Hello

Is Hierarchy Editor / SimVision are capable to "view" insite of Spectre netlist in form of subcircuit.

Regards.

Pavel.

Thank you for answer

Quote:


I did it already, but the AMS behaviour is different from one of Spectre.

Spectre behaviour was tested under Analog environment. It's reference for the moment.
Now we need the same block in AMS Designer. I converted block in AMS and simulated it in AMS Designer.
Its behaviour was different "Reference Spectre subcircuit", simulated in Analog Environment.

This morning I tried to instantiate "Reference Spectre subcircuit" in AMS Designer.
Its behaviour was also different from one, simulated in Analog Environment behaviour.

Pity, that I can't see inside of the Spectre block in order to troubleshoot behaviour mismatch.

Regards.

Pavel.

Pavel,
There are two ways to take the spectre/spice netlist as sub blocks into AMS designer for mixed-signal verification.
1st method
  . In HED , you can directly switch to the block from anyother view to "sourcefile"
       It's easy in HED -> select one cell -> set cell view -> sourcefile
           In source file browser form , you choose spectre/spice netlist.
   After this done , the block bind to the spectre/spice source file
   
   Note.  if you have level up schematic/verilogams/verilog instantiate this spectre/spice netlist which has the bus connectiion says
     
            cellA I0 (.A(X)) ;     // X and A say 4 bits bus
 In fact the spectre/spice netlist does not have bus , they are all scalar for example
          subckt cellA A_0 A_1 A_2 A_3

  Then, you need to define sourcefile_opt in HED
           HED -> view -> properties(on)
              You will see the sourcefile_opt colum in HED
           type-in
                -auto_bus  -bus_delim _

 So that AMS will merge A_0 -> A_3 to be A[0:3] and match the level up bus connectivities .
 This is compresive solution for bringing spice/spectre block as sub block for the AMS verification.

2nd method.
If you don't have bus/scalar situation
         You can also simply switch cellA to syymbol and add the spetre/spice netlist into you modelfile .

BTW, to probe the simulation result in spice netlist. you can't use tcl from simvision. You need to save the signal within spice block via analog control file. It can be done in AMS-in- ADE GUI which generated control file automatically  or standalone analogcontrol file provided by user and load it in AMS-in-HED GUI

Hope this helps .