AI assistance for CATIA V5 in vehicle development

1. What this is about

You know CATIA V5: sketches, Pads, Pockets, surfaces in Generative Shape Design, assemblies with constraints, parameters and measurements. Much of this work consists of recurring, clearly describable steps – a bracket with four mounting holes, a bolt circle on a flange, a wall-thickness variant with weight comparison, a STEP export for the supplier, a profile of a part you have taken over.

An AI assistant (for example GitHub Copilot in agent mode) can carry out these steps for you if it is allowed to operate CATIA. That is exactly what the MCP server does: it gives the assistant 86 clearly defined tools – “create sketch on XY”, “draw rectangle”, “Pad 12 mm”, “measure volume and centre of gravity”, “set parameter”, “export as STEP”. You describe the goal in plain language; the assistant breaks it down into tool calls, executes them in your running CATIA session and reports what happened.

Guiding principle of this project: The AI proposes and operates – CATIA calculates – the design engineer decides. Dimensions, volumes and distances come from CATIA, not from the language model. The language model is good at breaking an instruction into steps, calculating coordinates and summarising results; it is not a calculation program and knows your model only through what the tools report back.

2. How the AI works with CATIA

The building blocks in simple terms

MCP (Model Context Protocol)

An open standard through which an AI assistant uses external tools. Each tool has a name (e.g. catia_pad), a description and precisely defined parameters (e.g. height in mm).

MCP server

A small Python program that runs on the CATIA machine. It translates tool calls into CATIA commands and returns the response.

COM Automation

The programming interface that CATIA V5 provides for macros. In principle, anything a VBA or CATScript macro can do, the MCP server can also do – but only what a tool has been built for.

A workflow in detail

1. You describe the goal, e.g. “Create a plate 120 × 80 × 8 mm, centred on the origin, and give me its volume and mass in aluminium.”
2. The assistant plans: new part → sketch on XY → centred rectangle → close sketch → Pad 8 mm → measure with density 2700 kg/m³.
3. It calls the tools one after another. Each call is executed in your visible CATIA session – you see the tree grow.
4. CATIA calculates (update, volume) and reports back.
5. The assistant reports and states the values used. You check in CATIA (Measure Inertia) and decide.

3. Maturity and trust

Not all of the 86 tools are equally reliable. We use three levels; they appear next to every tool in the catalogue:

The reasons for each rating are given in chapter 8. As soon as the first test has run on a machine with a CATIA licence, this table will be updated – with CATIA release, date and result.

4. Setup and protection

Prerequisites

• Windows machine with CATIA V5 and a valid licence for the required workbenches (Part Design, Generative Shape Design, Assembly Design; for measurements, the usual measuring functions).
• GitHub Copilot in VS Code or Visual Studio 2022 (17.14 or later) with agent mode. With a company licence (Copilot Business/Enterprise), the organisation must enable the policy “MCP servers in Copilot” – it is off by default.
• Python 3.10–3.13 in your own user profile. Admin rights are not required.
• Agreement with IT/data protection on which model information may be sent to the AI service (see below).

Installation in four steps – without admin rights

1. Install Python for your own user (python.org installer, untick “Use admin privileges …”) – or use an existing Python.
2. Place the project folder in your own user profile (ZIP or Git).
3. Double-click scripts\setup_user.cmd. The script creates the Python environment, installs the server, creates the working folder %USERPROFILE%\CATIA_MCP_Work, writes the Copilot configuration .vscode\mcp.json with Safe Mode and checks everything without CATIA.
4. In VS Code, open the project folder, in .vscode\mcp.json, above the catia-v5 entry, click Start, and open Copilot Chat in Agent mode. Start CATIA normally beforehand (not “as administrator”).

The detailed guide with troubleshooting, and the list of cases where company policies do require IT after all (e.g. Copilot policy, AppLocker, missing CATIA COM registration), is in the project under docs/ANLEITUNG_COPILOT.md.

What the Copilot configuration looks like

Generated by the setup script with the paths on your machine; you do not have to write it by hand.

{
  "servers": {
    "catia-v5": {
      "type": "stdio",
      "command": "C:\\Users\\Name\\catia-ai-mcp\\.venv\\Scripts\\python.exe",
      "args": ["-m", "catia_mcp"],
      "env": {
        "CATIA_MCP_SAFE_MODE": "1",
        "CATIA_MCP_WORK_DIR": "C:\\Users\\Name\\CATIA_MCP_Work",
        "CATIA_MCP_RESULT_FORMAT": "v2"
      }
    }
  }
}

Working with Copilot

• Copilot asks for confirmation before every tool call. You can approve read-only tools (lists, measuring) for the session; saving, export and model changes are better confirmed individually.
• The chat’s tools menu shows the 86 CATIA tools. If Copilot reports “more than 128 tools”, deselect tools or other servers you do not need.
• Select a capable model in the model menu; simple models are worse at breaking down multi-step design instructions.

Safe Mode – strongly recommended

Without protection, the assistant can save an open original in place or overwrite arbitrary files. Safe Mode prevents this:

Typical workflow with a working copy: open the original → “Save a working copy as C:/CATIA_MCP_Work/Bracket_v1.CATPart” → from now on the session works with the copy → changes → saving goes to the copy. The original is no longer touched. If the assistant nevertheless tries to save an original, it receives a clear error message with the safe alternative.

Structured results (v2)

With CATIA_MCP_RESULT_FORMAT=v2, every tool reports a structured result: ok/not ok, a unique error code (e.g. NO_ACTIVE_DOCUMENT, OBJECT_NOT_FOUND, POLICY_BLOCKED) and a safe recommended action. This lets the assistant detect errors reliably instead of reading them out of free text. Without this setting, the server behaves exactly like the original project.

Data protection and confidentiality

To get started, we recommend purpose-built or anonymised test models.

5. Good working practice

5.1 Writing instructions so that the result is right

Proven elements of an instruction:

• Starting point: which document, which state (“in the active part”, “open copy X”).
• Geometry with units: dimensions always in mm, angles in degrees; state the plane (XY/YZ/ZX) and the reference point.
• Names: have features, sketches and surfaces named (“name the surface Duct_Inner”) – this makes later steps unambiguous.
• Check step: “then measure …”, “list the features”, “give volume and centre of gravity”.
• Limits: “no fillets”, “only on the copy”, “do not save anything”.
• Stop point for large instructions: “Show me the plan with all tool calls first, before you execute.”

5.2 Units, planes and coordinate systems

• Lengths: all tools work in millimetres. Angles: degrees (the server converts to radians internally where necessary).
• Volume/area: mm³ and mm² respectively; catia_get_inertia also outputs cm³/cm². Density in kg/m³ (steel ≈ 7850, aluminium ≈ 2700, PA6 GF30 ≈ 1360 – use the values from your material data sheet).
• Sketch coordinates are local: in a sketch, x/y mean the horizontal and vertical axis of the sketch plane, not automatically the global X/Y. On the YZ plane, for example, the sketch horizontal is the global Y axis. If in doubt, have the position confirmed by a measurement.
• Vehicle coordinates: many vehicle parts are modelled in the vehicle coordinate system (typically: X rearwards, Y to the right, Z upwards, origin at the vehicle zero point – your company standard is authoritative). The tools always use the part’s absolute coordinates. State in the instruction whether dimensions refer to the part system or the vehicle system.
• Planes: the Sketcher tools and many Part Design tools only know the three origin planes xy, yz, zx. Offset planes can be created with the surface tools (catia_gsd_plane_offset) and used there as a reference.

5.3 Names and references

The tools find elements by their name in the specification tree (e.g. Sketch.2, Pad.1, Contour_A). Three rules follow from this:

1. Names depend on the language: a German CATIA user interface may generate different default names from an English one. Assigning your own names is more robust.
2. Without a name, many tools take the most recently created element (last sketch, last feature). This is convenient but error-prone if something else has been created in between.
3. Edges and faces have no stable names. Tools that would need a specific edge or face (fillet, chamfer, draft, shell) are therefore currently not reliable.

5.4 Checking results – “measure, don’t trust”

Today, a success message means: CATIA accepted the command without error. It does not mean that the geometry looks as intended (a Pocket in the wrong direction, for example, cuts into empty space). So have a measurement taken after every material change:

• Volume before and after the feature (catia_get_inertia) – does it increase or decrease?
• Main dimensions – measure in CATIA (the Automation interface does not offer a bounding box), or by distance measurement to offset planes.
• Feature list – was the feature created, and what is it called?
• And finally: look in CATIA, take your own measurements at critical points.

Undo: “Show the journal” and “Undo the last change” revert the assistant’s last step (parameter value or most recently created feature) – as long as nothing has been built on it.

New (25 Sep 2026): with CATIA_MCP_RESULT_FORMAT=v2 – set by the setup script – the server measures the body volume before and after for 15 material tools (Pad, Pocket, Shaft, Groove, Hole, Shell, patterns, fillet …). A feature with no effect (“Pocket into empty space”) or with the wrong direction is reported as an error, together with the volume change and a recommended action. Tested offline, not yet confirmed in CATIA; your own check is still needed.

6. Tool catalogue – all 86 tools

Each tool with its purpose from a design engineer’s point of view, key parameters, maturity and notes. You do not need to know the tool names – the assistant chooses them itself. The overview helps you judge what is possible and what you are better off doing yourself.

6.1 Session and documents (9)

6.2 Sketcher – 2D sketches (11)

Sketches are always placed in the main body (PartBody) on one of the three origin planes. Coordinates are local sketch coordinates in mm.

6.3 Part Design – solids (15)

All features are created in the main body. Without sketch_name/feature_name, the most recently created sketch or the last feature is used.

6.4 Generative Shape Design – wireframe and surface geometry (24)

This group was tested by the original project in a real CATIA session (30/30 steps) and is the most carefully implemented. New elements are placed in the active Geometrical Set (if there is none, one is created). If an element fails on update, it is removed from the tree again and the reason is reported. Points can be given as a name or as [x, y, z] in mm.

6.5 Assemblies – Assembly Design (9)

6.6 Measuring and parameters (6)

6.7 View and export (4)

6.8 Session: journal and undo (2) – new

An addition by this project. During the running session, the server logs parameter changes and features created by material tools – including defective features from failed calls (K14).

6.9 Product structure, Knowledge and batch processing (6) – new

An addition by this project, tested offline against the simulator; Automation members checked against the reference (pycatia), not confirmed in CATIA. Details: docs/EXTENDED_TOOLS.md.

7. Use cases in vehicle development

The following scenarios show how to combine today’s tools sensibly. They have been chosen so that they get by with the reliable tools or explicitly work around the limits. The dialogues are shortened; the tool calls show what happens in the background. All dimensions are examples – not design specifications. Measured values in the responses are illustrative (not obtained in CATIA); where they can be recalculated, they have been.

7.1 Profile of a part you have taken over

Situation: You take over a part from a previous project or from a colleague – e.g. an ancillary-unit bracket – and need to get an overview quickly: structure, driving parameters, main dimensions, weight.

Benefit: familiarisation in minutes instead of half an hour; the profile can be taken straight into handover or review documents. Risk: low (read-only). Tip: Ask for anomalies to be listed – e.g. parameters without a comment, features that have not been renamed, very long trees.

7.2 Designing a simple bracket

Situation: A control unit, a relay carrier or a sensor needs a simple sheet-metal or machined bracket for a concept, a prototype or a package-space study.

Why holes as circle + Pocket? The hole tool currently ignores the hole type and deviates from the CATIA call; circle and Pocket are more reliable. The assistant checks the volume decrease against the circle formula – a simple but effective plausibility test.

What you do yourself: fillets and chamfers (tools not reliable), bend radii for sheet metal, tolerances, thread specifications.

7.3 Variant study and weight comparison

Situation: Lightweight-design discussion: how does the mass of a bracket change if the wall thickness goes from 4 to 3 mm and the rib height from 20 to 25 mm? Which combination stays within the package space?

Benefit: parameter studies that would otherwise cost an hour of clicking and an Excel list run reproducibly. Important: the server does not yet have automatic undo; so always ask in the instruction to “note the original values and reset them”, and work on a copy. A separate file for each variant: “save each variant as Bracket_W3_R25.CATPart in the working folder”.

7.4 Hole patterns, bolt circles and flange variants

Situation: A connection flange (e.g. exhaust, intake, pump) needs a bolt circle, or a hole pattern has to be adapted to a supplier part.

Why calculate instead of using a circular pattern? The circular-pattern tool cannot select the axis of rotation. The coordinates are simple trigonometry – the assistant shows the working, you can check it, and the result does not depend on an uncertain pattern function. Irregular hole patterns can be taken over from a supplier table in the same way (“hole pattern as per table: …”).

Variant: checking a supplier part’s hole pattern – “list the centre points of all circles in Sketch.4 and compare them with this table” (with catia_sketch_get_geometry while the sketch is open; coordinates may have to be read off in CATIA, as the tool only returns names and types).

7.5 Package-space and clearance study on a part

Situation: A part has to fit into a defined package space or maintain a minimum distance from a boundary surface (e.g. 10 mm from a heat-shield surface, 25 mm clearance from an envelope surface).

1. Have the boundaries created as geometry: “In the set ‘PackageSpace’, create a plane 180 mm above XY (upper package-space limit) and one 60 mm beside ZX.” (catia_gsd_plane_offset)
2. Measure distances: “Measure the minimum distance between PartBody and Limit_Top.” (catia_measure_distance)
3. Create an envelope: “Create an offset surface 10 mm around the surface HeatShield and measure the distance to the bracket.” (catia_gsd_offset_surface + measurement)
4. Have the result documented as a table with target/actual.

7.6 Surface design: air ducting, trim panel, duct

Situation: Concept phase of an air duct (e.g. brake cooling, charge air, cabin ventilation) or of a trim shell: cross-sections at specific stations, the shape in between, material thickness.

Further surface tasks: section contours at fixed stations (catia_gsd_intersection with offset planes) for cross-section progressions; mirroring to the other side of the vehicle (catia_gsd_symmetry about the vehicle centre); material thickness of shells via catia_gsd_offset_surface/thick_surface; blend surfaces (catia_gsd_blend) between two connecting contours.

7.7 Package space for lines and hoses

Situation: A coolant hose or wiring harness is to be routed between two connection points; you need an envelope geometry early on for package-space coordination.

1. Connection and support points in vehicle coordinates as 3D points (catia_gsd_point), e.g. from a table.
2. Routing as a spline through the points (catia_gsd_spline).
3. Cross-section: circle with outer diameter plus allowance at the first point, perpendicular to the line – for this, a plane through three points or an offset plane (catia_gsd_plane_3points, catia_gsd_circle).
4. Envelope tube by Sweep (catia_gsd_sweep), measure distances to neighbouring parts.

7.8 Assembly check

Situation: Before a review or a data handover, you want to know whether an assembly is consistent.

Not reliable today: creating constraints (coincidence, offset, angle) and reading exact positions. Use the assistant here as an inspector, not as an assembler.

7.9 Review documents and data exchange

• Views for the presentation: “Isometric, fit all, screenshot to C:/CATIA_MCP_Work/review/bracket_iso.jpg; then front view and top view.” (catia_set_view, catia_fit_all, catia_screenshot)
• Supplier or simulation data: “Export the working copy as STEP and as STL to the working folder, file name = part number + index.” (catia_export)
• Accompanying text: from the profile and measured values, the assistant can draft a data-handover text or a review slide – with mass, main dimensions, material, status.

Note: the image size is currently the window size. Exports are subject to your company’s licences and export rules (export control, confidentiality).

7.10 Checking design guidelines and naming conventions

Situation: Your department has modelling guidelines – e.g. “all driving dimensions as named parameters”, “give features meaningful names”, “wall thickness ≥ 2.5 mm”, “at most one main body”.

Benefit: quick pre-check before release or handover. Limit: the language model checks the rules against the reported data; geometric rules (minimum radius, wall thickness at every point, demouldability) need real analysis functions and are part of the outlook.

7.11 Onboarding, learning and explaining

• “Explain the structure of this part to me step by step – which sketch creates which feature, and which parameters control what?”
• “What modelling sequence would you suggest for a casting with ribs, bosses and drafts?” (planning, no execution)
• “How would I build this bracket in GSD instead of Part Design, and what are the pros and cons?”

For newcomers, this is a patient tutor that explains using the real model. Bear in mind that explanations of general CATIA functions come from the language model’s knowledge and may be wrong – if in doubt, consult the CATIA help or ask colleagues.

7.12 Batch processing: mass list and supplier export

Situation: Before a milestone, you need a mass list of all parts in a module, or a supplier is to receive all parts as STEP.

Safety: each file is closed without saving, documents that are already open are left untouched, existing export files are never overwritten. In Safe Mode, the source folder must be permitted (CATIA_MCP_READ_DIRS) and the export target must be in the working folder.

8. Limits and known issues

Fundamental limits

Known issues of the current tools

From the code analysis (25 Sep 2026), partly documented by the original project itself. The numbers refer to docs/PHASE1_FINDINGS.md.

Operational limits

• One session, one assistant: parallel operation by you and the AI in the same document leads to confusing states.
• CATIA dialogs: if CATIA opens a message box (e.g. update error, licence notice), the tool call waits – close the dialog and have the assistant re-read the current state.
• User interface language: default names (e.g. “Pad” vs. the German “Block”) depend on the CATIA language.
• Licences: every workbench and every export format needs the appropriate licence; if it is missing, CATIA reports an error.

9. Outlook: what the extensions make possible

The CATIA V5 Automation interface is far more extensive than today’s 86 tools. In principle, what a VBA macro can do, an MCP tool can do as well. On top of this comes the optional native extension (CAA) for the few cases that Automation does not cover. The following overview shows realistic extension stages – ordered by benefit for vehicle development. Each function is built only when a concrete use case and a test model are available, and depends on your CATIA licences.

Ideas with particularly high value for design engineers

10. Roadmap

The contribution that helps most: name two to three concrete, recurring workflows from your day-to-day work – with an anonymised example model and what has to come out at the end. The next tools will be derived from these.

11. Glossary

12. Frequently asked questions

Does the assistant replace CATIA skills?

No. It speeds up routine work and helps with understanding. To check results and write good instructions, you still need solid CATIA and design skills.

Can the assistant damage my original data?

Without Safe Mode: yes, by saving. With Safe Mode and a working folder: saving and exporting are only possible to working copies. Even so, never work with released states.

Why should I re-measure when the assistant reports “successful”?

Because “successful” today only means that CATIA accepted the command. Only a measurement shows whether the feature produces the desired geometry. This check will be automated in phase 2.

What data does the AI service see?

Everything contained in the tool responses: names, paths, parameters, dimensions, volumes. No CATPart files and no images. Clarify use with real project data with your IT and data protection teams beforehand.

Does this work with my CATIA version?

The server uses the standard Automation of CATIA V5. Which releases work will be determined in the first test with a licence and recorded in a compatibility list.

Do I need administrator rights?

No. Python, the server and the Copilot configuration are set up in your own user profile. It can only fail because of company settings: the Copilot policy “MCP servers in Copilot” (for Business/Enterprise), programs blocked in the user profile (AppLocker) or a missing COM registration of CATIA. Details in docs/ANLEITUNG_COPILOT.md.

Does this also work with Microsoft 365 Copilot or Copilot in Windows?

No. These variants cannot start local MCP servers on your machine. You need GitHub Copilot in agent mode in VS Code or Visual Studio.

Can I request my own tools?

Yes – that is exactly how the extensions come about. Describe the workflow, the expected result and a test model (see Roadmap).