KiCad MCP connects an AI assistant to tools that can read or change a KiCad project. You can use it to investigate component connections, make supported design edits, and request checks against actual project data. The available operations depend on the MCP server you install.
This guide uses Windows, KiCad 10, Konnect, and Claude Desktop to explain the connection process and a first PCB edit. You will move one footprint, compare the result with its starting state, and check whether the edit introduced a board-rule violation. The walkthrough follows project documentation; the example is a practice exercise rather than a measured test result.
What Is KiCad MCP?
KiCad MCP is a general name for integrations that give AI applications access to KiCad-related tools through the Model Context Protocol. Different servers expose different features, so there is no single installation that represents every KiCad MCP project.
The connection works like this:
Your request → AI application → MCP server → KiCad data or tools
The AI application interprets your request and calls an available tool. The server carries out the operation through its supported interface, such as KiCad’s API, a project file, or a command-line tool. The Model Context Protocol provides the communication framework between the application and server.
For example, you might ask which pins connect to a particular net before investigating a schematic problem. In an editing workflow, you might ask the assistant to move a footprint to a specified position. The practical benefit is that the answer or action can be tied to the design you are working on.
Which AI Assistants Work with KiCad MCP?
Claude Desktop, Claude Code, GitHub Copilot in VS Code, Cursor, and Windsurf have configuration routes documented by the projects below. Choose a combination with instructions for both your AI application and your selected server.
| AI application | Documented connection route |
|---|---|
| Claude Desktop | Konnect’s local server setup, used in this guide |
| Claude Code | Konnect’s project-level MCP configuration |
| GitHub Copilot in VS Code | The original KiCAD-MCP-Server configuration |
| Cursor or Windsurf | Seeed’s MCP client configuration |
A model name alone does not establish compatibility. The application hosting the model must support the server’s connection method and permit tool calls. For the walkthrough below, run Claude Desktop and KiCad on the same Windows computer.
Which KiCad MCP Server Should You Use?
For the live footprint edit in this guide, use Konnect with KiCad 10. If your main task is schematic analysis or you already maintain a different integration, compare the alternatives by the work you need to perform.
| Server | When to consider it | Setup consideration |
|---|---|---|
| Konnect | Editing a live KiCad 10 board through its IPC API | Native plugin package; currently identified as beta |
| Original KiCAD-MCP-Server | Continuing or adapting an existing workflow built around this implementation | Separate Python/TypeScript dependencies; do not use Konnect’s installation instructions |
| Seeed-Studio kicad-mcp-server | Investigating components, nets, and pin connections in project files | Its documented full PCB analysis setup uses KiCad’s Python environment |
Konnect is the original project’s successor, while the original server remains maintained. For a new installation following this article, staying with Konnect keeps the package, configuration, and editing tools consistent. Check the chosen project’s license before adopting it for your intended use.
For Seeed’s server, the Python environment affects the information available: its documented system-Python fallback offers more limited PCB analysis. That distinction matters if your task needs detailed board information rather than basic component or net data.
How Do You Connect AI to KiCad Using MCP?
Install the plugin, enable KiCad’s API connection, register the server in Claude Desktop, and confirm that it can read your board. Use a separate practice copy of an existing project, keeping its board, schematic, and project settings together.
1. Install the Konnect plugin.
Download the Windows PCM ZIP from Konnect Releases. In KiCad 10, open Plugin and Content Manager, choose Install from File, select the ZIP, and restart KiCad. Check Tools → External Plugins in the PCB Editor for Konnect. The PCM ZIP is the plugin package; other release archives may contain standalone server binaries.
2. Connect Konnect to the open board.
Open the practice board and enable the KiCad API under Plugins in KiCad’s preferences. Copy the complete listening address, including ipc://. In Konnect’s settings, paste that address into the IPC Socket field and save it. This address must come from your own KiCad session.
3. Register Konnect in Claude Desktop.
Edit %APPDATA%\Claude\claude_desktop_config.json. If you have no existing server configuration, use the following structure. Otherwise, add only the konnect entry inside your existing mcpServers object, keeping the other entries intact.
{
"mcpServers": {
"konnect": {
"command": "C:\\Users\\YOUR_NAME\\Documents\\KiCad\\10.0\\3rdparty\\plugins\\com_github_mixelpixx_konnect\\bin\\konnect.exe"
}
}
}Replace the example command with the actual installed executable path. The doubled backslashes are required by JSON string escaping. Check that the executable exists, save the configuration, and fully restart Claude Desktop.
4. Read the practice board.
Keep the board open and send this prompt:
Use Konnect to inspect the board currently open in KiCad. Report the board file path, copper layer count, and component references. Do not change anything. Include the tool output that identifies whether you accessed the live board or a saved file; if the tool does not report this, say so.
Compare the file path and references with your practice project. Proceed when the returned information matches. If tools are visible but the board cannot be read, use the connection troubleshooting section before requesting an edit.
How Do You Edit a PCB with KiCad MCP?
Describe the object, the change, and the properties that must stay fixed. A first edit should be easy to inspect, such as moving one unlocked, unrouted resistor on a practice board.
The Konnect tool directory covers schematic operations, footprint placement, routing, and checks. These are distinct tasks: moving a component is a useful introduction to editing, while routing requires its own instructions and review.
Prepare a baseline before changing anything.
Choose a resistor with enough clear space around it for a 2 mm move. Save the practice project and keep an untouched copy for comparison. In the PCB Editor, run Inspect → Design Rules Checker with zone refill enabled and save the report. This gives you the board’s starting condition, including any existing unconnected items.
Read the component’s starting state.
Use its actual reference in this prompt; R1 is the example:
Find R1 on the practice board. Report its X and Y coordinates in millimetres, rotation, board side, and pad net names. Do not modify it.
Check these values in KiCad’s footprint properties and pad properties. Use the same coordinate origin and units throughout the comparison. If the returned data does not match, resolve the discrepancy before continuing.
Request one specific edit.
Move R1 by +2.0 mm along the board’s X axis. Keep its Y coordinate, rotation, board side, and pad net assignments unchanged. Do not change tracks, vias, other components, or design rules. Stop if R1 is locked or the operation cannot be completed as specified.
An axis and distance give you a measurable result. An instruction such as “improve the layout” leaves the assistant to decide which objects and relationships it can change.
Read back the position.
Read R1 again using the board tools. Report its current coordinates, rotation, board side, and pad net names, and compare them with the starting values.
The expected relationship is:
X_after = X_before + 2.0 mm; Y_after = Y_before
Verify the result in KiCad. Reading R1 back establishes its reported state; checking for unrelated changes requires a wider comparison, as described below.
How Do You Check AI Changes in KiCad?
Check three things: whether the requested change happened, whether other design objects changed, and whether the board developed new rule violations. Each requires different evidence.
| Check | Evidence to use |
|---|---|
| Requested footprint move | Before-and-after footprint and pad properties in KiCad |
| Unrelated changes | A comparison with the untouched board, including object properties and saved-file differences where needed |
| New board-rule violations | DRC reports from before and after the edit, using the same settings |
Inspect the board beyond the moved footprint.
Look for overlap with adjacent components, movement across the board edge, and unexpected changes to nearby tracks or vias. Compare the edited board with the untouched copy before accepting the change. A saved-file diff can reveal additional edits, but formatting changes and generated data still need interpretation.
A visual review is useful for placement; it does not establish that every property stayed unchanged. If you have only checked R1, keep the conclusion limited to R1. An AI statement that “nothing else changed” needs supporting comparison data.
Compare the DRC results.
Run the checker again with zone refill enabled, using the same rules as the baseline. Inspect individual findings and their locations. A board can have the same total error count while one old problem disappears and a different problem appears.
On an unrouted practice board, existing unconnected items may remain after a successful move. Investigate newly introduced violations and any unexpected changes to the earlier findings. If the edit is wrong, undo it in KiCad or restore the practice copy, then recheck before trying again.
Match the check to the design change.
A footprint-only move calls for placement, connectivity, and board-rule review. If you also change the schematic, run electrical rule checking and check that the schematic and PCB remain consistent. Neither test establishes the circuit’s functional performance.
How Do You Fix KiCad MCP Connection Problems?
First determine whether the failure is between Claude Desktop and the server, or between the server and KiCad. Visible MCP tools confirm only the first part of that connection.
| Symptom | First action |
|---|---|
| No Konnect tools appear | Check the executable path and JSON syntax, then fully restart Claude Desktop |
| Tools appear, but the board is unavailable | Open the board, enable KiCad’s API, and save the current IPC address in Konnect |
| Results miss your latest edits | Check whether the tool read a saved file or the live editor before requesting further work |
| An older installation seems to be running | Use get_installation_info to check the active executable and build |
A check reports that kicad-cli is missing |
Check the CLI path and the active Konnect configuration |
After correcting a setting, repeat the read-only board prompt from the connection section. Confirm that the expected project is accessible before resuming edits.
If you need help, include the exact error, installed versions, and last successful step. “Konnect tools appear, but reading the open board fails” identifies the failing stage more clearly than “KiCad MCP does not work.”
FAQs About KiCad MCP
Is KiCad MCP an official KiCad product?
The servers discussed here are third-party projects. Using KiCad’s API does not make an integration an official KiCad product.
Can KiCad MCP work without the PCB Editor open?
Yes, for supported file-based operations. For example, schematic-file analysis can use a different access method from live board editing. The footprint exercise in this guide uses an open PCB Editor and an active IPC connection.
Does KiCad MCP include an AI model?
The server supplies tools. Your AI application supplies model access, with its own account and usage requirements.
Can I ask AI to design an entire PCB immediately?
Some servers provide schematic creation, placement, and routing tools, so a larger design request can involve several supported operations. Their availability does not guarantee a correct complete board from a short prompt. You still need to define the circuit requirements and review the electrical and physical design. This guide covers the first connection and edit.
Does a clean DRC report mean the PCB is ready to manufacture?
No. It means the board passed the enabled checks. Fabrication and assembly readiness also depend on the chosen stackup, manufacturing capabilities, and component requirements.
When you are ready to turn the reviewed design into hardware, EBest Circuit (Best Technology) can discuss PCB fabrication and PCBA requirements with you. Contact sales@bestpcbs.com with your KiCad MCP project requirements to discuss manufacturing support.
You may also like
Tags: KiCad MCP, KiCad MCP Server