Simulating a printed circuit project with spice-noqsi and ngspice

The project here is a simple broadband amplifier board. I've organized it in three directories:

• Schematic for the board schematics
• Symbols for custom symbols
• Simulation for test fixtures and models

Board Schematics

The top level has connectors and a subcircuit for the amplifier itself:

And here's the schematic of the amplifier subcircuit:

The Schematic directory has a suitable gafrc file, telling the tools where custom symbols and subcircuit source files are:

(source-library ".")
(component-library "../Symbols")

There's also a Makefile for building a netlist for Osmond PCB, a BOM, and for cleaning up:

 all : Board.osmond Board.bom.tsv
 
 Board.osmond : Board.sch BBamp.sch
 	lepton-netlist -g osmond Board.sch -o Board.osmond
 
 Board.bom.tsv : Board.sch BBamp.sch
 	`lepton-netlist -g bom Board.sch -o Board.bom.tsv`
 
 clean : 
 	rm -f Board.osmond Board.bom.tsv \#* *~

Simulation

For simulation, this project handles hierarchy in SPICE rather than lepton-netlist. Thus, in the Simulation directory, there is a gnetlistrc file containing the line (hierarchy-traversal "disabled"). The spice-noqsi back end does not require you to use this approach: your project may instead allow lepton-netlist to flatten hierarchy and pass the flattened netlist to SPICE. Either approach works.

Here's the simulation "test fixture":

To tell spice-noqsi to instantiate a subcircuit for the amplifier, the amplifier symbol contains a spice-prototype=X? %down BBamp attribute. The %down expands into a sorted list of pinlabel attributes. The subcircuit schematic matches this with a top level spice-prolog=.subckt BBamp %up attribute. The %up expands into a sorted list of the refdes attributes of INPUT, OUTPUT, and IO symbols. The result is the same connections as lepton-netlist makes when it expand hierarchy. You don't need to provide .ends: it is automatically appended to the output file.

The amplifier symbol also has a file=BBamp.cir attribute. This generates a .include BBamp.cir card in the output.

Most other components here use the default prototypes in spice-noqsi. Q1 is an exception: its model is a subcircuit, not an elementary device, so it has the attribute spice-prototype=X? #C #B #E fastnpn attached.

There is, of course, a Makefile for simulation:

GNET=lepton-netlist -L ../../.. -g spice-noqsi
SPICE=ngspice

%.cir : %.sch
$(GNET) $< -o $@

.PHONY : simulation

simulation : Test.cir BBamp.cir
	$(SPICE) Test.cir transistors.lib

BBamp.sch : ../Schematic/BBamp.sch
	cp $< $@

clean : 
	rm -f Test.cir BBamp.cir BBamp.sch \#* *~

This makes a copy of BBamp.sch in the Simulation directory. I like this approach because I often find myself tinkering with simulation schematics. Since I didn't use the "file=" mechanism to include the transistor models, I explicitly load the model library into SPICE here.

Typing make creates three plots: frequency response, transient response, and noise figure.

Roads not taken

As noted above, it's not necessary to assemble a hierarchical netlist in a Makefile. You can let lepton-netlist do the expansion. You can also do hierarchy in the style of older SPICE back ends, using spice-subcircuit-LL symbols and friends (but that gets in the way of printed circuit layout).

The Board.sch schematic could be the simulation test fixture if J1, J2, and J3 had suitable spice-prototype attributes to make them sources and loads. There is no need to make the amplifier itself a subcircuit, either.

The approach here is more attuned to larger projects, with multiple subcircuit instances and multiple test fixtures for smaller fragments. For big projects, the modular hierarchical approach has advantages, but this project could possibly benefit from a simpler approach.