# ECE 5745 Tutorial 10: SPICE Simulation

• Author: Christopher Batten
• Date: March 14, 2021

• Introduction
• Simulating an NMOS Discharging a Load Capacitance
• Simulating an NMOS Charging a Load Capacitance
• Simulating Simple Logic Gates
• Simulating Standard Cells
• To Do On Your Own

## Introduction

ngspice is an open-source SPICE simulator for electrical circuits. We can use it to try out some circuit simulations as we go through the semester. In this tutorial, we will start by exploring two simple circuits: an NMOS transistor discharging a load capacitance and an NMOS transistor charging a load capacitance. We can use ngspice to simulate these two scenarios and plot the voltages on various nets. We will then simulate simple logic gates constructed explicitly using transistors, before simulating a few gates from a standard cell library.

ngspice takes as input a SPICE deck. This is a text file which describes the circuit you want to simulate along with what kind of analysis you would like to perform on your circuit. You can learn more about SPICE decks in Chapter 8 of Weste & Harris. You can also look at the ngspice documentation:

• http://ngspice.sourceforge.net/docs/ngspice-34-manual.pdf

The first step is to source the setup script, clone this repository from GitHub, and define an environment variable to keep track of the top directory for the project.

``````% source setup-ece5745.sh
% mkdir \$HOME/ece5745
% cd \$HOME/ece5745
% git clone git@github.com:cornell-ece5745/ece5745-tut10-spice
% cd ece5745-tut10-spice
% TOPDIR=\$PWD
``````

## Simulating an NMOS Discharging a Load Capacitance

Here is a simple SPICE deck for the first scenario where we have an NMOS transistor discharging a load capacitance.

``````* MMOS Discharging Capacitor
* ========================================================================

* Parameters and Models
* ------------------------------------------------------------------------

.param VDD='1.1V'
.temp  25

* Supply Voltage Source
* ------------------------------------------------------------------------

Vdd vdd gnd VDD

* Transistors
* ------------------------------------------------------------------------

*  src  gate drain body type
M1 gnd  in   out   gnd  NMOS_VTL W=0.450um L=0.045um

* ------------------------------------------------------------------------

* Input Signals
* ------------------------------------------------------------------------

Vin in gnd pwl( 0ns 0V 0.5ns 0V 0.7ns VDD )

* Analysis
* ------------------------------------------------------------------------

.ic   V(out)=VDD
.tran 0.01ns 2.5ns

.control
run
set color0=white
set color1=black
set xbrushwidth=2
plot V(in) V(out)
.endc

.end
``````

The first line in the SPICE deck must be a comment. Comments start with an asterisk. Let’s discuss each part. The first part sets up parameters and models:

``````.param VDD='1.1V'
.temp  25
``````

We create a constant named VDD which is the supply voltage we want to use in our circuit. Note that VDD is -not- a voltage source or a node in our circuit. It is just a constant. We set the temperature we want to use for the simulation. Finally, we include the model files associated with the technology we want to use. We will be using the FreePDK 45nm technology in the labs/projects, so here we are including the transistor models from that technology.

The next part instantiates a supply voltage source:

`````` Vdd vdd gnd VDD
``````

SPICE decks have this weird thing where the very first character of a line indicates the type of circuit element you want to instantiate. The book gives many more examples. If the first character is a `V` then it is a voltage source. So here we are creating a voltage source between two nodes named `vdd` and `gnd`. Other examples include `R` for resistor, `C` for capacitor, `M` for MOSFET transistor, `A` for models with special code, and `X` for subcircuits. Note that SPICE decks are case sensitive. The voltage source is a constant 1.1V. We just use the constant `VDD` so we can set the supply voltage in one place at the top of the deck.

The next part instantiates a transistor:

``````*  src   gate drain body type
M1 gnd   in   out   gnd  NMOS_VTL W=0.450um L=0.045um
``````

The first letter is an `M` which means MOSFET. We specify nodes for the source, gate, drain, and body. We also indicate whether this is an NMOS or PMOS and the width and length in micron. This is a 45nm technology, so we use the minimum transistor length of 45nm (0.045um). If we look at our Nangate standard cell library for a INV_X1 we can see that the NMOS has a width of about 10x the length, so for we make the NMOS width to be 0.450um. So the above example creates a “minimum” sized NMOS transistor, where “minimum” means the NMOS we will be using in a minimum sized inverter.

The next part instantiates an output load:

``````Cload out gnd 7fF
``````

The first letter is a `C` which means capacitor. We specify the positive and negative terminals and the capacitance. An INV_X4 inverter has an input cap of 6.25fF so we round up to 7fF as a reasonable output load.

The next part instantiates another voltage source, but this source will be used for the input signal:

``````Vin in gnd pwl( 0ns 0V 0.5ns 0V 0.7ns 1.1V )
``````

Here we can use `pwl` to create a piece-wise-linear voltage signal.

The final part specifies what analysis we want to do:

``````.ic   V(out)=VDD
.tran 0.01ns 2.5ns

.control
run
set color0=white
set color1=black
set xbrushwidth=2
plot V(in) V(out)
.endc
``````

So the `.ic` line sets an initial condition. Here we want to make sure the output node is initially charged up. The `.tran` line specifies that we want to do transient analysis for 2.5ns in 0.01ns timesteps. The `.control`/`.endc` block is a set of interactive commands which run the simulation and then plot the results.

Now let’s run the simulation using ngspice:

``````% cd \$TOPDIR/sim
% ngspice nmos-discharge-cap-sim.sp
``````

A little plot should pop up that looks like the following. This plot clearly shows Vin going from 0V to 1.1V and Vout going from 1.1V to 0V. Everything is “full rail”. To Do On Your Own: Increase the load capacitance by 10x and then 100x and observe the impact on the time to discharge the capacitor.

## Simulating an NMOS Charging a Load Capacitance

Now let’s try a similar experiment except this time we are going to use the NMOS transistor to charge up an output load. Here is the corresponding spice deck:

``````* MMOS Charging Capacitor
* ========================================================================

* Parameters and Models
* ------------------------------------------------------------------------

.param VDD='1.1V'
.temp  25

* Supply Voltage Source
* ------------------------------------------------------------------------

Vdd vdd gnd VDD

* Transistors
* ------------------------------------------------------------------------

*  src  gate drain body type
M1 vdd  in   out   gnd  NMOS_VTL W=0.450um L=0.045um

* ------------------------------------------------------------------------

* Input Signals
* ------------------------------------------------------------------------

Vin in gnd pwl( 0ns 0V 0.5ns 0V 0.7ns VDD )

* Analysis
* ------------------------------------------------------------------------

.ic   V(out)=0V
.tran 0.01ns 2.5ns

.control
run
set color0=white
set color1=black
set xbrushwidth=2
plot V(in) V(out) V(in)-V(out) V(vdd)-V(out)
.endc

.end
``````

This is similar to what we had above except now the source of the NMOS transistor is connected to vdd, and we set the initial condition such that the output load is initially discharged. Now let’s run the simulation using ngspice:

``````% cd \$TOPDIR/sim
% ngspice nmos-charge-cap-sim.sp
``````

A little plot should pop up that looks like the following. This plot shows things are not working as well! Vin obviously goes from 0V to 1.1V, but Vout goes from 0V and then starts to level off around 0.8V. It never reaches 1.1V. Why? Well, we are also plotting Vgs (this is the organize line, it is V(in)-V(out)). You can see that Vgs goes up but then starts to go down because Vout is increasing! The transistor starts to turn off an this prevents us from fully charging up Vout. Notice that Vout is still slowly increasing … this is probably due to some second order effect like leakage or more likely that the NMOS is not 100% off since Vgs is right around the threshold voltage. To Do On Your Own: Increase the load capacitance by 10x and then 100x and observe the impact on the time to discharge the capacitor.

## Simulating Simple Logic Gates

Let’s experiment with some simple logic gates. Take a look at the SPICE deck in `inv-sim.sp` which contains the canonical minimum sized inverter:

``````*  src  gate drain body type
M1 vdd  in   out   vdd  PMOS_VTL W=0.900um L=0.045um
M2 gnd  in   out   gnd  NMOS_VTL W=0.450um L=0.045um
``````

Notice how the PMOS transistor is sized to be twice the size of the minimum-sized NMOS transistor. We can use a more complicated piece-wise linear voltage source to toggle the input to the inverter:

``````Vin in gnd pwl
+ (
+   0.0ns  0V
+   0.4ns  0V
+   0.6ns VDD
+   0.9ns VDD
+   1.1ns VDD
+   1.4ns VDD
+   1.6ns  0V
+   1.9ns  0V
+ )
``````

We can use `+` to continue a long line SPICE command across multiple lines in the SPICE deck. Here we have formatted the piece-wise linear voltage source to look a little like a table. The input is low for 0.5ns, then goes high for 1ns, and then goes low again for 0.5ns. Our SPICE deck also includes some measurement commands:

``````.measure tran tpdr trig v(in) val='VDD/2' fall=1 targ v(out) val='VDD/2' rise=1
.measure tran tpdf trig v(in) val='VDD/2' rise=1 targ v(out) val='VDD/2' fall=1
.measure tran tpd param='(tpdr+tpdf)/2'
``````

The ngspice manual explains measurement commands in more detail. Briefly, the first command measures the propagation delay for a low-to-high output transition, and the second command measures the propagation delay for a high-to-low output transition. These delays are measured from when the input is VDD/2 to when the output is VDD/2. The third measurement command uses the average of these two propagation delays to estimate the overall propagation delay of the inverter. Chapter 8 of Weste & Harris discusses in more detail how to effectively characterize various CMOS circuits. Now let’s run the simulation using ngspice:

``````% cd \$TOPDIR/sim
% ngspice inv-sim.sp
...
tpdr = 1.037703e-11 targ = 1.510377e-09 trig = 1.500000e-09
tpdf = 2.409571e-11 targ = 5.240957e-10 trig = 5.000000e-10
tpd  = 1.72364e-11
``````

A little plot should pop up that shows the input and output voltages, and the measurement results will be displayed in the terminal. The propagation delay is approximately 17.2ps.

To Do On Your Own: Increase the load capacitance by 10x and then 100x and observe the impact on the propagation delay. Make sure you look at the actual waveforms to see if the output has time to go full rail. If not, you need to increase the time between input transitions to make an accurate estimate of the propagation delay.

Let’s dig a little deeper. Notice that the rise time is not equal to the fall time for our inverter. The rise time is 10.4ps but the fall time is 24.1ps. We have made the PMOS twice the width of the NMOS (i.e., the PMOS is 900nm wide while the NMOS is 450nm wide), so why aren’t the rise and fall times equal? Part of the reason is the PMOS mobility is not exactly half the NMOS mobility in this technology as well as many other second order effects. Change the size of PMOS so it is only 1.5x as large as the NMOS like this:

``````*  src  gate drain body type
M1 vdd  in   out   vdd  PMOS_VTL W=0.675um L=0.045um
M2 gnd  in   out   gnd  NMOS_VTL W=0.450um L=0.045um
``````

Rerun the simulation:

``````% cd \$TOPDIR/sim
% ngspice inv-sim.sp
...
tpdr = 1.940778e-11 targ = 2.019408e-09 trig = 2.000000e-09
tpdf = 1.812324e-11 targ = 1.018123e-09 trig = 1.000000e-09
tpd  = 1.87655e-11
``````

You can now see the rise and fall times are much closer to being equal. Of course this begs the question, “Why is it important to have equal rise and fall times?”. To some degree this is a design decision. It is certainly possible to have unequal rise and fall times, and indeed this can also often lead to better area/power or enabling making a critical transition faster (at the expense of the other transition). However, the largest motivation for equal rise and fall times is that it maximizes the noise margins. To understand this, let’s use ngspice to analyze the DC transfer curve of an inverter. Take a look at the SPICE deck in `inv-sim-xfer.sp` which contains the same canonical minimum sized inverter but with DC instead of transient analysis:

``````.dc Vin 0 'VDD' 0.01
``````

Here is the resulting DC transfer curve showing Vin vs Vout (after I manually annotated the noise margins): Recall that the noise margins are with respect to where the slope of the transfer curve is -1 (i.e., maximum gain). V_IL is the maximum low input voltage and V_IH is the minimum high input voltage. V_OL is the maximum low output voltage and V_OH is the minimum high output voltage. The noise margins are NM_H = V_OH - V_IH and NM_L = V_IL - V_OL and we want these noise margins to be as large as possible. With large noise margins we can tolerate noise on the input without it propagating through the inverter and causing it to switch the output. For this example the noise margins are roughly equal at 0.3V:

``````V_IL = 0.45V
V_IH = 0.65V
V_OL = 0.15V
V_OH = 0.95V
NM_H = V_OH - V_IH = 0.95V - 0.65V = 0.31V
NM_L = V_IL - V_OL = 0.45V - 0.15V = 0.30V
``````

Now the problem with unequal rise and fall times is it means we essentially skew the noise margins. We make one noise larger but the other noise margin smaller. Try rerunning the simulation, but this time make the PMOS the same size as the NMOS like this:

``````*  src  gate drain body type
M1 vdd  in   out   vdd  PMOS_VTL W=0.450um L=0.045um
M2 gnd  in   out   gnd  NMOS_VTL W=0.450um L=0.045um
``````

Rerun the simulation and you should see something like the following (after I manually annotated the noise margins): And here are roughly the corresponding noise margins:

``````V_IL = 0.35V
V_IH = 0.48V
V_OL = 0.15V
V_OH = 0.98V
NM_H = V_OH - V_IH = 0.98V - 0.48V = 0.5V
NM_L = V_IL - V_OL = 0.35V - 0.15V = 0.2V
``````

Notice how the low noise margin has gone from 0.3V to 0.2V. This means the gate is now much more sensitive to noise. So in general we perfer equal rise and fall times becuase it improves our noise margins (and also simplifies our analysis).

To Do On Your Own: Make the NMOS twice as big as the PMOS and observe how this impacts the noise margins.

Creating voltage sources to change the inputs can be very tedious, especially when we want to drive multiple inputs. We can take advantage of ngspice’s support for mixed-signal analog/digital simulation to simplify the task of creating many digital input values. Take a look at the SPICE deck in `inv-dsource-sim.sp` to see a different way of generating input sources:

``````A1 [in_] inv_source
.model inv_source d_source (input_file="inv-source.txt")
``````

Here we are instantiating a `d_source` and giving this new component the name `a1`. The `d_source` reads an input text file to see the values of the given input nodes (i.e., `in_`). The `inv-source.txt` file looks like this:

``````* inv-source.txt
* ====================================================================

* time in
0.0ns  0s
1.0ns  1s
2.0ns  0s
``````

Lines that start with `*` are comments. The first column corresponds to time and each remaining column corresponds to an input node. The input node can be either `0s` (for a strong logic zero) or `1s` (for a strong logic one). So the above example toggles the input node just as with the previous piece-wise linear voltage source. Note that there is a positional mapping from the columns in the text file to the nodes in the SPICE deck when instantiating the `d_source`. So the second column maps to the `in_` input node.

We also need to instantiate a digital-to-analog converter (DAC) to translate the digital values into analog values suitable for driving a CMOS circuit:

``````Ain [in_] [in] dac_in
.model dac_in dac_bridge (out_low=0V out_high='VDD' t_rise=0.2ns t_fall=0.2ns)
``````

The `dac_bridge` component takes parameters specifying the logic low and logic high voltage levels and the rise/fall times. We also need to specify the mapping from digital input nodes (`in_`) to analog input nodes (`in`). Now let’s run the simulation using ngspice and confirm that the result is the same as when using piece-wise linear voltage sources:

``````% cd \$TOPDIR/sim
% ngspice inv-dsource-sim.sp
``````

Now let’s experiment with a NAND2 gate. Take a look at the SPICE deck in `nand2-sim.sp` which contains the canonical NAND2 gate:

``````*  src  gate drain body type
M1 vdd  a    y     vdd  PMOS_VTL W=0.900um L=0.045um
M2 vdd  b    y     vdd  PMOS_VTL W=0.900um L=0.045um
M3 n0   a    y     gnd  NMOS_VTL W=0.900um L=0.045um
M4 gnd  b    n0    gnd  NMOS_VTL W=0.900um L=0.045um
``````

Notice how we have sized this NAND2 gate to have equal worst-case rise and fall times assuming a PMOS/NMOS mobility ratio of two, and we have also sized this NAND2 gate to have similar effective resistance as the canonical minimum-sized inverter

To Do On Your Own: Copy the `nand2-sim.sp` SPICE deck to create a new file named `nor2-sim.sp` and copy the `nand2-source.txt` input file to create a new file named `nor2-source.txt`. Replace the NAND2 gate with an explicit transistor implementation of a NOR2 gate. Size the NOR2 gate to have equal worst-case rise and fall times assuming a PMOS/NMOS mobility ratio of two and similar effective resistance as the canonical minimum-sized inverter. Run the simulation and verify the functionality using the waveforms.

## Simulating Standard Cells

A standard cell library will include many views including SPICE decks for each standard cell. Actually, the standard cell library will usually include two kinds of SPICE decks. The schematic SPICE deck includes just the transistors, while the extracted SPICE deck will include all of the extracted parasitic resistances and capacitances. Take a look at the schematic SPICE deck for a minimum sized inverter (INV_X1):

``````% less -p INV_X1 \$ECE5745_STDCELLS/stdcells.spi
.SUBCKT INV_X1 A ZN VDD VSS
*.PININFO A:I ZN:O VDD:P VSS:G
*.EQN ZN=!A
M_i_0 ZN A VSS VSS NMOS_VTL W=0.415000U L=0.050000U
M_i_1 ZN A VDD VDD PMOS_VTL W=0.630000U L=0.050000U
.ENDS
``````

The SPICE deck for an inverter is encapsulated in a SPICE subcircuit (`SUBCKT`). A subcircuit is like a PyMTL3 or Verilog module with an interface (i.e., list of ports) and an implementation (i.e., instantiating transistors or other subcircuits). In this case, the INV_X1 gate includes four ports: the input (`A`), the output (`ZN`), the power supply (`VDD`) and ground (`VSS`). As expected, the implementation includes a PMOS and NMOS transistor. Notice that even though the minimum length transistor in this technology is 0.045um, both transistors are 0.050um. This is actually quite common. Standard cells often use slightly longer transistors to offer a better performance vs. power trade-off (i.e., lower leakage). Some standard cell libraries will actually include different implementations of every gate each with a different channel length. Also notice how the PMOS is only 1.5x larger than the NMOS. Again, this is actually quite common. A PMOS/NMOS mobility ratio of two is just an assumption; a specific technology will likely have a different mobility ratio which is often less than two. Standard cells will also often have slightly skewed rise/fall times to offer a better area vs. noise margin trade-off.

While we could certainly simulate the schematic SPICE deck, it is more useful to simulate the extracted SPICE deck since this will provide accurate performance analysis. Take a loo at the extracted SPICE deck for a minimum sized inverter (INV_X1):

``````% less -p INV_X1 \$ECE5745_STDCELLS/stdcells-lpe.spi
.SUBCKT INV_X1 VDD VSS A ZN
*.PININFO VDD:P VSS:G A:I ZN:O
*.EQN ZN=!A
M_M1 N_ZN_M0_d N_A_M0_g N_VDD_M0_s VDD PMOS_VTL W=0.630000U L=0.050000U
M_M0 N_ZN_M1_d N_A_M1_g N_VSS_M1_s VSS NMOS_VTL W=0.415000U L=0.050000U
C_x_PM_INV_X1%VDD_c0 x_PM_INV_X1%VDD_31 VSS 4.13109e-17
C_x_PM_INV_X1%VDD_c1 x_PM_INV_X1%VDD_19 VSS 2.61599e-16
C_x_PM_INV_X1%VDD_c2 x_PM_INV_X1%VDD_18 VSS 1.89932e-17
C_x_PM_INV_X1%VDD_c3 N_VDD_M0_s VSS 3.88255e-17
C_x_PM_INV_X1%VDD_c4 x_PM_INV_X1%VDD_12 VSS 1.92462e-17
C_x_PM_INV_X1%VDD_c5 x_PM_INV_X1%VDD_11 VSS 2.334e-16
C_x_PM_INV_X1%VDD_c6 x_PM_INV_X1%VDD_8 VSS 5.52247e-16
R_x_PM_INV_X1%VDD_r7 VDD x_PM_INV_X1%VDD_31 0.13879
R_x_PM_INV_X1%VDD_r8 VDD x_PM_INV_X1%VDD_28 0.392137
...
.ENDS
``````

The INV_X1 gate still includes four ports (although they are in a different order which is annoying), but notice that the implementation is radically different. There are ~50 parasitic resistances and capacitances extracted from the actual layout for this standard cell. These parasitics are what enable more accurate performance analysis.

Take a look at the SPICE deck in `inv-stdcell-sim.sp` which is meant for simulating the INV_X1 standard cell. First, notice that we need to include the standard cell SPICE deck:

``````.param VDD='1.1V'
.temp  25
``````

Instead of directly instantiating transistors, we simply instantiate the `INV_X1` subcircuit:

``````X1 vdd gnd in out INV_X1
``````

The instance name of subcircuits (`X1`) must start with `X`. The instance name is followed by the list of nodes that should be connected to the ports of the subcircuit. The nodes are connected by position. So since the port list in the subcircuit definition is `VDD VSS A ZN`, we must list the nodes in the subcircuit instance in the exact same order. The subcircuit instance ends with the type of subcircuit we wish to instantiate. The rest of the SPICE deck is the same as earlier in the tutorial. Let’s run the simulation using ngspice:

``````% cd \$TOPDIR/sim
% ngspice inv-stdcell-sim.sp
...
tpdr = 2.577757e-11 targ = 2.125778e-09 trig = 2.100000e-09
tpdf = 2.275623e-11 targ = 1.122756e-09 trig = 1.100000e-09
tpd  = 2.42669e-11
``````

Recall that the propagation delay when we instantiated transistors directly was 17.2ps while now it is 24.3ps. The extracted SPICE decks are almost always slower than schematic SPICE decks, since we are actually modeling the parasitic resistances and capacitances.

To Do On Your Own: Increase the load capacitance by 10x and then 100x and observe the impact on the propagation delay. Make sure you look at the actual waveforms to see if the output has time to go full rail. If not, you need to increase the time between input transitions to make an accurate estimate of the propagation delay.

Now let’s experiment with the NAND2_X1 gate from the standard cell library. Take a look at the SPICE deck in `nand2-stdcell-sim.sp` which instantiates the appropriate subcircuit, then run the simulation using ngspice:

``````% cd \$TOPDIR/sim
% ngspice nand2-stdcell-sim.sp
``````

To Do On Your Own: Copy the `nand2-stdcell-sim.sp` SPICE deck to create a new file named `nor2-stdcell-sim.sp` and copy the `nand2-source.txt` input file to create a new file named `nor2-source.txt`. Replace the NAND2_X1 subcircuit instance with an instance of the NOR2_X1 gate from the standard cell library. Run the simulation and verify the functionality using the waveforms.

## To Do On Your Own

The Nangate standard cell library includes a full-adder gate:

``````% less -p FA_X1 \$ECE5745_STDCELLS/stdcells-lpe.spi
.SUBCKT FA_X1 VDD VSS CO CI A B S
*.PININFO VDD:P VSS:G CO:O CI:I A:I B:I S:O
*.EQN CO=((A * B) + (CI * (A + B)));S=(CI ^ (A ^ B))
M_M14 N_VDD_M0_d N_4_M0_g N_CO_M0_s VDD PMOS_VTL W=0.630000U L=0.050000U
M_M15 net_007 N_B_M1_g N_VDD_M0_d VDD PMOS_VTL W=0.315000U L=0.050000U
M_M16 N_4_M2_d N_A_M2_g net_007 VDD PMOS_VTL W=0.315000U L=0.050000U
M_M17 N_6_M3_d N_CI_M3_g N_4_M2_d VDD PMOS_VTL W=0.315000U L=0.050000U
M_M18 N_VDD_M4_d N_A_M4_g N_6_M3_d VDD PMOS_VTL W=0.315000U L=0.050000U
M_M19 N_6_M5_d N_B_M5_g N_VDD_M4_d VDD PMOS_VTL W=0.315000U L=0.050000U
M_M20 N_11_M6_d N_B_M6_g N_VDD_M6_s VDD PMOS_VTL W=0.315000U L=0.050000U
M_M21 N_VDD_M7_d N_CI_M7_g N_11_M6_d VDD PMOS_VTL W=0.315000U L=0.050000U
M_M22 N_11_M8_d N_A_M8_g N_VDD_M7_d VDD PMOS_VTL W=0.315000U L=0.050000U
M_M23 N_12_M9_d N_4_M9_g N_11_M8_d VDD PMOS_VTL W=0.315000U L=0.050000U
M_M24 net_010 N_CI_M10_g N_12_M9_d VDD PMOS_VTL W=0.315000U L=0.050000U
M_M25 net_009 N_B_M11_g net_010 VDD PMOS_VTL W=0.315000U L=0.050000U
M_M26 N_VDD_M12_d N_A_M12_g net_009 VDD PMOS_VTL W=0.315000U L=0.050000U
M_M27 N_S_M13_d N_12_M13_g N_VDD_M12_d VDD PMOS_VTL W=0.630000U L=0.050000U
M_M0 N_VSS_M14_d N_4_M14_g N_CO_M14_s VSS NMOS_VTL W=0.415000U L=0.050000U
M_M1 net_000 N_B_M15_g N_VSS_M14_d VSS NMOS_VTL W=0.210000U L=0.050000U
M_M2 N_4_M16_d N_A_M16_g net_000 VSS NMOS_VTL W=0.210000U L=0.050000U
M_M3 N_7_M17_d N_CI_M17_g N_4_M16_d VSS NMOS_VTL W=0.210000U L=0.050000U
M_M4 N_VSS_M18_d N_A_M18_g N_7_M17_d VSS NMOS_VTL W=0.210000U L=0.050000U
M_M5 net_002 N_B_M19_g N_VSS_M18_d VSS NMOS_VTL W=0.210000U L=0.050000U
M_M6 net_006 N_B_M20_g N_VSS_M20_s VSS NMOS_VTL W=0.210000U L=0.050000U
M_M7 N_VSS_M21_d N_CI_M21_g net_006 VSS NMOS_VTL W=0.210000U L=0.050000U
M_M8 N_10_M22_d N_A_M22_g N_VSS_M21_d VSS NMOS_VTL W=0.210000U L=0.050000U
M_M9 N_12_M23_d N_4_M23_g N_10_M22_d VSS NMOS_VTL W=0.210000U L=0.050000U
M_M10 net_004 N_CI_M24_g N_12_M23_d VSS NMOS_VTL W=0.210000U L=0.050000U
M_M11 net_003 N_B_M25_g net_004 VSS NMOS_VTL W=0.210000U L=0.050000U
M_M12 N_VSS_M26_d N_A_M26_g net_003 VSS NMOS_VTL W=0.210000U L=0.050000U
M_M13 N_S_M27_d N_12_M27_g N_VSS_M26_d VSS NMOS_VTL W=0.415000U L=0.050000U
...
.ENDS
``````

Try instantiating and chaining four of these gates together to create a four-bit ripple-carry adder. Create an appropriate SPICE deck to drive the simulation including a `d_source` that reads in a text file with the two four-bit input values. Here is what the results look like if you start with adding 0b1111 to 0b0000 and then change the b input to 0b0001 at 200ps. Notice the sum outputs transitioning from 0 to 1 as the carry is propagated through the full-adder gates. As discussed in Chapter 8 of Weste & Harris, for more accurate performance analysis you would need to add inverters to the inputs for realistic waveform shaping and to the outputs for realistic load capacitance. 