matlab-read-pcb-layout

name	matlab-read-pcb-layout
description	Import Gerber, ODB++, Allegro .brd, .mcm files for PCB boards and IC packages. Inspect nets, layers, shapes, and stackups. TRIGGER: user asks to import, read, or open a PCB layout file. Gerber files use gerberRead or PCBReader; ODB++, Allegro .brd, .mcm, and native formats use pcbFileRead. Also when inspecting nets, layers, components, or stackups from an imported board. Invoke BEFORE writing import code — the query API (cadnet, cadnetList, componentList) is specialized. SKIP: EM analysis or S-parameter extraction (use matlab-analyze-em), PDN/IR-drop analysis (use matlab-analyze-pcb-pdn), building custom geometry (use matlab-assemble-pcb-layout), material/stackup definition only (use matlab-manage-pcb-material).
license	MathWorks BSD-3-Clause
metadata	{"author":"MathWorks","version":"1.0"}

Reading PCB and Package Layouts

Scope: pcbFileRead handles both PCB boards and IC/SiP packages. ODB++ and Allegro files may contain package-level designs (BGA substrates, interposers, embedded passives). The workflow is identical — the format determines what's inside, not the function name.

When to Use

• Importing Gerber files (.gtl, .gbl, .gbr, etc.) into MATLAB for visualization or EM analysis
• Reading ODB++ archives (zipped or unzipped) to inspect board or package layouts
• Importing Cadence Allegro .brd files
• Inspecting cadnets, components, layers, pins, or shapes from imported layouts
• Extracting metal layer polygons from Gerber files for use in custom designs
• Building a pcbComponent from externally designed layouts for S-parameter analysis

When NOT to Use

• Exporting designs to Gerber files — use matlab-write-pcb-layout
• Building PCB structures from scratch with shape primitives — use matlab-assemble-pcb-layout
• Running EM analysis after import — use matlab-analyze-em
• Defining substrates or stackup materials — use matlab-manage-pcb-material

Typical Workflow

1. This skill: Import the PCB layout from Gerber, ODB++, or Allegro
2. After: matlab-analyze-pcb-pdn — PDN DC analysis on imported board; or matlab-analyze-em — S-parameter extraction from imported geometry; or matlab-model-via — via analysis on imported stackup

Quick Reference

Task	Code
Import Gerber file	P = gerberRead('file.gtl')
Extract shapes	shp = shapes(P)
Define stackup	S = stackUp
Multi-layer import	p = PCBReader('StackUp', S)
Convert to pcbComponent	pcb = pcbComponent(p)
Import ODB++	pfile = pcbFileRead('design.zip')
Import Allegro .brd	pfile = pcbFileRead('design.brd')
List cadnets	tbl = cadnetList(pfile)
Open a cadnet	cnet = cadnet(pfile, "NET_NAME")
Query layer stackup	su = stackUp(pfile)
List components	tbl = componentList(pfile)
List padstacks	tbl = padStackList(pfile)

gerberRead — Simple Import

The gerberRead function imports Gerber files and returns a PCBReader object. Use shapes() to extract the metal layers as polygon shapes.

Basic Usage

P = gerberRead('interdigital_Capacitor.gtl');
shp = shapes(P);      % Extract metal layer shapes
show(shp(1));          % Show top layer polygon

Centering Imported Geometry

Imported shapes often have non-zero offsets from CAD origin. Extract shapes, then center:

P = gerberRead('myDesign.gtl');
shp = shapes(P);
layer1 = shp(1);

% Get bounding box to compute center offset
verts = layer1.Vertices;
cx = (max(verts(:,1)) + min(verts(:,1))) / 2;
cy = (max(verts(:,2)) + min(verts(:,2))) / 2;

% Center using translate
layer1 = translate(layer1, [-cx -cy 0]);
show(layer1);

Supported Gerber File Extensions

Extension	Layer Type
.gtl	Top copper
.gbl	Bottom copper
.gts	Top solder mask
.gbs	Bottom solder mask
.gto	Top silkscreen
.gbo	Bottom silkscreen
.drl	Drill file
.gbr	Generic Gerber

stackUp — Multi-Layer Definition

The stackUp object defines the full PCB layer structure for importing multi-layer boards.

Default stackUp

S = stackUp;

A default stackup has numbered layers. Odd layers are conductors (metal or Gerber files), even layers are dielectrics.

Assigning Gerber Files to Layers

S = stackUp;
S.Layer1.Thickness = 0.1e-3;           % Air layer above board
S.Layer2 = 'interdigital_Capacitor.gtl'; % Top copper from Gerber

Multi-Layer Stackup

S = stackUp;
S.Layer1.Thickness = 0.1e-3;       % Air
S.Layer2 = 'top_copper.gtl';       % Top copper
S.Layer3.Thickness = 0.2e-3;       % Dielectric
S.Layer3.EpsilonR = 4.4;
S.Layer4 = 'inner_layer.g2';       % Inner copper
S.Layer5.Thickness = 1.0e-3;       % Core dielectric
S.Layer5.EpsilonR = 4.4;
S.Layer6 = 'bottom_copper.gbl';    % Bottom copper

PCBReader — Full Board Import

PCBReader wraps the stackup with Gerber files into a reader object that can be converted to pcbComponent.

Basic Workflow

S = stackUp;
S.Layer1.Thickness = 0.1e-3;
S.Layer2 = 'interdigital_Capacitor.gtl';

p = PCBReader('StackUp', S);
pcb = pcbComponent(p);
pcb.FeedDiameter = 0.001;
show(pcb);

Adding Feeds After Import

After converting to pcbComponent, add feed locations for EM analysis:

pcb = pcbComponent(p);
pcb.FeedDiameter = 1e-3;
pcb.FeedLocations = [-5e-3 0 1 3;    % Port 1
                      5e-3 0 1 3];    % Port 2
sp = sparameters(pcb, linspace(1e9, 10e9, 51), 'SweepOption', 'interp');
rfplot(sp);

Determining Feed Locations from Imported Geometry

Feed locations must fall on metal traces. After converting a Gerber import to pcbComponent, inspect the geometry to find valid feed points:

pcb = pcbComponent(p);
show(pcb);                      % Visual inspection — identify trace endpoints
layout(pcb);                    % Top-down layout view with dimensions

For programmatic placement, extract the imported layer's mesh vertices and compute edge midpoints:

m = mesh(pcb);                  % Get mesh structure for coordinate reference

When feed locations are uncertain, place feeds at the visual endpoints of the main transmission line trace, inset by at least FeedDiameter/2 from the trace edge.

FeedLocations Column Semantics

FeedLocations = [x, y, col3, col4] — Column 3 is the signal layer (where the feed probe/sphere appears). Column 4 is the ground reference layer. The probe connects from col3 to col4. If you swap them, the feed sphere renders on the wrong layer.

Edge Feeds (Strip Model)

For structures fed at the board edge (e.g., microstrip lines terminating at the PCB boundary), use the strip feed model:

pcb.FeedViaModel = 'strip';
pcb.FeedDiameter = traceWidth / 2;  % Must be half the trace width for edge feeds

The 'strip' model creates a planar feed at the board edge rather than a vertical via probe. Place feeds at the exact edge of the BoardShape where the trace terminates.

PCBReader Layer Structure

After pcbComponent(PCBReader), the Layers cell array follows the standard alternating pattern: {metal, dielectric, metal, ...}. The metal layers contain the imported Gerber shapes. Layer indices for FeedLocations follow the same odd-numbered convention (1, 3, 5, ...) as manually assembled pcbComponent objects.

Converting PCBReader to pcbComponent

The pcbComponent constructor accepts a PCBReader object directly.

Cadence Allegro .brd Import

When the user references a .brd file for import or analysis, always ask for their Cadence extracta.exe path before attempting the import. The extracta utility is required and must be configured first. Do not assume it is already set up.

% Step 1: Check if extracta is already configured
extractaSetup()                % Displays current path, or [] if not set

% Step 2: If [], ask user for path and configure (persists across sessions)
extractaSetup('C:/Cadence/SPB_17.4/tools/bin/extracta.exe')

% Step 3: Import
pcb = pcbFileRead('design.brd');

extractaSetup(path) accepts the full path to the Cadence extracta.exe executable. The path persists across MATLAB sessions — it only needs to be run once. Without this, .brd imports fail with an extracta error.

Calling extractaSetup() with no arguments displays the currently configured path (or [] if not yet set). Use this to check whether setup has already been done.

ODB++ Import

pcb = pcbFileRead('design.zip');       % Zipped ODB++
pcb = pcbFileRead('odb_directory');    % Unzipped ODB++

Board and Package Inspection

pcbFileRead opens ODB++, Allegro, or native PCB files for hierarchical inspection — layers, cadnets, components, parts, pins, and shapes. This works identically for PCB boards and IC/SiP packages.

Opening a File

pfile = pcbFileRead('ExampleBoard.odb');

The returned object exposes: NumLayers, NumCadnets, NumPadStacks, NumComponents, NumParts, LayerHeight.

Querying Layer Stackup

stackUp(pfile) returns a table of material details for every layer in the imported board:

su = stackUp(pfile);                   % Full stackup table
su = stackUp(pfile, [2 3 4]);         % Specific layers only

The table has columns: LayerNumber, LayerName, LayerType, Material, Thickness(inch), EpsilonR, LossTangent, Conductivity(S/m).

Note: This is an object function on pcbFileRead that returns a table — it is unrelated to the stackUp constructor used with Gerber import (see the Pitfalls section).

Navigating the Hierarchy

% List cadnets (electrical nets)
tbl = cadnetList(pfile);               % Returns table with net names

% Open a specific cadnet and get its shapes
cnet = cadnet(pfile, "VDD_CORE");
data = cadnetData(cnet);               % Struct with .Surfaces, .Pins, .Vias, .Traces
s = shapes(cnet);                      % Same struct as cadnetData (equivalent call)

% List and inspect components
tbl = componentList(pfile);
comp = component(pfile, "U1");
pins = componentPinData(comp);         % Returns pinsData array (see below)

% List and inspect parts (component types)
tbl = partList(pfile);
p = part(pfile, "IC6ANT");
cdata = componentData(p);             % Components that use this part type

% List padstacks
tbl = padStackList(pfile);

% Layer-level inspection (metal layers only — use pfile.MetalLayer for valid indices)
lyr = layer(pfile, pfile.MetalLayer(1));
ldata = layerData(lyr);

% Search for components in a cadnet
results = findComponents(cnet);
results = findComponents(cnet, 'ComponentType', 'IC');

Shape Data Structure

shapes(cnet) and cadnetData(cnet) are equivalent — both return a struct with fields:

Field	Type	Content
.Surfaces	antenna.Polygon array	Copper pours and fills
.Pins	antenna.Polygon array	Pad shapes
.Vias	antenna.Polygon array	Via barrel shapes
.Traces	antenna.Polygon array	Routed trace segments

s = shapes(cnet);
s.Traces(1).Vertices   % Vertices of first trace segment
numel(s.Surfaces)      % Number of copper pours

layerData(lyr) returns the same struct format. Each antenna.Polygon has a .Vertices property (Nx3 double).

componentPinData — Pin Positions and Properties

componentPinData(comp) returns a pinsData array. Each element has:

Property	Type	Description
Center	1x2 double	XY position of pin center (board units)
PinNumber	char/string	Pin number/name
CadnetName	char/string	Net the pin connects to
PinShape	char	Shape type (e.g., 'Rect', 'Circle')
StartLayer	double	First layer the pin spans
StopLayer	double	Last layer the pin spans
Length	double	Pad length
Width	double	Pad width
Diameter	double	Pad diameter (for circular pads)
Vertices	Nx3 double	Full pad outline vertices

comp = component(pfile, "U1");
pins = componentPinData(comp);
pins(1).Center       % [x, y] in board units (inches for ODB++)
pins(1).CadnetName   % Which net this pin connects to
pins(1).PinNumber    % Pin identifier

Coordinate units: For ODB++ imports, pin positions (.Center) and shape vertices are in the board's native units — typically inches. Convert to meters for use in pcbComponent: multiply by 25.4e-3.

Tracing a Circuit Path Across Nets

Use findComponents + componentPinData to hop across nets via shared components:

pwr_net = cadnet(pfile, "+PWR");
pwr_comps = findComponents(pwr_net);   % Table: ComponentIndex, Refdes, PinList, ComponentType, Part

% Open a component and discover its other nets
q4 = component(pfile, string(pwr_comps.Refdes(9)));
q4_pins = componentPinData(q4);
for i = 1:numel(q4_pins)
    fprintf('%s.%s -> %s at [%.3f, %.3f]\n', "Q4", ...
        string(q4_pins(i).PinNumber), string(q4_pins(i).CadnetName), ...
        q4_pins(i).Center(1), q4_pins(i).Center(2));
end

% Follow Q4's output net to find the next component
next_net = cadnet(pfile, string(q4_pins(1).CadnetName));
next_comps = findComponents(next_net);

Using Imported Shapes in Custom Designs

Import Gerber geometry and combine with other shapes using Boolean operations:

% Import a CSRR pattern from Gerber
reader = gerberRead('csrr_pattern.gbr');
shp = shapes(reader);
csrr = shp(1);
verts = csrr.Vertices;
cx = (max(verts(:,1)) + min(verts(:,1))) / 2;
cy = (max(verts(:,2)) + min(verts(:,2))) / 2;
csrr = translate(csrr, [-cx -cy 0]);

% Use as DGS or combine with other geometry
ground = traceRectangular(Length=30e-3, Width=20e-3);
groundWithSlots = ground - csrr;

pcb = pcbComponent;
signal = traceRectangular(Length=25e-3, Width=3e-3);
sub = dielectric("FR4");
sub.Thickness = 1.6e-3;
pcb.Layers = {signal, sub, groundWithSlots};
pcb.BoardShape = ground;
pcb.BoardThickness = sub.Thickness;
show(pcb);

Import-to-Analysis Workflow

%% Import
S = stackUp;
S.Layer1.Thickness = 0.1e-3;
S.Layer2 = 'myFilter.gtl';

p = PCBReader('StackUp', S);
pcb = pcbComponent(p);

%% Configure for analysis
pcb.FeedDiameter = 0.5e-3;
pcb.FeedLocations = [-10e-3 0 1 3; 10e-3 0 1 3];
pcb.Conductor = metal("Copper");
show(pcb);

%% Analyze
freq = linspace(1e9, 10e9, 51);
sp = sparameters(pcb, freq, 'SweepOption', 'interp');
rfplot(sp);

Common Error Diagnostics

Error	Cause	Fix
"File not found"	Wrong path or unsupported format	Verify path; use fullfile() for cross-platform paths
"Unrecognized file format"	File extension doesn't match content	Pass format explicitly: pcbFileRead(file, 'FileType', 'ODB++')
Stack-up mismatch after import	Layer count/materials differ from design	For pcbFileRead imports: call stackUp(pfile) to inspect the imported layer table. For Gerber imports: verify your stackUp constructor matches the source design
extracta error on .brd import	Cadence Allegro extracta not configured	Run extractaSetup() first, then retry
Empty cadnetList results	Board has no routed nets or wrong format version	Open board in native EDA tool to verify routing exists

Pitfalls

1. Coordinate alignment: Gerber files from different CAD tools may use different origins. Always check and translate to center before combining layers or adding feeds.

2. Units mismatch: Gerber files can be in mils or mm. RF PCB Toolbox uses meters internally. If imported geometry looks too large or too small, check the source file's unit setting.

3. gerberRead returns PCBReader, not shapes: gerberRead returns a PCBReader object. Call shapes(P) to extract the metal layer polygons. Don't try to use P.Vertices or show(P) directly on the reader.

4. Layer ordering in stackUp constructor: Layer numbering in the stackUp constructor starts from the top. Layer1 is typically air above the board, Layer2 is the top copper. Odd-numbered physical metal layers map to even stackUp layers (since Layer1 is air).

5. layer() only accepts metal layer indices. layer(pfile, idx) requires idx to be a metal layer number. Use pfile.MetalLayer to get valid indices. Passing a dielectric layer index (e.g., layer(pfile, 1) when layer 1 is dielectric) errors with "Value must be a member of this set: ..."

6. componentData is on part, not component. To get the list of components that use a part type, call componentData(p) where p = part(pfile, partName). The component object has componentPinData and shapes, but not componentData.

7. stackUp name collision. S = stackUp (no arguments) creates a constructor object for defining Gerber import layer structures. su = stackUp(pfile) is an object function on pcbFileRead that returns a table of material details. These are completely different types with different purposes. Do not confuse them.

8. Large imported geometries: Full-board Gerber imports can be very large. For EM analysis, extract only the region of interest rather than analyzing the entire board.

9. Always ask for extracta path before .brd import. When the user points to a .brd file, first run extractaSetup() (no args) to check if it's already configured. If it returns [], ask the user for the path to their Cadence extracta.exe and run extractaSetup(path). Typical path: C:/Cadence/SPB_<version>/tools/bin/extracta.exe. Without this, .brd imports fail.

10. Package vs board — same workflow. ODB++ and Allegro files may contain IC packages, not just PCBs. pcbFileRead handles both identically. The format determines the content, not the function name.

Related Skills

• matlab-write-pcb-layout — Export designs to Gerber manufacturing files
• matlab-assemble-pcb-layout — Building custom PCB structures from shapes
• matlab-analyze-em — Running EM analysis on imported boards
• matlab-manage-pcb-material — Substrate setup for imported stackups
• matlab-analyze-pcb-pdn — PDN analysis on imported boards

---

Copyright 2026 The MathWorks, Inc.