is generated from the MSPS flow and can be used
to create a subset of the extracted_view, with only selected nets or parasitics.
This then generates the analog_extracted_view.

In the old days, Diva required the Build Analog to be performed on the extracted_view to generate the analog_extracted_view for simulation, but this is no longer needed (for many years now). The analog_extracted_view is basically
legacy. If you are simulating the entire extracted_view it is not required.

After an Assura RCX/QRC extraction, open the extracted_view and do a Tools->Parasitics->Refine Extracted View... You can still generate the analog_extracted_view for selected parasitics using sbaLib devices.(very convaluted flow and not needed since selected net extraction can be performed instead now).

analog extracted view

eda_rimrunner, thx very much for your reply, it makes sense I think.
But I still have one question on how to select the nets if I only need some of the parasitics during the build analog process.
Can you show me the process detail, thank you in advance.

generate extracted view

It is much easier to do a Selected Nets Proper with QRC extraction, but
if you insist on the Build Analog method....

The options are:

1) Include All - Simulate with all the parasitics that have been extracted.

2) Set From Schematic - Select parasitics to include in the simulation by placing
special symbols (spresistor, spcapacitor, spinductor,
and spcapacitor2) on nets in the schematic view. The
spcapacitor2 device is used to include parasitics in the
simulation that appear between two specified nets. If
you add or remove symbols from the schematic, click
Check and Save to save the modified view.
The parasitics you select by placing these symbols
(which are provided in sbaLib) are the only ones
included in the simulation.
Note: The sbaLib can be found at the following location
in the Cadence installation:
<installation_dir>/tools/dfII/etc/cdslib/artist/sbaLib
To define this library in your cds.lib you need to set
the following:
DEFINE sbaLib <installation_dir>/tools/dfII/etc/cdslib/artist/sbaLib

If you choose Set From Schematic and click OK
without identifying any nets on the schematic, the
Extracted Parasitics Selective Annotation form asks you
to confirm your choice.

3) None - Simulate with none of the parasitics.