This website requires JavaScript.
Coupons
Ship to
Blog

Can AI Really Design a PCB? Putting Claude Fable 5.2 to the Test

Published Nov 20, 2026, updated Nov 20, 2026

17 min

Table of Contents
  • Introduction
  • Can AI Design a PCB? Fable 5.2 Test Results at a Glance
  • How Fable 5.2 Designed the PCB in KiCad 10
  • Fable 5.2 Test PCB: A BK7238 Wi-Fi and BLE Castellated Module
  • From Datasheet to Schematic: How Fable 5.2 Read the BK7238 Reference Design
  • Fable 5.2 PCB Layout: Placement, PCB Antenna, and RF Routing
  • Fable 5.2 Design Verification: ERC, DRC, and Approved Exceptions
  • Fable 5.2 PCB Manufacturing Files: Gerbers, Drill, BOM, and CPL
  • Fable 5.2 Token Usage: How Many Tokens One PCB Design Took
  • Can AI Design a PCB? What Fable 5.2 Did Well and Where It Needed a Human
  • Conclusion
  • FAQs About AI PCB Design

ai pcb design with claude fable 5.2

Introduction

Can AI design a PCB from datasheets to manufacturing files?

We put Fable 5.2 to the test with a real hardware design project, taking it through schematic capture, PCB layout, design rule checks, and Gerber generation in KiCad 10. The result was a complete manufacturing file set with every DRC error either resolved or explicitly approved. But does that mean AI can design a reliable, working PCB on its own?

Not quite. An engineer reviewed and approved each stage, rejected the model's initial component placement, and corrected three misinterpreted reference connections. Although the final deliverables included Gerbers, a bill of materials (BOM), and component placement files, the board has not yet been fabricated or physically tested.

bk7238 wi fi module pcb in kicad designed by fable 5.2

Figure: Top view of the BK7238 Wi-Fi module PCB in KiCad designed by Fable 5.2.

In this guide, you will learn:

  • What AI achieved: The design files Fable 5.2 generated and what passing DRC actually proves.
  • How the workflow operated: The step-by-step process from datasheets to Gerbers using KiCad 10.
  • Where human intervention mattered: The placement decisions, circuit corrections, and engineering approvals.
  • What the experiment cost: The total token usage, why cache reads dominated, and what the numbers reveal about AI-assisted PCB design.

Note

JLCPCB, Anthropic (Claude), and KiCad are not affiliated with PCB_Flow or the kicad-mcp-pro project and are not responsible for designs made with them. Whoever runs an AI-assisted design flow is responsible for the design and for the third-party tools, MCP servers, and models they choose, including checking every result before fabrication.

Can AI Design a PCB? Fable 5.2 Test Results at a Glance

Fable 5.2 completed every design stage, from requirements to release files, for a 16 × 24 mm, two-layer Wi-Fi and BLE module.

Design TaskFable 5.2 ResultWhat It Does Not Prove
Part selection18 fitted parts with LCSC codes; basic parts wherever one met the requirementPart stock, which was not re-checked before release
SchematicERC with 0 violations; a custom 32-pin BK7238 symbol that matches the datasheet pin tableA readable drawing; the engineer corrected three reference-sheet connections
PlacementRev B approved after the engineer rejected Rev AHow far the antenna detunes on this board
Routing0 unconnected items, 0 clearance or short errorsRF line impedance, which is an estimate
DRC review216 items explained; four exceptions approved by the engineerThat the narrowed PA supply trace is harmless under load
Manufacturing files6 Gerbers, a drill file, a job file, and a JLCPCB-format BOM and CPLGerber content in a viewer; the files were checked by content only
HardwareNot fabricated, not bench-testedAnything that needs a VNA or a powered board

How Fable 5.2 Designed the PCB in KiCad 10

Fable 5.2 performed the design work in KiCad 10.0.4, and an engineer approved each stage before the next one began. PCB_Flow is an independent KiCad design panel we built, which sets the fixed stages and holds the model at each approval gate.

The model reads and edits the KiCad project through kicad-cli and an MCP (Model Context Protocol) server. The panel can run Claude or ChatGPT/Codex models; this test used Fable 5.2 throughout. A full PCB_Flow guide will follow once the tool is open to everyone.

For a general setup, see our KiCad MCP guide, and for a similar test in EasyEDA Pro, see Claude Code PCB design.

pcb flow panel in kicad with the 22 stage design workflow

Figure: PCB Flow panel in KiCad with the 22-stage design workflow and the AI provider selection.

The 22 stages fall into six groups:

  1. Setup and requirements: environment check, requirements, architecture, and board parameters
  2. Parts and libraries: component selection, compatibility checks, and the symbol and footprint libraries
  3. Schematic: schematic capture, schematic checks, and a datasheet review
  4. Placement: net classes, 3D models, placement references, placement plan, placement, and placement checks
  5. Routing and checks: routing setup, routing, and PCB checks
  6. Release: fabrication files, assembly files, and the release record

Each stage saves its evidence as notes. Choices that belong to the engineer, such as the layer count, appear in the panel as questions; this design logged 12 decisions, D1 to D12.

Fable 5.2 Test PCB: A BK7238 Wi-Fi and BLE Castellated Module

The main test was a standalone Wi-Fi 4 and BLE module built around the Beken BK7238, a 4 × 4 mm QFN32 chip with a 0.4 mm pin pitch. An on-board antenna makes it a demanding layout test.

The project started from our own need for a low-cost, reliable Wi-Fi and BLE option for our IoT devices, in the same role as the ESP modules. The BK7238 is a low-cost Wi-Fi 4 and BLE chip. We asked Fable 5.2 to design a castellated module around it on the familiar ESP-12F footprint, with 22 pads at 2.0 mm pitch. Only the VBAT and GND pads keep their ESP-12F positions, so the module is footprint-compatible with an ESP-12F but not pin-compatible.

ParameterValue
Board size16.00 × 24.00 mm, 0.8 mm thick
Layers2 (F.Cu, 0.73 mm FR-4 core, B.Cu), 1 oz copper, ENIG
Edge connection22 castellated pads at 2.0 mm pitch, ESP-12F footprint pattern
Main chipBK7238QH321, QFN32, 4 × 4 mm, 0.4 mm pitch
Antenna2.4 GHz meandered inverted-F PCB antenna
Clock26 MHz crystal, 9 pF load, 3225 package
References33: 18 fitted, 9 unfitted tuning positions, 6 copper-only items
Build planBare boards with a stencil, hand assembly, 5 to 10 pieces

Fable 5.2 received five inputs:

  • The BK7238 chip datasheet
  • The ME16WS02 module datasheet
  • The Beken reference schematic, revision 1.2
  • Photos of a reference module's component placement
  • A completed hand-over prompt with the board requirements

From Datasheet to Schematic: How Fable 5.2 Read the BK7238 Reference Design

Fable 5.2 turned the datasheets into a requirements list, a parts list, and a schematic that passed ERC with 0 violations. The engineer still had to settle the layer count and correct three connections that the model had misread from the reference sheet.

Requirements and Part Selection

The engineer requested basic parts from the JLCPCB Parts Library to avoid extra assembly charges. Fable 5.2 followed that rule and documented each exception:

  • Basic where possible: the exceptions, each with a stated reason, were the BK7238, the 26 MHz crystal, the 3.6 nH RF inductor, the 18 Ω PLL supply resistor, and three RF capacitors from the Preferred class.
  • Alternative offered: for the 18 Ω resistor, the model offered a Basic 22 Ω part and calculated the shift in the PLL supply filter; the engineer kept the 18 Ω reference value.
  • Layer count: the model recommended 4 layers. The engineer chose 2 layers at 0.8 mm, and the model switched to Beken's 2-layer layout rules.
  • Crystal load: with no 7–8 pF, 26 MHz crystal at LCSC, the model chose a 9 pF part. It meets the chip datasheet's 9 pF maximum but not the Beken sheet's 7–8 pF note, and the model flagged it as the largest electrical risk.

Custom BK7238 Symbol and Schematic: Correct Connectivity, Poor Readability

Fable 5.2 generated a custom BK7238 symbol from the datasheet pin table. All 32 PINs and primary pin names match the datasheet, and the exposed pad connects to ground.

bk7238 module schematic drawn by fable 5.2

Figure: BK7238 module schematic drawn by Fable 5.2, with correct connectivity but parts scattered as label-linked fragments.

Schematic readability is where the model fell short. The connections are correct, but the sheet is hard to read:

  • Fragmented circuit: Each passive sits on its own short wire between net labels, so the RF chain from the ANT pin to the antenna has to be traced label by label.
  • Crowded symbol: The pin names on the custom QFN32 symbol overlap each other at the chip body.
  • No signal flow: Supply filters, RF match, crystal, and edge pads sit in separate columns rather than flowing from input to output.

A schematic is also a review document. ERC confirms connectivity, but checking design intent depends on a drawing that an engineer can read at a glance.

Fable 5.2 PCB Layout: Placement, PCB Antenna, and RF Routing

Fable 5.2 placed and routed the board on two layers, but its first placement crowded the antenna. The engineer rejected it, and the approved second version moved the RF parts away from the antenna ground edge.

Placement Rev A Rejected, Rev B Approved

Rev A left the lower board largely empty, and the parts near the antenna posed a risk of parasitic coupling.

placement rev a rejected rev b approved

Figure: Rejected placement Rev A, with the BK7238 RF parts crowded against the antenna.

Placement MeasureRev ARev B
Chip positionStarting positionMoved 3.0 mm away from the antenna
Parts in the 4 mm strip below the antenna124: the antenna match C7, C8, C9, and test pad TP2
Nearest other part to the antenna ground edge1.0 mm4.0 mm
Test pad TP2 to the antenna ground edge0.4 mm2.3 mm
PA supply traceAlong the antenna ground edgeCrosses 4 mm from the edge

approved placement rev b

Figure: Approved placement rev B, with the chip cluster moved down to clear the strip below the antenna.

Fable 5.2 also found a gap in its own rev B: the VBAT supply pin (pin 10) had no capacitor next to it. It proposed fitting the spare C20 position with a 1 µF component and asked first because the change altered the approved parts list. The engineer agreed.

PCB Antenna and RF Match Network

Fable 5.2 did not design its own antenna. It used KiCad's library footprint of the inverted-F antenna from TI application note AN043 (SWRA117D) and confirmed a 0.8 mm margin to each side edge of the 16 mm board.

The RF match follows the Beken sheet: L1 3.6 nH, C4 1.5 pF, C6 1 pF, and C7 1 pF, plus unfitted positions C8 and C9 for tuning. The model recorded two limits:

  • Footprint not checked against the TI drawing: the model could not open the PDF, so the footprint is KiCad's drawing of the note, not checked dimension by dimension.
  • Detuning: TI designed the antenna on its own board. On 0.8 mm FR-4 with a smaller ground area, it is expected to detune by an amount that only a VNA measurement can show.

Two-Layer Routing and Supply Deviations

The routed board has 181 track segments and 28 0.30 mm vias. The RF path runs on the top layer only, with no bottom trace under it, and the 19 GPIO signals reach the edge pads on the top layer without crossings.

routed bk7238 module in kicad

Figure: Routed BK7238 module in KiCad, with top copper in red, bottom copper in blue, and ground fills kept out of the antenna area.

Two supply traces break the approved width rules. Fable 5.2 reported both and asked for approval:

  • Bottom supply branches at 0.3 mm instead of 0.5 mm: a 0.5 mm trace did not clear the ground vias next to the GND pad. The model calculated a drop of 10 mV or less at 270 mA, the datasheet's typical TX current, and these branches do not carry the PA current, which flows on the 0.5 mm branch.
  • PA supply neck at 0.25 mm for 2.0 mm: Beken recommends wider than 0.4 mm. The channel between C10 and C4 is 0.56 mm, so 0.25 mm is the widest trace that keeps 0.15 mm clearance; a wider trace needs a placement change.

Fable 5.2 Design Verification: ERC, DRC, and Approved Exceptions

The final board passed ERC with 0 violations and DRC with 0 unconnected items and 0 clearance or short errors. KiCad still listed 216 DRC items, and each one traces back to a design choice the engineer reviewed.

kicad drc result for the bk7238 module

Figure: KiCad DRC result for the BK7238 module, showing 216 violations, 26 errors, 190 warnings, and 0 unconnected items.

DRC ItemCountCauseStatus
Copper-to-edge errors22Castellated pads sit on the board edge by designApproved exception
Courtyard overlap errors4Test pad TP1 on the RF line overlaps four-part courtyardsApproved exception
Track-width warnings3117 short necks into chip and 0402 pads, plus 14 segments on the two supply deviationsReviewed and approved
Silkscreen warnings159Overlapping reference text; no silkscreen layer is exported (D12)Not in the fabrication files
Total21626 errors and 190 warningsAll reviewed

Fable 5.2 PCB Manufacturing Files: Gerbers, Drill, BOM, and CPL

Fable 5.2 exported a complete file set for fabrication and a later assembly order, and it fixed a unit problem in KiCad's placement export.

The release contains:

  • Gerbers: copper and solder mask for both sides, top paste, and the board outline, with no silkscreen layer by decision
  • Drill and job files: one plated drill file with 51 holes (28 vias, 1 antenna ground hole, 22 edge holes) and a job file
  • BOM: 18 fitted parts in JLCPCB columns with LCSC codes
  • CPL: the placement list for the same 18 parts, in millimeters
  • Documents: a 3D render, the schematic, a board PDF, and the decision log

KiCad's position export came out in inches and listed unfitted parts. Fable 5.2 rebuilt the CPL from the schematic in millimeters and checked five part centers against their pad midpoints.

Note

To create these files for your own board, see how to generate the BOM and centroid file from KiCad. The model checked the Gerbers by file content, not in a Gerber viewer. The BOM and CPL are kept so the same board can move to PCB assembly later.

Fable 5.2 Token Usage: How Many Tokens One PCB Design Took

The design used 52.3 million tokens across 343 model requests, and setup used another 13.3 million across 54 requests. About 95% of the design tokens were cache reads, the lowest-cost token type.

Token MeasureSetupDesign
Model requests54343
Fresh (uncached) input130686
Cache write1,059,0952,265,645
Cache read12,183,31349,530,929
Output (of which thinking)63,151 (27,685)542,935 (309,387)
All tokens13,305,68952,340,195
Tool calls80817
Sessions112

Setup covers the hand-over prompt, reading the datasheets, and setting up the panel. Design covers panel stages 00-21. Each token type means:

  • Fresh input: new text that is not already in the model's cache
  • Cache write: project context, such as stage instructions and datasheet text, stored the first time the model reads it
  • Cache read: the model re-reading that stored context on each request; providers typically bill it at a small fraction of the fresh-input rate, because the context is already processed.
  • Output: the text the model writes, including its internal reasoning (thinking)

cumulative fable 5.2 tokens over the run

Figure: Cumulative Fable 5.2 tokens over the run and the split by token type: 52.3 M for design and 13.3 M for setup, mostly cache reads.

For the design stage, each request re-read about 144,000 tokens of stored context and wrote about 1,580 new tokens. Reasoning took 57% of the output. The design spanned about 6 hours of wall-clock time, including waits for approvals. Token usage was higher than is practical for routine work, so a second, more token-efficient version of PCB_Flow has since been built.

Can AI Design a PCB? What Fable 5.2 Did Well and Where It Needed a Human

Fable 5.2 reasoned well through a staged design and stated what it had not verified. It still required an engineer for key decisions, reference sheet corrections, and drawing quality.

What Fable 5.2 Did Well

  • Reasoning with numbers: it backed each trade-off with a calculation, such as the voltage drop on a narrowed supply trace or the filter shift from a Basic resistor.
  • Step-by-step flow: it worked through 22 stages in order and kept evidence notes for each, so a stopped run resumed without repeating work.
  • Plain-language instructions: PCB_Flow's stage instructions are written in plain language, and the model followed them stage by stage.
  • Questions before guesses: it raised 12 decisions, from layer count to silkscreen, and asked for approval instead of guessing, including deviations from rules it had set itself.
  • Stated limits: each stage note lists what was not verified, such as the unopened TI PDF, the unviewed Gerbers, and the crystal pad map.

Where the Engineer Stepped In

TaskFable 5.2Engineer
Layer countRecommended 4 layersChose 2 layers at 0.8 mm
Reference schematicMisread three connectionsCorrected them in D9
PlacementCrowded the antenna in rev ARejected rev A, approved rev B
Pin 10 decouplingFound the missing capacitorApproved fitting C20 with 1 µF
DRC reviewListed and explained all 216 itemsApproved four exceptions
SilkscreenReported overlapping reference textChose no silkscreen layer (D12)
Schematic readabilityCorrect but fragmented drawingNot yet solved

Verdict: Can Fable 5.2 Design a PCB on Its Own?

Fable 5.2 is a capable PCB design assistant. It can carry a design to manufacturing files under engineer supervision, but it does not yet replace the engineer's review.

Its connections and checks were sound, while its schematic and symbols were accurate but hard to read. To become more capable, it needs more training on PCB design or a dataset of reviewed designs to learn from.

For other AI tools at each design stage, see AI tools for PCB design guide.

Conclusion

AI can design a PCB up to manufacturing files: Fable 5.2 took a BK7238 Wi-Fi module from datasheets to Gerbers, BOM, and CPL, with an engineer approving each stage and every DRC exception. Use it as a staged assistant behind human approval gates, and treat each passed check as a file-level result until the board is tested. Fabrication, assembly, and hardware testing remain the next steps toward validating the design.

jlcpcb pcb assembly service banner 1
Ready to turn your PCB design into real hardware?
Quote Now
  • Whether you designed it manually or with AI assistance, upload your Gerber files and BOM to JLCPCB to get an instant quote for PCB fabrication and assembly.

  • Move from digital design to a physical prototype and put your circuit to the test.

FAQs About AI PCB Design

Can AI Design a PCB Without a Human?

Not yet. In this test, Fable 5.2 needed an engineer to choose the layer count, correct three reference connections, reject a placement, and approve four DRC exceptions.

Did the Fable 5.2 Board Work?

Not known yet. The module is designed and passes DRC with approved exceptions, but it has not been fabricated, so antenna tuning, TX power, and crystal frequency remain unproven.

How Many Tokens Does AI Need to Design a PCB?

This BK7238 module used 52.3 million tokens for the design and 13.3 million for setup. About 95% of the design tokens were cache reads, which are typically billed at a fraction of the fresh-input rate.

Can AI Design an RF PCB with an Antenna?

Only as far as the layout. Fable 5.2 placed a TI inverted-F antenna and the Beken match network, but tuning and RF line impedance need a VNA measurement on a built board.

Which PCB Design Software Did Fable 5.2 Use?

KiCad 10.0.4. Fable 5.2 worked on the live project through the kicad-mcp-pro MCP server and kicad-cli, guided by the PCB_Flow panel with an approval gate at each stage.

Keep Learning