# Using the substitution theorem to derive Thevenin resistance values with SPICE

#### Article By : K. Bharath Kumar In this Design Idea, we explore how the substitution theorem of network analysis can been applied to SPICE circuit simulation software to obtain the equivalent resistance/conductance.

Thevenin and Norton equivalent circuits [1-3] are a valuable analytical tool for circuit designers and researchers. How to obtain the Thevenin resistance and Norton conductance of a network with available network theorems?

In this Design Idea, the substitution theorem of network analysis has been used to obtain the equivalent resistance/conductance using the SPICE circuit simulation software [4-5]. The Thevenin equivalent representation of a network with an arbitrary load resistance of value (k·RT) with k >0, is shown in the Figure 1a. The Thevenin resistance RT is to be determined between terminals A,B. The load resistance k·RT can be, by the substitution theorem, replaced by an equivalent voltage source Ec·k/(k+1), where Eis the Thevenin open circuit voltage, which can be obtained by separately defining the network whose Thevenin resistance is of interest, as a sub-circuit in the SPICE netlist file description. The product of EC with k/(k+1) is realized by (in SPICE) a voltage dependent voltage source connected as shown in Figure 1b. Figure 1 The Thevenin equivalent representation of a network with an arbitrary load resistance of value (k · RT) with k >0, is shown (1a); the product of EC with k/(k+1) is realized by (in SPICE) a voltage dependent voltage source connected as shown in 1b.

The value of RT for the network (Figure 3) can be obtained [6-7] by dividing this voltage by the product of current Ik through the voltage dependent voltage source and k, with a value defined as: Ec/(Ik(k+1)). Figure 3 A Network whose Thevenin resistance across terminals A,B is to be determined.

The Thevenin resistance calculated for various values of k is given in Table I for Figure 3: The Norton equivalent circuit for a linear network with an arbitrary load conductance of value (GNOR/k) with k>0, is shown in the Figure 2a for the network, whose Norton conductance (GNOR) is to be determined between terminals C, D. The load conductance  GNOR/k in the Norton equivalent representation, by the substitution theorem, can be replaced (Figure 2b) by an equivalent current source ISC/(k+1) , where Isc is the Norton short circuit current, which can be obtained by a separate sub circuit SPICE description of the network under consideration. Figure 2 The Norton equivalent circuit for a linear network with an arbitrary load conductance of value ( GNOR/k) with k>0, is shown in 2a for the network; the load conductance GNOR/k in the Norton equivalent representation, by the substitution theorem, can be replaced (2b) by an equivalent current source.

The final Norton conductance value can be obtained by the expression: k·ISC/((k+1)·Vk)

The voltage Vk (the voltage across the current controlled current source) can be derived using the SPICE program. Figure 4 shows a network whose Norton conductance across terminals C, D is to be determined. Figure 4 A network whose Norton conductance across terminals C, D is to be determined.

The Norton conductance GNOR (in millimhos) for various values of k for Figure 4 is given in Table 2: Description of SPICE file to obtain Thevenin resistance (RT)

The sub-circuit THEV is used to describe the network (Figure 3) in Table 3: The Thevenin open circuit voltage is available at node 1 at the subcircuit X1. The voltage source ESUBS as required by the substitution theorem is connected at node 3 of sub-circuit X2. The current through the zero voltage source V23 gives the current  I through the voltage dependent voltage source ESUBS. The current Ik is converted to a DC voltage of the same value (Ik= v(4)) at node 4 using current controlled current source FSUBS and a 1-ohm resistor, RR40. The expression Ec/((k+1)·Ik), which is equivalent to the DC voltage at node 5 (v(5)), is obtained by equating the triple product current of polynomial source GSUBS, i.e., current Ik * voltage v(5) *  (k+1) with the current (=Ec) carried by the voltage controlled current source GSUBS1. Now, the Thevenin resistance (in ohms) can be obtained by reading the DC voltage at node 5,  v(5), after running the SPICE/PSPICE file.

Description of SPICE file to obtain Norton conductance (GNOR)

The network (Figure 4) whose Norton conductance (GNOR) is to be determined, is described under sub-circuit name NORT in Table 4: The short circuit Norton current ISC is obtained by the current through the zero voltage source V10 connected across nodes 1 and ground 0. This short circuit current is converted to a DC voltage (v(4)=ISC) by a current controlled current source FNORT using a 1-ohm resistor. The equivalent current source ISC/(k+1) is connected to node 2, as required by the substitution theorem. This is the same as connecting GNOR/k conductance across the Norton equivalent circuit. The Norton conductance GNOR given by  (k·ISC)/((k+1)·Vk) (where Vk= DC node voltage at V(2)), is obtained by equating the current of polynomial voltage dependent current source (triple product) Vk * (k+1)*V(5) to the current of voltage dependent current source GNOR1 connected across nodes 5 and ground node 0. Running the SPICE/PSPICE file yields the value of the DC node voltage V(5), which gives the numerical value of GNOR for Figure 4.

References

1. E. Van Valkenburg, Network Analysis, 3rd Edition, Chapter IX, pp. 259-261, Prentice-Hall 1976
2. P. Malvino, Electronic Principles,Chapter I, pp. 4-7, Tata-McGraw Hill 1998
3. Karpaty,”Simple Method uses PSpice for Thevenin-equivalent Circuits”, EDN, Design Ideas, pp. 47-48, April 23, 2009
4. Vladimirescu, K. Zhang, A. R. Newton, D. O. Pederson, A. Sangiovanni-Vincentelli, SPICE Version 2G User’s Guide, Dept. of Electrical Engineering and Computer Science, University of California, Berkeley, CA, USA
5. MicroSim PSpice & Basics, Circuit Analysis Software, User’s Guide, Version 8.0, June 1997
6. Epler, SPICE2 application notes for dependent sources, IEEE Circuits & Devices Magazine, pp. 36-44,3(5), 1984
7. Bharath kumar,”Inverse ABCD parameter determination using SPICE”, International Journal of Analog Integrated Circuits, IJAIC, Vol-3, issue 1, pp. 1-6, 2017 