Bistable Latch Circuit

【MAL-Seeker Circuit Equation Test】DC operating points of cross-coupled inverters

$$v_1=f(v_2),\qquad v_2=f(v_1)$$ $$f(v)=0.5-1.4(v-0.5)+2.0(v-0.5)^3$$

2-Variable Cubic Circuit Model
Physical Operating Points: 3 / All Real Roots: 5 / All Complex Roots: 9

1. A minimal model that remembers 0 or 1

A bistable latch retains one of two states by feeding the output of each inverter back to the input of the other. In the SPICE netlist, each stage consists of a load resistor and an NMOS transistor: the left output $q$ drives the right-hand gate, and the right output $\overline{q}$ drives the left-hand gate.

The circuit is small, but an operating point must satisfy both feedback paths simultaneously. The first test is whether the solver can capture the central symmetric point as well as the two asymmetric points corresponding to complementary logic states.

Transistor-Resistor SPICE3f5 Netlist

Resistor-loaded NMOS bistable latch

VDD vdd 0 1.0

RL1 vdd q  10k
RL2 vdd qb 10k

M1 q  qb 0 0 NMOS_LATCH L=1u W=20u
M2 qb q  0 0 NMOS_LATCH L=1u W=20u

.model NMOS_LATCH NMOS (LEVEL=1 VTO=0.35 KP=100u LAMBDA=0.02)

.nodeset V(q)=0.95 V(qb)=0.05

.op
.end

2. Simplified model used for all-root search

The netlist above is a SPICE3f5 model of a latch built from load resistors and NMOS transistors. Its device values are illustrative and were not fitted to the cubic curve. MAL-Seeker actually solved the simplified model implemented by SPICE B current sources, with each inverter represented by the following cubic transfer law.

$$f(v)=0.5-1.4(v-0.5)+2.0(v-0.5)^3$$ $$v_1=f(v_2),\qquad v_2=f(v_1)$$

In the simplified SPICE3f5 model, normalized $R=1$ resistors from the two nodes to ground provide the $v_1$ and $v_2$ terms, while B current sources provide the $-f(v)$ terms controlled by the opposite node. The resulting DC KCL conditions expand to:

$$v_1-0.1v_2+3v_2^2-2v_2^3-0.95=0$$ $$v_2-0.1v_1+3v_1^2-2v_1^3-0.95=0$$

Each equation is cubic, so the total-degree bound for this isolated-root search is $3\times3=9$. I examined the system in three stages: the physical voltage range, an extended real range, and the full complex domain.

3. Three operating points in the physical range

Operating Point	v1	v2	Interpretation
A	0.9472135955	0.0527864045	High / Low state
B	0.5000000000	0.5000000000	Central symmetric point
C	0.0527864045	0.9472135955	Low / High state

The two asymmetric points correspond to complementary latch states, while the third is a central symmetric operating point. These are static equilibrium equations; a rigorous statement about dynamic stability would require an additional model containing capacitance or explicit time evolution.

4. From five real roots to all nine complex roots

Run	Search Domain	Expected Roots	Solutions Found	Run Time (sec)
Physical search	Real, 0 ≤ v1, v2 ≤ 1	3	3	0.002338
All-real search	Extended real range	5	5	0.006594
Total-degree homotopy	Complex domain	9	9	0.000677

Extending the real range adds $(-0.5954451150,-0.5954451150)$ and $(1.5954451150,1.5954451150)$, giving five real roots. Total-degree homotopy then tracked all nine paths successfully and captured the four remaining complex roots.

5. Analysis environment

Analysis EngineMAL-Seeker (Project Antares Ver 3.1.6)
Development ProjectProject Bellatrix V1.0.4
ComputerMacBook Pro (Mac17,2)
OSmacOS Tahoe 26.4 (Build 25E246)
CPUApple M5, 10-core (4P + 6E), arm64
Memory32 GB

Dr.WataWata Insight:

Even in a two-variable circuit, the operating points we intend to use, the roots that exist over the reals, and the complete algebraic solution set are different things. Expanding the map step by step—from three physical points, to five real roots, and finally nine complex roots—made the relationship between circuit design and all-solution search especially clear.

1. A minimal model that remembers 0 or 1

2. Simplified model used for all-root search

3. Three operating points in the physical range

4. From five real roots to all nine complex roots

5. Analysis environment

Related books

Electronic Circuit Simulation

Circuit Simulation and Modeling with Python

電子回路シミュレータLTspice入門編