Back Annotation

The above simulation did not actually include the parasitic capacitances and resistances of the interconnect. Spectre (or hSpice) will by default use the gate area (L and W) to estimate the gate capacitance, but additional poly is not considered. If you specified perimeters (ps, pd) and areas (as, ad) in the pcell form, it will include those estimates in simulation. However, it does not include any extra routing, contacts, diffusion, etc. In order to include these, you need to perform parasitic extraction and back-annotation. The extraction is similar to the device extraction you used to extract a netlist for LVS, but now it extracts parasitic resistances and capacitances too.

Your design must pass DRC and LVS to do this.

Extract Parasitics

This is very similar to LVS. Go to Calibre->Run PEX. You will need to specify a layer map like LVS again. Also, select the rule file as this:

/mada/software/techfiles/FreePDK45/ncsu_basekit/techfile/calibrexRC.rul

Under the Input section, in the Layout tab, make sure that GDSII and "Export from layout viewer" are selected. Under the Netlist tab, make sure that SPICE and "Export from schematic viewer" are selected.

Under the Output section, most options should be left as default. By default, "All Nets" under the Nets tab should be checked. Under the Report tab, select "Generate PEX report" and "View report after PEX finishes". Under SVDB, make sure that "Start RVE after PEX" is checked.

After this, there are a few files that were created

• The .pex file ("invx1.pex.netlist.pex") contains all of the parasitics in a hierarchical format like spice.
• The actual netlist ("NAND2.pex.netlist") with only the transistors is the .netlist file.
• The .pxi file ("invx1.pex.netlist.INVX1.pxi") contains the connections between the parasitics and the transistors.

If the above simulation gets too slow, you can run without resistive parasitics but with less accuracy. To do this, change the extraction type to "C+CC" instead of "R+C+CC".

Now, you are ready to run a back-annotated simulation.

Back-Annotated Simulation

To run simulations, copy the .pex, .pxi and .netlist file to your prior spectre simulation directory. By default, this will be "spectre.run1".

Rename the .netlist file to just "netlist". This will over-write your original netlist without parasitics.

Now, re-run Spectre as before, but right before you run, uncheck the "netlist" option to prevent it from generating a new netlist from your schematic as shown here: