KiCad Schematic Filter Generator

This is a fairly simple filter generator that not only calculates cascades but can also output KiCad schematics. I created this because capturing and then populating components values in a schematic is rather tedious - and error prone.

The schematic files probably require KiCAD v5, but it's possible they will also load into v4.

It currently only knows of Multiple-Feedback (MFB) low-pass filters. These are sometimes referred to as Rauch filters in the literature.

It can generate a single-stage second order filter for an arbitrary gain, corner frequency, and Q.

It can generate cascaded stages for Bessel and Butterworth filters. (I will add Chebyshev at some point.)

It's run from the command line, and without any arguments produces a usage message.

$ python ./rauch.py
usage:
  rauch.py [sim] stage f0 H0 Q R1 [filename]
  rauch.py [sim] butterworth f0 H0 N R1 [filename]
  rauch.py [sim] bessel f0 H0 N R1 [filename]

     Generates either a single stage or an N-stage Rauch/MFB low-pass filter
     with a specific response.  Calculates component values for a cut-off
     frequency (-3dB) of f0 Hz, gain H0.
     R1 is used to scale resistors, with 1k being a good starting point.
     If supplied, a KiCad schmatic is output to 'filename'.

     Adding an initial 'sim' argument outputs a KiCAD schematic suitable
     for simulation with KiCad's built-in ngspice support.

SI suffixes: M k  m u n p

At the bottom are the SI suffixes it's aware of.

$ python ./rauch.py bessel 25k 10 3 1k ~/Desktop/filter.sch
Rauch LPF Stage (#1, Q=1.0233)
  R1: 1000ohm
  R2: 317ohm
  R3: 464ohm
  C1: 37.2nF
  C2: 2.82nF

Rauch LPF Stage (#2, Q=0.6111)
  R1: 1000ohm
  R2: 317ohm
  R3: 464ohm
  C1: 25.1nF
  C2: 5.32nF

Rauch LPF Stage (#3, Q=0.5103)
  R1: 1000ohm
  R2: 317ohm
  R3: 464ohm
  C1: 22.0nF
  C2: 6.72nF

Wrote schematic to /Users/bson/Desktop/filter.sch
$

The N parameter is the cascade length, NOT the filter order. Each stage is always second order, hence the filter order is always twice that of N supplied. It doesn't generate odd-order filters. It also doesn't know how to add passive stages as of now.

The filter generated can be added to KiCad via File -> Append Schematic Sheet...; the schematic has a token A4 page, with the filter below it. It's placed outside the page to make it easy to move it in whole or pieces onto the sheet as desired. The op amps will be LM358; this is just a placeholder and is intended to be edited to suit.

If you don't want the stage boxes (line notes) or text notes, just remove them. Feel free to cut it up and rearrange as needed, adding or renaming labels as desired.

Note that when a schematic is appended in KiCad all reference IDs are reset, and when annotated will be fit into the existing schematic. When stage component value are printed during generation the components re named according to this reference stage:

The command line argument R1 is the value of R1 in the circuit above. The resistors set the gain, so you can pick anything suitable for this. If in doubt, 1k is a fine value. If the other resistors start getting small, by all means step up to something bigger.

The code is mostly reasonably well factored, but some of it is overly naive. The offseting and relocation of subcircuits needs work. It works by building a tree representing the circuit and then outputting it as a .SCH file.

Simulation

Adding the keyword parameter "sim" makes the script output a .SCH file with KiCad v5 ngspice simulation fixings. The op amps will use an ideal model (1M gain, no poles or anything else, just flat response to infinity), an input source, and a .ac analysis directive. It also adds some other token components such as source and load resistors and rail voltage sources. The trivial opamp model doesn't use the rail voltages, but they're handy if you want to use a different model. For simulation LM321 pinout is used, which is a common single op amp. It also identifies the opamps as X? since this is what ngspice expects for a subckt model.

To use it:

1. Create an empty KiCad project and close it
2. Output a filter .sch file into the project
3. Open the project
4. Open the schematic
5. Run ngspice: Tools -> Simulator
6. Press the run button
7. Press the "Add Signals" button and add V(VOUT)

It's important to open the simulation schematic directly via the project and not try to append it. If you append it the reference IDs will be reset and any auto-generated simulation scripting (NYI) will no longer match the reference IDs.

This is a first stab at it, and higher orders than 4 (more than two stages) will push off the sheet.

The main purpose is to find reasonable E series component values. I'll add a Monte Carlo analysis out of the box at some point. This would be made easier if KiCad could pick up plot instructions from the schematic.

Notes

The grid positions are snapped to 100mil. This means if you use a metric grid size you may run into alignment problems. KiCad unfortunately can make these a pain to fix. I'll add a grid parameter at some point.

The rounding of numbers to N significant digits is buggy and currently counts the decimal point as a digit. I'll fix this also at some point.