Millwright — API Reference & SolidWorks COM Cheat Sheet

Version 1.0 · 2026-04-23

1. LLM Adapter API

1.1 Configuration Interface

interface LLMConfig {
  protocol: 'anthropic' | 'openai';  // API protocol
  baseURL: string;                    // Service endpoint
  apiKey: string;                     // Auth key
  model: string;                      // Model identifier
  systemPrompt?: string;              // Custom system prompt
  temperature?: number;               // Sampling temperature (0–1, default 0.3)
  maxTokens?: number;                 // Max output tokens (default 4096)
  stream?: boolean;                   // Stream output (default true)
}

1.2 Message Format

interface ChatMessage {
  role: 'user' | 'assistant' | 'system';
  content: string;
  toolCalls?: ToolCall[];             // Tools the AI requested to call
  code?: string;                      // Extracted code block
  codeLanguage?: 'vba' | 'python';   // Code language
}

interface ToolCall {
  name: string;                       // Tool name
  parameters: Record<string, any>;    // Call parameters
  result?: string;                    // Execution result
}

1.3 Anthropic Protocol Request Format

{
  "model": "claude-sonnet-4-20250514",
  "max_tokens": 4096,
  "system": "You are a SolidWorks automation assistant...",
  "messages": [
    { "role": "user", "content": "Change every fillet to 3mm" }
  ]
}

Headers:

Content-Type: application/json
x-api-key: sk-ant-xxxxx
anthropic-version: 2023-06-01

1.4 OpenAI-Compatible Protocol Request Format

{
  "model": "gpt-4o",
  "messages": [
    { "role": "system", "content": "You are a SolidWorks automation assistant..." },
    { "role": "user", "content": "Change every fillet to 3mm" }
  ]
}

Headers:

Content-Type: application/json
Authorization: Bearer sk-xxxxx

2. COM Bridge API

2.1 Connection Management

class SolidWorksBridge {
  connect(): Promise<boolean>          // Connect to SolidWorks
  disconnect(): void                   // Disconnect
  isConnected(): boolean               // Check connection status
  getVersion(): string                 // Get SW version
  getActiveDocument(): ModelDoc2       // Get the active document
  getDocumentType(): 'part' | 'assembly' | 'drawing' | null
}

2.2 Script Execution

interface ScriptResult {
  success: boolean;
  output: string;        // Standard output
  error?: string;        // Error message
  duration: number;      // Execution duration (ms)
}

class ScriptEngine {
  runVBA(code: string): Promise<ScriptResult>
  runPython(code: string): Promise<ScriptResult>
  validate(code: string): { safe: boolean; issues: string[] }
}

2.3 Registered Tool List

Tool	Description	Parameters
`create_part`	Create a new part	—
`create_assembly`	Create a new assembly	—
`create_drawing`	Create a new drawing	template?: string
`create_sketch`	Start a sketch	plane: Front/Top/Right
`close_sketch`	Close the current sketch	—
`draw_rectangle`	Draw a rectangle	x, y, width, height (mm)
`draw_circle`	Draw a circle	x, y, radius (mm)
`draw_line`	Draw a line segment	x1, y1, x2, y2 (mm)
`extrude_feature`	Extrude feature	depth (mm), direction?: both
`cut_extrude`	Cut-extrude	depth (mm)
`create_revolve`	Revolve feature	angle (degrees)
`create_fillet`	Fillet	radius (mm)
`create_chamfer`	Chamfer	distance (mm)
`create_pattern`	Linear pattern	count, spacing (mm), direction
`mirror_feature`	Mirror feature	plane: Front/Top/Right
`insert_component`	Insert component	filePath
`add_mate`	Add mate	type: coincident/parallel/...
`modify_dimensions`	Modify dimension	featureName, dimName, value
`export_step`	Export STEP	outputPath
`export_pdf`	Export PDF	outputPath
`export_stl`	Export STL	outputPath, quality?
`export_dxf`	Export DXF	outputPath
`batch_rename`	Batch rename	pattern, replacement
`check_interference`	Interference check	—
`mass_properties`	Mass properties	—
`bom_export`	BOM export	outputPath, format: xlsx/csv

3. SolidWorks COM API Cheat Sheet

3.1 Connection & Documents

' Get the SolidWorks application
Dim swApp As SldWorks.SldWorks
Set swApp = Application.SldWorks

' Get the active document
Dim swModel As ModelDoc2
Set swModel = swApp.ActiveDoc

' Create a new part
Dim templatePath As String
templatePath = swApp.GetUserPreferenceStringValue(swUserPreferenceStringValue_e.swDefaultTemplatePart)
Set swModel = swApp.NewDocument(templatePath, 0, 0, 0)

' Open a file
Dim errors As Long, warnings As Long
Set swModel = swApp.OpenDoc6("C:\parts\bracket.sldprt", swDocPART, swOpenDocOptions_Silent, "", errors, warnings)

' Save
swModel.Save3 swSaveAsOptions_Silent, errors, warnings

' Save as STEP
swModel.Extension.SaveAs "C:\output\part.step", swSaveAsCurrentVersion, swSaveAsOptions_Silent, Nothing, errors, warnings

3.2 Sketch Operations

' Select a reference plane
swModel.Extension.SelectByID2 "Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0

' Enter sketch mode
swModel.SketchManager.InsertSketch True

' Draw a rectangle (in meters)
swModel.SketchManager.CreateCornerRectangle -0.025, 0.015, 0, 0.025, -0.015, 0

' Draw a circle
swModel.SketchManager.CreateCircle 0, 0, 0, 0.01, 0, 0

' Draw a line
swModel.SketchManager.CreateLine 0, 0, 0, 0.05, 0.03, 0

' Exit sketch mode
swModel.SketchManager.InsertSketch True

3.3 Feature Operations

' Extrude (boss)
swModel.FeatureManager.FeatureExtrusion3 _
    True, False, False, _           ' Single direction, not a cut
    0, 0, _                         ' End condition: given depth
    0.02, 0, _                      ' Depth 20 mm
    False, False, False, False, _
    0, 0, False, False, False, False, _
    True, True, True, 0, 0, False

' Cut-extrude
swModel.FeatureManager.FeatureCut4 _
    True, False, False, _
    0, 0, _
    0.01, 0, _                      ' Cut depth 10 mm
    False, False, False, False, _
    0, 0, False, False, False, False, _
    True, True, True, True, _
    0, 0, False

' Fillet (first select an edge)
swModel.Extension.SelectByID2 "", "EDGE", 0.025, 0.015, 0.02, False, 1, Nothing, 0
swModel.FeatureManager.FeatureFillet3 195, 0.003, 0, 0, 0, 0, 0  ' 3 mm fillet

' Revolve
swModel.FeatureManager.FeatureRevolve2 True, True, False, False, False, False, _
    0, 0, 6.28318530718, 0, False, False, 0, 0, 0, 0, 0, True, True, True

3.4 Dimension Modification

' Modify a dimension
Dim swDim As Dimension
Set swDim = swModel.Parameter("D1@Boss-Extrude1")
swDim.SetSystemValue3 0.03, swSetValue_InAllConfigurations, Nothing  ' Change to 30 mm

' Iterate all dimensions
Dim swFeat As Feature
Set swFeat = swModel.FirstFeature
Do While Not swFeat Is Nothing
    Dim swDispDim As DisplayDimension
    Set swDispDim = swFeat.GetFirstDisplayDimension
    Do While Not swDispDim Is Nothing
        Dim swDimObj As Dimension
        Set swDimObj = swDispDim.GetDimension2(0)
        Debug.Print swDimObj.FullName & " = " & swDimObj.GetSystemValue3(1, Nothing) * 1000 & " mm"
        Set swDispDim = swFeat.GetNextDisplayDimension(swDispDim)
    Loop
    Set swFeat = swFeat.GetNextFeature
Loop

3.5 Assembly Operations

' Get the assembly document
Dim swAssembly As AssemblyDoc
Set swAssembly = swModel

' Insert a component
Dim swComponent As Component2
Set swComponent = swAssembly.AddComponent5( _
    "C:\parts\bolt_m6.sldprt", _
    swAddComponentConfigOptions_CurrentSelectedConfig, _
    "", False, "", 0, 0, 0)

' Add a coincident mate
swModel.Extension.SelectByID2 "Face1@Part1-1", "FACE", 0, 0, 0, False, 1, Nothing, 0
swModel.Extension.SelectByID2 "Face1@Part2-1", "FACE", 0, 0, 0, True, 1, Nothing, 0
swAssembly.AddMate5 swMateCOINCIDENT, swMateAlignALIGNED, False, 0, 0, 0, 0, 0, 0, 0, 0, False, False, 0, errors

3.6 Drawing Operations

' Get the drawing document
Dim swDrawing As DrawingDoc
Set swDrawing = swModel

' Create a view
swDrawing.CreateDrawViewFromModelView3 _
    "C:\parts\bracket.sldprt", "*Front", _
    0.15, 0.15, 0  ' Position (m)

' Insert model annotations
swDrawing.InsertModelAnnotations3 0, 32776, True, True, False, True

3.7 Python (win32com) Equivalent

import win32com.client

# Connect
sw = win32com.client.Dispatch("SldWorks.Application")
sw.Visible = True

# Active document
model = sw.ActiveDoc

# Create a new part
template = sw.GetUserPreferenceStringValue(21)  # swDefaultTemplatePart
model = sw.NewDocument(template, 0, 0, 0)

# Sketch
model.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, None, 0)
model.SketchManager.InsertSketch(True)
model.SketchManager.CreateCornerRectangle(-0.025, 0.015, 0, 0.025, -0.015, 0)
model.SketchManager.InsertSketch(True)

# Extrude
model.FeatureManager.FeatureExtrusion3(
    True, False, False, 0, 0,
    0.02, 0,  # 20 mm
    False, False, False, False,
    0, 0, False, False, False, False,
    True, True, True, 0, 0, False
)

# Export
errors, warnings = 0, 0
model.Extension.SaveAs2(
    r"C:\output\part.step", 0, 1, None, "", False, errors, warnings
)

4. IPC Protocol

Electron main and renderer communicate via IPC:

Channel	Direction	Data	Description
`sw:connect`	R→M	—	Request connection to SolidWorks
`sw:status`	M→R	{ connected, version }	Connection status
`sw:heartbeat`	M→R	boolean	Heartbeat result
`llm:chat`	R→M	{ messages, config }	Send chat
`llm:stream`	M→R	{ chunk, done }	Streaming response
`llm:error`	M→R	{ message, code }	Error info
`script:run`	R→M	{ code, lang }	Execute script
`script:result`	M→R	ScriptResult	Execution result
`config:save`	R→M	LLMConfig	Save config
`config:load`	M→R	LLMConfig	Load config

5. Error Code Reference

Code	Description	Handling
`SW_NOT_FOUND`	SolidWorks is not running	Tell the user to start SW
`SW_NO_DOCUMENT`	No open document	Tell the user to open a file
`SW_COM_ERROR`	COM call failed	Retry or check SW version
`LLM_AUTH_FAILED`	API auth failed	Check API key
`LLM_RATE_LIMIT`	API rate-limited	Wait and retry
`LLM_NETWORK_ERROR`	Network error	Check network/proxy
`SCRIPT_UNSAFE`	Script failed safety check	Show specific risks
`SCRIPT_EXEC_FAILED`	Script execution failed	Show error details
`SCRIPT_TIMEOUT`	Script execution timed out	Abort and notify

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Millwright — API Reference & SolidWorks COM Cheat Sheet

1. LLM Adapter API

1.1 Configuration Interface

1.2 Message Format

1.3 Anthropic Protocol Request Format

1.4 OpenAI-Compatible Protocol Request Format

2. COM Bridge API

2.1 Connection Management

2.2 Script Execution

2.3 Registered Tool List

3. SolidWorks COM API Cheat Sheet

3.1 Connection & Documents

3.2 Sketch Operations

3.3 Feature Operations

3.4 Dimension Modification

3.5 Assembly Operations

3.6 Drawing Operations

3.7 Python (win32com) Equivalent

4. IPC Protocol

5. Error Code Reference