IC6.1.8: Introduction to AMS Designer Simulation ( 10 Oct 2025) - RAK : Issue of NMOS and PMOS transistor not in its range of parameters

I just quickly went through the steps in the RAK until pressing the run button on page 28, and it runs successfully for me (I'm using a newer XCELIUM and SPECTRE version but that really shouldn't matter).

Please check two things:

1. In the netlist (Simulation->Netlist->Display) does the inv module look like this: (particularly the w and l values):
   

   module inv (Y, A);
   output Y;
   input A;
   wire (*
   integer inh_conn_prop_name = "bulk_n";
   integer inh_conn_def_value = "cds_globals.\\gnd! "; *)
   \bulk_n_gnd! ;
   wire (*
   integer inh_conn_prop_name = "bulk_p";
   integer inh_conn_def_value = "cds_globals.\\vdd! "; *)
   \bulk_p_vdd! ;
   nmos1 #(.w(1e-06), .l(1.8e-07)) M1 (Y, A, cds_globals.\gnd! , \bulk_n_gnd! );
   pmos1 #(.w(2e-06), .l(1.8e-07)) M0 (Y, A, cds_globals.\vdd! , \bulk_p_vdd! );

   endmodule

2. Please check Simulation->Options->Analog(Spectre) on the Component tab. Check that scale and scalem are both 1 (not 1u for example). I could get it to fail with 1u (for scale). The default should be 1, but maybe in your environment it's changed?

Andrew

Thanks, the scalem was set to 1u, that is the issue.

Thanks, the scalem was set to 1u, that is the issue.