AI in SOLIDWORKS: Create Parts Automatically Using Smart Macros!
Unlock the future of CAD automation! In this video, I show you how to integrate AI with SOLIDWORKS to automatically create 3D parts using smart macros.
If you’re still modelling manually in 2025, you’re already behind — AI-powered macros can speed up your workflow, reduce repetitive tasks, and instantly generate code for part creation.
Cope the below macro code:
Option Explicit
Sub main()
Dim swApp As Object, swModel As Object
Dim swSketchMgr As Object, swFeatMgr As Object, swExt As Object
' Connect to SolidWorks (Late Binding)
On Error Resume Next
Set swApp = GetObject(, "SldWorks.Application")
If swApp Is Nothing Then
Set swApp = CreateObject("SldWorks.Application")
If swApp Is Nothing Then
MsgBox "Unable to start SolidWorks.", vbCritical
Exit Sub
End If
End If
On Error GoTo 0
swApp.Visible = True
' Template path (update for your version, e.g. 2026)
Dim templatePath As String
templatePath = "C:\ProgramData\SolidWorks\SOLIDWORKS 2026\templates\Part.prtdot"
If Dir(templatePath) = "" Then
MsgBox "Template file not found at: " & vbCrLf & templatePath, vbCritical
Exit Sub
End If
' Create new part
Set swModel = swApp.NewDocument(templatePath, 0, 0, 0)
If swModel Is Nothing Then
MsgBox "Failed to create new part.", vbCritical
Exit Sub
End If
' ISO bolt data arrays (M1–M36, coarse threads)
Dim sizes, dVals, sVals, kVals, pVals, lengthOptions
sizes = Array("M1", "M1.2", "M1.6", "M2", "M2.5", "M3", "M4", "M5", _
"M6", "M8", "M10", "M12", "M14", "M16", "M18", "M20", _
"M22", "M24", "M27", "M30", "M33", "M36")
dVals = Array(1, 1.2, 1.6, 2, 2.5, 3, 4, 5, _
6, 8, 10, 12, 14, 16, 18, 20, _
22, 24, 27, 30, 33, 36)
sVals = Array(2, 2.5, 3.2, 4, 5, 5.5, 7, 8, _
10, 13, 16, 18, 21, 24, 27, 30, _
34, 36, 41, 46, 50, 55)
kVals = Array(0.8, 1, 1.3, 1.6, 2, 2.4, 3.2, 4, _
4, 5.3, 6.4, 7.5, 8.8, 10, 11.5, 12.5, _
14, 15, 17, 19, 21, 23)
pVals = Array(0.25, 0.25, 0.35, 0.4, 0.45, 0.5, 0.7, 0.8, _
1, 1.25, 1.5, 1.75, 2, 2, 2.5, 2.5, _
2.5, 3, 3, 3.5, 3.5, 4)
' Ask user for bolt size
Dim sizeList As String, i As Integer
For i = LBound(sizes) To UBound(sizes)
sizeList = sizeList & sizes(i) & IIf(i < UBound(sizes), ", ", "")
Next
Dim boltSize As String
boltSize = InputBox("Select Bolt Size from: " & vbCrLf & sizeList, "ISO Bolt Generator", "M6")
boltSize = UCase(Trim(boltSize))
Dim idx As Integer: idx = -1
For i = LBound(sizes) To UBound(sizes)
If sizes(i) = boltSize Then idx = i: Exit For
Next
If idx = -1 Then
MsgBox "Invalid bolt size entered.", vbCritical
Exit Sub
End If
' Length options
lengthOptions = Array(6, 8, 10, 12, 16, 20, 25, 30, 35, 40, 45, 50, _
60, 70, 80, 90, 100, 120, 150, 200)
Dim lenList As String
For i = LBound(lengthOptions) To UBound(lengthOptions)
lenList = lenList & lengthOptions(i) & IIf(i < UBound(lengthOptions), ", ", "")
Next
Dim Lmm As Double
Lmm = Val(InputBox("Select Bolt Length (mm) from: " & vbCrLf & lenList, "ISO Bolt Generator", lengthOptions(0)))
If Lmm <= 0 Then
MsgBox "Invalid length.", vbCritical
Exit Sub
End If
' Convert mm to meters
Dim d As Double, s As Double, k As Double, L As Double, pitch As Double
d = dVals(idx) / 1000#
s = sVals(idx) / 1000#
k = kVals(idx) / 1000#
L = Lmm / 1000#
pitch = pVals(idx) / 1000#
Dim callout As String
callout = sizes(idx) & "x" & CStr(pVals(idx))
' Geometry Creation
Set swSketchMgr = swModel.SketchManager
Set swFeatMgr = swModel.FeatureManager
Set swExt = swModel.Extension
' Shaft
swExt.SelectByID2 "Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0
swSketchMgr.InsertSketch True
swSketchMgr.CreateCircleByRadius 0, 0, 0, d / 2#
swSketchMgr.InsertSketch True
swFeatMgr.FeatureExtrusion2 True, False, False, 0, 0, L, 0, False, False, False, False, 0, 0, _
False, False, False, False, True, True, True, 0, 0, False
' Hex head
swExt.SelectByID2 "Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0
swSketchMgr.InsertSketch True
swSketchMgr.CreatePolygon 0, 0, 0, 0, s / 2#, 0, 6, False
swSketchMgr.InsertSketch True
swFeatMgr.FeatureExtrusion2 True, False, False, 0, 0, k, 0, False, False, False, False, 0, 0, _
False, False, False, False, True, True, True, 0, 0, False
' Cosmetic Thread
Dim selEdgeOk As Boolean
selEdgeOk = swExt.SelectByID2("", "EDGE", d / 2#, 0, 0, False, 0, Nothing, 0)
If Not selEdgeOk Then
selEdgeOk = swExt.SelectByID2("", "EDGE", d / 2#, 0, L, False, 0, Nothing, 0)
End If
If Not selEdgeOk Then
MsgBox "Could not select shaft edge for cosmetic thread.", vbExclamation
Exit Sub
End If
Dim threadDia As Double
threadDia = d - 0.0002
Dim myFeature As Object
Set myFeature = swFeatMgr.InsertCosmeticThread2(False, threadDia, L, callout)
If myFeature Is Nothing Then
MsgBox "Failed to create cosmetic thread.", vbCritical
Exit Sub
End If
' Make cosmetic threads visible
swApp.SetUserPreferenceToggle 9, True ' 9 = swDetailingDisplayCosmeticThreads
swModel.GraphicsRedraw2
MsgBox "ISO Bolt " & sizes(idx) & " x " & Lmm & " mm with visible cosmetic thread (" & callout & ") created successfully!", vbInformation
End Sub
Use it, modify it, and automate your workflow!
This is not just a tutorial — it’s the start of smart, automated CAD design.
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