Ngspice is an open-source circuit simulator that supports the standard BSIM transistor models that were developed at UC Berkeley. There are many similar commercial simulators such as Synopsys HSPICE, OrCAD PSpice, LTSpice, etc. The differences are mainly simulation performance, some minor syntax differences (primarily in the analysis commands), and possibly some enhanced features. For full information on the syntax of spice see the Spice Syntax tutorial.
Ngspice is available for all major operating systems. You can download and install it from
the Ngspice web site.
You must use Ngspice in WSL for Windows.
You should be using at least version 37 of ngspice. You can check the version by typing:
ngspice --versionAnother (preferred) method is to use Nix. In this method, Nix will provide the binaries, but you first need to install Nix depending on your OS: https://openlane2.readthedocs.io/en/latest/getting_started/common/nix_installation/index.html If you are using Nix (such as for the OpenLane flow), you can install it with:
nix shell github:efabless/nix-eda#ngspiceYou should install the PDK using volare which you can install with Python pip. For example,
pip install volare
volare enable --pdk sky130 0fe599b2afb6708d281543108caf8310912f54afYou should now see the PDK installed:
$ ls ~/.volare
sky130A sky130B volareOnce you create an ngspice file like example.sp, you can run it on the command line by typing:
ngspice example.sp We provide an example spice file that should work right now and you can test it. Spice files usually end with the extension .sp (for spice) such as the example provided but you may also see .spc, .spice or others. After the program runs, you will see output like this with a prompt:
Circuit: * example inverter with transient analysis and measure
ngspice 1 ->
The first line of a spice file is always the circuit name. This is
often a source of confusion if someone thinks it is a command since it
will always be ignored. You will also see any possible errors or
warnings loading your spice file. You must fix these before you can
procede, but it is safe to ignore one about Note: can't find init file.
To actually simulate, you must type run at the prompt. When you want to exit ngspice, type quit at the prompt. There is no elegant way reload a spice file, so you must quit and restart the program each time. Please ask if you don't understand a warning or error message.
You can embed those commands directly into the spice file using a control card like this:
.control
run
quit
.endc
However, this is syntax specific to Ngspice.
Ngspice can perform at least three types of circuit analysis: direct current (DC), alternating current (AC) and transient simulation. (There are also noise and monte carlo analysis, but we will ignore those!) DC is basically a static circuit solver. AC performance frequency response analysis of circuits. Transient simulation performs time simulation of circuit responses and is the most flexible analysis for digital circuits.
The .DC statement is used in DC analysis to:
- Sweep any parameter value
- Sweep any source value
- Sweep temperature range
- Perform a DC Monte Carlo analysis (random sweep)
- Perform a DC circuit optimization
- Perform a DC model characterization At each point of the sweep, the circuit is solved and values can be printed. The most common use is:
.dc <source> <start> <stop> <step>
source is the name of the independent voltage or current source, a model parameter, or an operating point such as the temperature (TEMP). The start, stop and step give the range and accuracy of the static points to simulate.
The following example causes the value of the voltage source VIN to be swept from 0.25 volts to 5.0 volts in increments of 0.25 volts and the circuit is solved for each value:
.DC VIN 0.25 5.0 0.25
The following example invokes a sweep of the drain-to-source voltage from 0 to 10 V in 0.5 V increments at VGS values of 0, 1, 2, 3, 4, and 5 V:
.DC VDS 0 10 0.5 VGS 0 5 1
This type of analysis will be very useful for characterizing devices! The following example asks for a DC analysis of the circuit from -55C to 125C in 10C increments:
.DC TEMP -55 125 10
We won't use AC analysis in this class, but it is useful if you have analog or radio frequency circuits. This lets you apply an alternating current (or voltage) signal to an input over a range of frequencies to determine frequency response (i.e., Bode) plots.
.ac <lin|dec|oct|> <number of samples> <freq start> <freq stop>
Ngspice transient analysis computes the circuit solution as a function of time over a time range specified in the .TRAN statement. Since transient analysis is dependent on time, it uses different analysis algorithms, control options with different convergence-related issues and different initialization parameters than DC analysis. However, a transient analysis first performs a DC operating point analysis to know the starting point of the circuit at time 0.
The TRAN statement looks like:
.tran <stepsize> <endtime>
The following statement will perform 1ns of simulation with time steps of roughly 1ps
.tran 1ps 1ns
Performing too long of a simulation or too fine of a step may take a long time!
The .PRINT statement specifies output variables for which values are printed. The maximum number of variables in a single .PRINT statement is 32. You can use additional .PRINT statements for more output variables.
To simplify parsing of the output listings, a single "x" printed in the first column indicates the beginning of the .PRINT output data, and a single "y" in the first column indicates the end of the .PRINT output data.
Syntax
.PRINT antype ov1 <ov2 ... ov32>
where antype specifies the type of analysis for output (DC, AC, TRAN, etc.). ov1... specify the values to be printed.
Example
.PRINT TRAN v(vs) v(vo)
This example prints out the results of a transient analysis for the nodal voltage named vs and vo. The output looks like this:
x
time voltage voltage
vs vo
0. 0. 0.
10.00000u 0. 0.
20.00000u 0. 0.
30.00000u 0. 0.
...
y
This example
.PRINT DC V(2) I(VSRC) V(23,17) I1(R1) I1(M1)
specifies that the DC analysis results are to be printed for several different nodal voltages and currents through the resistor named R1, the voltage source named VSRC, and the drain-to-source current of the MOSFET named M1. The output of this plot will be similar to the transient one except the first column will be the DC voltage that is swept in the analysis instead of time.
There are generally two plot commands in spice tools: the standard text plot and a graphical one. The syntax for the text .PLOT command is identical to the .PRINT command. However, plotting the results will display a text graph of the output values. This is sometimes useful in a pinch.
More realistically, you can graphically plot results using the {\bf plot} command at the ngspice prompt. Since you can have multiple analyses in one spice session, this will use the transient one, by default, I believe. You can list the other analyses by typing:
setplot
which will show something like this:
Type the name of the desired plot:
new New plot
Current tran1 * example inverter with transient analysis and measure (Transient Analysis)
dc1 * example inverter with transient analysis and measure (DC transfer characteristic)
const Constant values (constants)
You can either type the name or press enter to quit. To view other results, you must switch to the other analysis using the {\bf setplot} command like this:
setplot tran1
Then, you can plot transient results like this, for example,
plot A Z
which plots the waveforms of the input and output. If I want to plot the DC voltage transfer curve, I would issue the following commands:
setplot dc1
plot Z
The .measure command is used to measure almost any parameter in your circuit under some specified conditions. For example, it can be used to measure rise time, fall time, delay, maxima and minima, etc.
One use of the .measure command involves specifying a trigger and a target (TRIG and TARG, respectively). A trigger tells the command when to start measuring, and the target tells the command when to stop measuring. The command will then report the value you want to measure at the trigger condition, target condition, and the difference between its values under those conditions. This is best illustrated through an example that is supplied with the homework.
Let’s say we want to measure the propagation delay and the output rise time of an inverter. First, we want to measure the delay from the input rising to 50% of the supply voltage to the output falling to 50% of the supply voltage. Next, we define the output rise time metric as the time it takes for the output to go from 10% to 90% of its final value (i.e. from 0.12V to 1.08V for a 1.2V supply).
The structure of the command is as follows (note that the plus signs allow you to continue a command on the next line but isn't necessary):
.measure <ac|dc|tran> <name>
+ trig <node> val=<value> <rise|fall|cross>=<value>
+ targ <node> val=<value> <rise|fall|cross>=<value>
The first argument specifies what analysis statement to associate the measurement with. For example, if measuring time the first argument should be tran. If measuring frequency, it should be ac, and if voltage, dc. The second argument is simply a name for your measurement. We must specify the trigger and target, which have identical structure. For each, you must specify what node you want to trigger/target on, the value it needs to equal at the time of the trigger/target, and how many rises/falls/crosses have occurred prior to the node reaching that value. You should understand the concept of rising and falling, i.e. a signal going from low to high or high to low. A cross is simply the sum of rises and falls.
Pay attention to the two .measure commands in the example spice file that compute this:
.meas tran rise_delay
+ trig v(vs) val=`0.5*supply_voltage` rise=1
+ targ v(vo) val=`0.5*supply_voltage` fall=1
.meas tran rise_time
+ trig v(vo) val=`0.1*supply_voltage` rise=1
+ targ v(vo) val=`0.9*supply_voltage` rise=1
In the example for computing delay and rise time, we use the names rise_delay and rise_time, respectively. Since it is an inverter, the rising input triggers a falling output. The rise_delay is triggered when v(vs), the input source, reaches half of the supply voltage (a parameter) during the first rising crossing. The time is then measured until the target which is when the v(vo), the output voltage, reaches half the supply voltage during the first falling. Similarly, the rise_time is triggered when the output voltage, v(vo) reaches 10% of the supply voltage and stops when it reaches 90% of the supply voltage. Both of these are the first rising time.
If you simulate this netlist in Ngspice and look at the output, the output will be:
rise_delay= 6.9297p targ= 31.9797p trig= 25.0500p
rise_time= 7.9874p targ= 134.4470p trig= 126.4596p
This gives you the trigger time, the target time, and the difference with the label you gave for each measure.
One issue to watch out for is that you cannot set your trigger at a zero value. If you want to trigger at zero, you can approximate the measurement by using a very small, but non-zero, trigger value. For example, I could trigger on the value 1n.
There is a list of other tutorials on the Ngspice web page: http://ngspice.sourceforge.net/tutorials.html The ngspice manual is also available at: http://ngspice.sourceforge.net/docs/ngspice-manual.pdf
Copyright 2024 VLSI-DA (see LICENSE for use)