[SOLVED] Post- simulation use calibre pex view, all parasitic capacitance connected to a net 0

hi everybody,
i am doing post-simulation using calibre view, I found all the parasitic capacitances connected to a net called “0”。
It is a floating net, the voltage on the net is floating.
and the smimulate result is wrong. anyone who know why all parasitic capacitances connected to the net.

a part of pex.netlist is follow

Hi Andy-

I haven't used xRC in several years, but back when I did, net 0 was reserved for substrate. Are you doing multiple power domains? Particularly with the old versions that could be tricky to set up correctly. What version are you using?

Best-

Sam.

Net "0" is usually a (default) ground net.

Check your extraction settings - if you want to see coupling capacitances between the nets in your post-layout netlist, you should not be grounding them (this is what's happening in your netlist now).
You should select extraction mode "RCC" or something like that (also called coupled RC extraction - as opposed to decoupled RC extraction - what you are doing now).

But it's strange that net "0" is floating in your simulations, it should have zero potential.

timof said:

Net "0" is usually a (default) ground net.

Check your extraction settings - if you want to see coupling capacitances between the nets in your post-layout netlist, you should not be grounding them (this is what's happening in your netlist now).
You should select extraction mode "RCC" or something like that (also called coupled RC extraction - as opposed to decoupled RC extraction - what you are doing now).

But it's strange that net "0" is floating in your simulations, it should have zero potential.

Click to expand...

thanks for your reply, timof,
i select C+CC mode.
My circuit have two ground， AGND and DGND, when i do simulation, i use analogLib vdc symbol, and set to DC value 0, to set AGND, DGND to zero potential.
you say the net "0" is substrate. how do i set the net "0" potential? like the way AGND,DGND? or leave it alone?

I am not saying that net "0" is substrate - it is a "ground".

There should be a command in your extraction tool command file (or GUI) that defines the net name for "ground".
You can set it to AGND or DGND values (strings).
Or, you can keep it to be called "0", but set it to 0 voltage in your simulations.
(I thought that a SPICE simulator sets net "0" to zero voltage by default).

The concept of "ground net" is one of (but not the only one) the most confusing ones in parasitic extraction.
"ground" in extraction can be a real net (like AGND), or a virtual one (like "0").
Virtual means that there is no such net in your design, it is added by the extraction tool.

If you select decoupled C extraction mode - all capacitances are "grounded" to "ground" net.

Also, in coupled C, or coupled RC (or RCC) extraction mode, capacitive couplings that cannot be associated with any real net are assigned to net "ground".