Skip to content
SiLab-BonnPublic

About

🦥 Tools for characterization of GDS and PCB layouts

Resources

Stars

1 star

Watchers

0 watching

Forks

Latest commit

 

History

11 Commits

Folders and files

Repository files navigation

layz

Layout tools for SiLab's FR4 PCBs, in-house RDL chips (maskless lithography) and the flex PCBs that connect them, as one command line tool:

layz drc       design rule check of a GDS (gdscheck, with the kit's deck)
layz pcb       GDS -> KiCad .kicad_pcb (copper zones, footprints, vias, outline, stackup)
layz nets      assign zone/via nets from a seed footprint's pad nets
layz hyp       .kicad_pcb or GDS -> HyperLynx .hyp (for SI/PI)
layz svg       GDS -> SVG preview
layz pex       3-D capacitance matrix with FasterCap/FastCap2 (.kicad_pcb, or GDS + stack)
layz field     electric field and potential from a `layz pex --charges` run
layz view      open a result: DRC report in KLayout, or ParaView renders of a field run
layz doctor    which external tools this machine has

layz <command> -h shows each command's options.

Install

layz is a standard Python package (pyproject.toml, Python 3.12 to 3.15), installed with Python's own venv and pip. It also uses tools that are not on PyPI:

Tool Needed for Linux macOS
KiCad (its pcbnew Python module, kicad-cli) pcb, hyp, pex on boards, schematic netlists kicad.org/download/linux kicad.org/download/macos
KLayout viewing GDS and DRC results klayout.de/build.html klayout.de/build.html
FasterCap (default) / FastCap2 pex, field scripts/build_solvers.sh (sources: FasterCap, FastCap2) FasterCap releases (or scripts/build_solvers.sh)
gdscheck drc github.com/aesc-silicon/gdscheck, with Rust's cargo (rust-lang.org/tools/install) same
ParaView (optional) view of field results paraview.org/download paraview.org/download

gdscheck installs with cargo install --git https://github.com/aesc-silicon/gdscheck gdscheck.

KLayout's Python module, KLayout-PEX, Shapely and the rest come from PyPI. From the repo root:

./install.sh                # once; again after a pull that changes dependencies
layz doctor                 # checks klayout, kicad-cli, FasterCap and gdscheck, and more

install.sh (bash; works from zsh too, on Linux and macOS) makes .venv/ with the Python that KiCad's pcbnew module is built for (Linux: python3, 3.14 on Ubuntu 26.04; macOS: KiCad's own), checks it's Python 3.12 to 3.15, installs layz into it with pip install --editable . (changes in this repo take effect directly), links layz into ~/.local/bin, and adds that folder to PATH in ~/.bashrc or ~/.zshrc if it isn't there yet. ./install.sh --test also installs pytest, ./install.sh --uninstall removes the link. Keep the clone: the DRC decks (drc/) and stacks (stacks/) are read from it.

By hand, the same is:

python3 -m venv --system-site-packages .venv      # system packages: pcbnew comes with KiCad
.venv/bin/pip install --editable .
ln -sf "$PWD/.venv/bin/layz" ~/.local/bin/layz

layz finds KiCad's pcbnew by itself, also from a venv without the system's packages; set LAYZ_KICAD_PYTHONPATH to the folder holding pcbnew.py if it's somewhere unusual. layz doctor exits with an error when a required tool is missing, and warns about optional ones (HyperLynx via LAYZ_HYPERLYNX, FastCap2, ParaView).

On Ubuntu also sudo apt install cmake g++ libomp-dev libopenblas-dev, then scripts/build_solvers.sh: it builds FasterCap (iic-jku fork, headless), FastCap2 and a wxWidgets base library into ~/.local/share/layz and links the solvers into ~/.local/bin. layz finds them on PATH, or through LAYZ_FASTERCAP / LAYZ_FASTCAP2. On macOS see the notes at the top of the script.

Tests run in the same venv:

./install.sh --test
.venv/bin/python -m pytest

Stack files

A GDS carries only 2-D shapes; heights, thicknesses and permittivities come from a stack file, one per process, in stacks/. It lists the layers top to bottom; z positions are derived from the order. Every tool reads the same file:

name = "SiLab RDL, 4 copper"
outline = "70/0"              # GDS layer of the board/die outline

[[layer]]
name = "F.Mask"
type = "mask"                 # mask | copper | dielectric
thickness_um = 1.0
er = 3.3

[[layer]]
name = "F.Cu"                 # KiCad names: F.Cu, In1.Cu, ..., B.Cu
type = "copper"
thickness_um = 0.5
gds = "8/0"
pads = true                   # GDS sub-cells with these shapes become footprint pads
zones = false                 # top-level shapes become copper zones (default true)

[[layer]]
name = "DE_F.Cu"
type = "dielectric"
thickness_um = 4.0
er = 4.5
material = "FR4"
# ... more layers ...

[[via]]
gds = "7/0"
top = "F.Cu"
bottom = "In1.Cu"

layz pcb --stack writes the stack into the board as its KiCad physical stackup, so the .kicad_pcb, the .hyp and the FasterCap model all carry it. A board made in KiCad uses its own stackup (Board Setup > Physical Stackup). The full format is documented in src/layz/stack.py.

Stack file Process Source
uni_bonn_rdl.toml Uni Bonn RDL, Al on polyimide (obelix1: M2 + M3 on the chip pads) asiclab tech/uni-bonn-rdl thicknesses, obelix1 KiCad mapping; polyimide εr and 8/0 to confirm
multicb_4L-01.toml Multi-CB 4-layer FR4, 1.6 mm Multi-CB defined buildup 4L-01 (mask assumed: 10 µm, εr 3.3)
multicb_4L-02.toml Multi-CB 4-layer FR4, 1.0 mm Multi-CB defined buildup 4L-02 (mask assumed)
multicb_flex_2F-l.toml Multi-CB 2-layer flex, adhesiveless, 161 µm Multi-CB standard 2F-l
multicb_flex_2F-a.toml Multi-CB 2-layer flex, adhesive-bonded, 187 µm Multi-CB standard 2F-a

The Multi-CB files are their published standard buildups; for a board ordered with a custom buildup, copy the closest one and enter the ordered thicknesses and materials.

GDS -> KiCad -> HyperLynx

layz hyp example_files/obelix1_ivtx_ladder_v2.gds --stack stacks/uni_bonn_rdl.toml   # one step

or step by step, to edit the board in between:

layz pcb --lay design.gds --stack stacks/uni_bonn_rdl.toml          # -> design.kicad_pcb
# KiCad: Update PCB from Schematic (references and the seed footprint's pad nets)
layz nets design.kicad_pcb --seed-footprint VTX2       # -> design_nets_assigned.kicad_pcb
layz hyp design_nets_assigned.kicad_pcb               # -> design_nets_assigned.hyp

layz pcb: GDS cells with pad-layer shapes become footprints (one per cell and orientation), top-level copper becomes filled zones, via layers become blind/buried vias, the outline layer becomes Edge.Cuts; Y is flipped so the board shows the GDS top view. nets: nets propagate from the seed footprint's pads through touching copper and vias. hyp: a re-implementation of KiCad's HyperLynx exporter (KiCad has it only in the GUI), same records and number format: board outline, stackup, devices, padstacks, and per net its pins, vias, tracks and zone fills.

Design rule check

layz drc --lay design.gds --kit uni-bonn-rdl                  # -> design.lyrdb
layz view design.lyrdb --lay design.gds                     # KLayout with the violation markers

Decks are gdscheck PDKs in its own YAML format, one per kit in drc/<kit>/. drc/uni-bonn-rdl/ is the in-house RDL (maskless lithography), with the layers of asiclab's tech/uni-bonn-rdl: chip pads 68/0, Al M1 1/0, M2 3/0, M3 6/0, polyimide openings V1 2/0, V2 4/0, pad openings 7/0, outline 70/0.

Rule Value
M1, M2, M3 width, spacing, notch ≥ 10 µm
M1, M2, M3 area (minimum feature 10 × 10 µm) ≥ 100 µm²
V1, V2, pad opening size / spacing (spacing assumed = metal spacing) ≥ 10 µm
V1 by M2, V2 by M2 and M3, pad openings by M3, every side ≥ 10 µm (pads ≥ 30 × 30 µm)
V1 landing on M1 or a chip pad contained
metal density in any 1 × 1 mm window (step 500 µm), inside the outline 70/0 ≤ 95 %

Chip pads (68/0) are the chip's and aren't checked. V2 is the 4/0 opening alone (asiclab's tech has 4/0 AND 5/0; designs draw V2 on 4/0). --suite geometry leaves out density. --benchmark times each rule on its own (slowest first): on the obelix1 ladder the M2 and M3 width checks are 98 % of the run. --tile is gdscheck's merge tile; layz uses 20 mm, about 5x faster than 2 mm on the ladder's long planes. The obelix1 ladder GDS takes about 35 s (18 threads) and reports 261 violations: V2 enclosure by M2 (52) and M3 (138), density in 19 + 20 windows on M2/M3, 19 notches, 1 width, and 12 at V1 and pad openings.

Capacitance and fields

layz pex board.kicad_pcb                              # stack from the board
layz pex chip.gds --stack stacks/uni_bonn_rdl.toml       # stack from the file
layz pex board.kicad_pcb --charges --out run          # also keep charges for fields
layz field run --voltage TOP=1                        # 3-D grid -> run/field.vtk
layz field run --voltage TOP=1 --plane y=5000         # cross-section, PNG + VTK
layz view section run/section_y5000_edge.vtk          # ParaView: heatmap + field lines
layz view geometry run                                # ParaView: the 3-D model

A conductor is any copper that touches or is joined by vias (no LVS, no netlist), named by net (KiCad), by GDS texts or --name NAME=LAYER@X,Y. The 3-D model (extrusion, dielectric interfaces, triangulation into FasterCap's .lst/.geo) comes from KLayout-PEX's FasterCapModelBuilder. Results: maxwell_matrix_fF.csv (Maxwell sign convention: diagonal total, off-diagonal −mutual) and spice_caps_fF.csv.

Keep --tolerance at 1 % or tighter (the default). With dielectrics FasterCap's first passes can be far off: plates with εr = 4 gave 2336 fF at 5 % and 3591 fF at 1 %, without an error. layz warns when FasterCap stops after a single pass.

--voltage sets conductor voltages when computing fields; any bias is a superposition of the solved columns, so it needs no new solve. On Ubuntu ParaView needs HWLOC_COMPONENTS=-gl (layz view sets it).

Checks

.venv/bin/python -m pytest (about 3 s):

  • GDS -> .hyp of the obelix1 RDL design gives the same STACKUP section as the .hyp KiCad's GUI exported (example_files/obelix1_ivtx_ladder_with_nets_v3.1.hyp).
  • tests/plates.gds, two 1 mm² plates 10 µm apart in vacuum: 918.8 fF (ideal 885 fF + fringe).
  • tests/pcb_plates.kicad_pcb (two 10 × 10 mm, 35 µm plates on 0.2 mm FR4, from tests/make_pcb_plates.py) builds the validated 3-D model. Solved at 1 %: 21.54 pF against ~21.7 pF from Palmer's edge-corrected formula, 5.16 kV/m in the FR4 at 1 V (ideal 5.0).
  • Stack files: heights, validation, KiCad stackup round trip.

Files

  • src/layz/ the package; stacks/ process stacks; example_files/ reference designs (GDS, KiCad schematic, a KiCad-exported .hyp); tests/; scripts/build_solvers.sh.

About

🦥 Tools for characterization of GDS and PCB layouts

Resources

Stars

1 star

Watchers

0 watching

Forks

Contributors

Languages