Electronic – HSPICE command naming weirdness

edahspicesimulationspicesynopsys

I have a simple digital invert circuit using ASAP7 nmos and pmos transistors. When I use Synopsys HSPICE to simulate the below script, it throws an error Definition of model/subckt "nmos_rvt" is not found for the element "xinv1^xm1". Please specify a defined model/subckt name.

However, when I change xm0 to mm0 (and xm1 to mm1) everything works! What is wrong with using xm0 as the instance name? Where is this documented?

The script:

** Generated for: hspiceD
** Generated on: Feb  2 16:49:44 2021
** Design library name: demo
** Design cell name: invtest
** Design view name: schematic
.GLOBAL vdd!


.TEMP 25.0
.OPTION
+    ARTIST=2
+    INGOLD=2
+    PARHIER=LOCAL
+    PSF=2
.INCLUDE "7nm_TT.pm"

** Library name: asap7ssc7p5t
** Cell name: INVx1_ASAP7_75t_R
** View name: schematic
.subckt INVx1_ASAP7_75t_R a y vdd vss
xm1 y a vss vss nmos_rvt w=81e-9 l=20e-9 nfin=3
xm0 y a vdd vdd pmos_rvt w=81e-9 l=20e-9 nfin=3
.ends INVx1_ASAP7_75t_R
** End of subcircuit definition.

** Library name: demo
** Cell name: invtest
** View name: schematic
xinv1 in1 out1 vdd! 0 INVx1_ASAP7_75t_R
v0 vdd! 0 DC=700e-3
c0 out1 0 2e-15
VIN in1 0 0 pulse 0 0.7 0 50p 50p 2n 4n 
.tran 10p 10n
.END

```

Best Answer

This is standard SPICE syntax and I suspect it is documented in many places. Instance names for MOSFETs must begin with M and instance names of subcircuits must begin with X. Voltage sources start with V, resistors start with R, and so on. The first letter tells SPICE how to parse the rest of the line.

It gets tricky when a MOSFET is actually described using a subcircuit rather than directly with a MOSFET model, but if it's a subcircuit then it needs to start with an X.

Related Solutions

HSPICE node naming convention

From the hspice perspective and how it simulate circuit BIT0:5 and BIT0:6 are separate nodes.

Regarding the naming convention extraction program try to keep the name of the nodes the same as in schematic(for circuit designer convenience). However sometimes it is not possible -> for example if using RC extraction one metal path will be represented by several cascaded circuits like so:

BIT0       BIT0:1        BIT0:2         BIT0:3
    R1             R2             R3
---/\/\/\----|----/\/\/\----|----/\/\/\---
            ---            ---
       C1   ---         C2 ---
             |              |
            ___            ___

So this naming convention is just a mark that those nets correspond somewhat to schematic net.

How to use PTM corner models in hspice

Typically the value is passed on the command line at the time of evoking the run.

Here is the setup line from my simulator which has the ability to read several different library hierarchies:

foundry/process-name/mosst/param.lib 3s; -> that says use the 3 sigma values 
foundry/process_name/mosst/model-name.lib wp -> that says use the wp values 
 - wp here is similar to FF,TT,SS etc.

note: file names are changed for confidentiality reasons

The actual file that the simulator uses is assembled at run time through a series of calls that are like ifdefine statements used in compilers. Here is a snip from a *.lib file

.lib tm
*bsim3v3
.include ./models/bsim3v3/parameter-name.par
.include ./models/bsim3v3/nmos-name.mod
.include ./models/bsim3v3/pmos-name.mod

This reads as "if the called library is tm then include these files in the subdirectories"

If you are using a graphical tool there will be command parameters that you have to set that get passed to the spice executable. If you are running from the command line this will go in to your scripts to call the spice executable.

Temperature is set as a global parameter and SPICE uses it to change the models.

Monte Carlo simulation uses process corners, Voltage and Temperature and schmoos the design (and can be used to schmoo the W/L and stray capacitances at higher levels) to see the safe operating area. It is very computationally intensive.

Corner analysis is much more and can be viewed to be setting the outer limits that monte carlo must stay within.

I would recommend that you snoop through the library directory and under stand how things are called. I bet you'll find stuff in the library that would surprise you.

Related Topic

Electronic – Generate HSPICE input signal