• GitHub: Teddy-van-Jerry/ngspice-cmos
• Website: spice.tvj.one
• PDF Report: NGSPICE_CMOS_Report.pdf

Table of Contents

• Summary
• Environments
  • Preparation
  • Settings
  • Development
• Definitions
• Sources
  • FreePDK45/
  • Inverter
    • Design
    • Simulation
  • NAND2
    • Design
    • Simulation
  • AND2
  • NOR2
    • Design
    • Simulation
  • AND8
    • Basic Components
    • AND8A (Symmetrical Design)
    • AND8B (NAND4A * 2 NOR2 * 1)
    • AND8C (AND4B * 2 AND2 * 1)
    • Analysis
  • Clock Controlled SR Latch
    • Schematic Design
    • MOS W/L Design
    • Simulation
• License

NGSPICE is a powerful open-source SPICE simulation software in command line, which can efficiently simulate CMOS circuits. Basic logic gates, including NOT, NAND, AND, NOR, are implemented and analyzed. The delay parameters and response plots can help understand the circuit characteristics. As examples, the 8-input NAND gate with three distinct designs is investigated, and the clock controlled SR latch is also simulated to design appropriate MOS parameters.

Note This is the course project of Fundamentals of VLSI Design, Southeast University, 2023 Spring.

Install NGSPICE CLI app. The schematic plot and the PDF report requires installation of LaTeX.

NGSPICE is set to be compatible with HSPICE (see .spiceinit).

My development environments:

• macOS 13 (Ventura) with M1 chip
• NGSPICE 40 (Homebrew version)

Warning There is no guarantee that the provided code can run on other platforms or other SPICE tools. Make changes if appropriate.

Delay:

• tr: rise time (from output crossing 0.1 VDD to 0.9 VDD)
• tf: fall time (from output crossing 0.9 VDD to 0.1 VDD)
• tpdr: rising propagation delay (from input to rising output crossing VDD/2)
• tpdf: falling propagation delay (from input to falling output crossing VDD/2)
• tpd: average propagation delay (tpd = (tpdr tpdf)/2)

Operating corner:

• SS: slow-slow
• NOM: nominal (average)
• FF: fast-fast

This is a 45nm CMOS library. See README for more information.

TNOM is 27C.

Inverter with 1 PMOS and 1 NMOS. (Design Requirement: tr = tf when CL = 24fF)

• inv.inc is the subckt design;
• inv.cir is the CMOS inverter simulation.

Schematic

Designed MOS Parameters

tr = 119ps, tf = 120ps, tpdr = 60ps, tpdf = 64ps, tpd = 62ps.

Source inv.inc

.subckt INV gnd i o vdd
  *  src  gate drain body type
  M1 vdd  i    o     vdd  PMOS_VTL W=360nm L=45nm
  M2 gnd  i    o     gnd  NMOS_VTL W=225nm L=45nm
.ends INV

Simulate with

ngspice inv.cir

Response

The CMOS NAND2 gate is symmetrically designed with parameters for the worst case.

Schematic

Designed MOS Parameters

Source nand2.inc

.subckt NAND2 gnd i1 i2 o vdd
  *   src  gate drain body type
  Mp1 vdd  i1   o     vdd  PMOS_VTL W=360nm L=45nm
  Mp2 vdd  i2   o     vdd  PMOS_VTL W=360nm L=45nm
  Mn1 t1   i1   o     gnd  NMOS_VTL W=450nm L=45nm
  Mn2 gnd  i2   t1    gnd  NMOS_VTL W=450nm L=45nm
.ends NAND2

The worst case is simulated. Simulate with

ngspice nand2.cir

Response

AND2 is NAND2 INV.

Simulate with

ngspice and2.cir

Response

Schematic

Source nor2.inc

.subckt NOR2 gnd i1 i2 o vdd
  *   src  gate drain body type
  Mp1 t1   i1   o     vdd  PMOS_VTL W=720nm L=45nm
  Mp2 vdd  i2   t1    vdd  PMOS_VTL W=720nm L=45nm
  Mn1 gnd  i1   o     gnd  NMOS_VTL W=225nm L=45nm
  Mn2 gnd  i2   o     gnd  NMOS_VTL W=225nm L=45nm
.ends NOR2

Simulate with

ngspice nor2.cir

Response

8-input AND gate. With a large fan-in, there can be several designs. Here we want to investigate the performance of different designs.

The test circuit (defined in add8_test_inv2.inc) involves a 24fF capacitor load at the output, and 8 sets of two stages of inverters for each input. For the inverter in the test circuit, NMOS has W = 0.75um, L = 0.25um, and PMOS has W = 2.60um, L = 0.25um.

The response simulation has the PVT condition of 1.0V, FF, 25°C.

This directly extends the structure of NAND2 into NAND4.

This directly extends the structure of NAND2 into NAND8.

This is the most basic case, extending 2-input NAND to 8-input NAND, before applying an inverter.

Schematic

Response

Schematic

Response

Schematic

Response

Among the three designs (AND8A, AND8B and AND8C), AND8B has the smallest latency, closely followed by AND8c, and the largest latency is observed with AND8A. Compared with AND8A, the fan-in of AND8B is significantly reduced, resulting in lower latency. Though AND8C has an even smaller fan-in, the number of stages in the circuit is larger than that of AND8B. Thus, AND8B achieves a reasonable tradeoff, and has the lowest latency.

There are also some other observations:

• A larger VDD can reduce the latency to some extent, but resulting in much larger power consumption.
• A faster operating corner (FF > NOM > SS) will help cut down latency, but also increases power.
• A higher temperature increases power in return for a reduced latency.

2 PMOS 6 NMOS

Source SR_latch_clk.inc

* .param WL = 5
.subckt SR_LATCH_CLK gnd s r clk q qn vdd
  *  src  gate drain body type
  M1 qn   q    gnd   gnd  NMOS_VTL W=     90nm L=45nm
  M2 qn   q    vdd   vdd  PMOS_VTL W=    270nm L=45nm
  M3 q    qn   gnd   gnd  NMOS_VTL W=     90nm L=45nm
  M4 q    qn   vdd   vdd  PMOS_VTL W=    270nm L=45nm
  M5 ts   s    gnd   gnd  NMOS_VTL W={WL*45nm} L=45nm
  M6 qn   clk  ts    gnd  NMOS_VTL W={WL*45nm} L=45nm
  M7 tr   r    gnd   gnd  NMOS_VTL W={WL*45nm} L=45nm
  M8 q    clk  tr    gnd  NMOS_VTL W={WL*45nm} L=45nm
.ends SR_LATCH_CLK

You need to specify the parameter WL, for example .param WL = 5.

We need to determine the appropriate W/L for M5 to M8. Using a sweep, implemented by alterparam within a foreach loop, we can obtain the following graph.

Clearly, we need W/L > 4.5 (at least 4.2) for the latch to work properly. (M1/M3 and M2/M4 have W/L as 2 and 6, respectively.)

ngspice SR_latch_clk.cir

Response

Copyright (C) 2023 Wuqiong Zhao ([email protected])

This project is distributed by an MIT license.