SolidWorks Macro Tutorial: Your First VBA Macro

A SolidWorks macro is a small program that drives SolidWorks for you. Anything you click — new part, sketch, extrude, save — the macro can do through the SolidWorks API, and it will do it the same way every time. This tutorial takes you from recording a macro to writing one that builds a part on its own. You need SolidWorks (any recent version) and nothing else: the VBA editor is built in.

1. Record a macro and read what SolidWorks wrote

1. Open a new part. Go to Tools → Macro → Record (or the Record button on the Macro toolbar).
2. Sketch a rectangle on the Front plane and extrude it 10 mm.
3. Tools → Macro → Stop, save it as FirstMacro.swp.
4. Tools → Macro → Edit, pick the file. The VBA editor opens with code like this:

Dim swApp As Object
Dim Part As Object
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long

Sub main()
    Set swApp = Application.SldWorks
    Set Part = swApp.ActiveDoc
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
    Part.SketchManager.InsertSketch True
    Part.SketchManager.CreateCornerRectangle 0, 0, 0, 0.05, 0.03, 0
    Part.FeatureManager.FeatureExtrusion2 True, False, False, 0, 0, 0.01, 0.01, False, False, False, False, 0, 0, False, False, False, False, True, True, True, 0, 0, False
    Part.ClearSelection2 True
End Sub

Three things to notice, because they are the whole SolidWorks API in miniature:

• swApp is SolidWorks itself (SldWorks), Part is the open document (ModelDoc2). Every macro starts by getting these two.
• Lengths are in metres: 0.05 is 50 mm, 0.01 is 10 mm. Forgetting this is the number-one beginner bug.
• FeatureExtrusion2 has a long list of arguments. The recorder fills them in; you only ever change one or two (depth, direction).

2. Turn the recording into a macro that builds the part itself

The recorded macro assumes a part is already open and a sketch plane is selected by name. Let us make it self-contained: create a new part from the default template, sketch, extrude, and name the feature.

Option Explicit

Sub main()
    Dim swApp As SldWorks.SldWorks
    Dim swModel As SldWorks.ModelDoc2
    Dim swFeat As SldWorks.Feature
    Dim template As String

    Set swApp = Application.SldWorks
    template = swApp.GetUserPreferenceStringValue(swUserPreferenceStringValue_e.swDefaultTemplatePart)
    Set swModel = swApp.NewDocument(template, 0, 0, 0)

    ' sketch a 50 x 30 mm rectangle on the Front plane
    swModel.Extension.SelectByID2 "Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0
    swModel.SketchManager.InsertSketch True
    swModel.SketchManager.CreateCornerRectangle 0, 0, 0, 0.05, 0.03, 0
    swModel.SketchManager.InsertSketch True   ' close the sketch

    ' extrude it 10 mm (blind, one direction)
    swModel.Extension.SelectByID2 "Sketch1", "SKETCH", 0, 0, 0, False, 0, Nothing, 0
    Set swFeat = swModel.FeatureManager.FeatureExtrusion2(True, False, False, 0, 0, 0.01, 0.01, _
        False, False, False, False, 0, 0, False, False, False, False, True, True, True, 0, 0, False)

    If Not swFeat Is Nothing Then
        swFeat.Name = "Base-Plate"
    End If

    swModel.ViewZoomtofit2
End Sub

Before running it, add the type library so VBA knows the SolidWorks types: in the VBA editor, Tools → References, tick SldWorks 20xx Type Library and SolidWorks 20xx Constant type library. That is what makes SldWorks.ModelDoc2 and swUserPreferenceStringValue_e resolve, and it gives you IntelliSense for every method.

Run it with F5. SolidWorks opens a new part, draws the rectangle, extrudes it and renames the feature. Change 0.05, 0.03 and 0.01 and run it again — that is already a parametric part generator.

3. Make it ask for the sizes

A macro that asks for inputs is the first thing engineers actually use day to day. Replace the three numbers with a tiny prompt:

    Dim w As Double, h As Double, d As Double
    w = CDbl(InputBox("Width (mm)", "Base plate", 50)) / 1000
    h = CDbl(InputBox("Height (mm)", "Base plate", 30)) / 1000
    d = CDbl(InputBox("Thickness (mm)", "Base plate", 10)) / 1000

and use w, h in CreateCornerRectangle and d for both depth arguments of FeatureExtrusion2. Dividing by 1000 converts the millimetres people type into the metres the API expects.

4. Where to go next

• Traverse what exists: swModel.FirstFeature and Feature.GetNextFeature walk the feature tree — the basis of every "find all holes and change their diameter" macro.
• Drawings and BOMs: DrawingDoc.CreateDrawViewFromModelView3 places views; ModelDoc2.SaveAs3 exports PDF/DXF in a batch.
• From VBA to C#: the same objects and methods are available from C# as a standalone program or an add-in, which is where you go when a macro grows into a tool other people use.

All of that is the curriculum of the SolidWorks API & Automation Course: it opens with exactly these VBA macros and continues to C# add-ins, drawings and batch processing. If you want to try the teaching style first, the trial lesson is the first chapter of that course.

Common errors, and what they mean

Message	Cause	Fix
Object variable or With block variable not set	swApp.ActiveDoc was Nothing — no document open	Open a part, or create one with NewDocument as above
User-defined type not defined	Type library reference missing	Tools → References → tick the SldWorks type libraries
Rectangle is tiny or huge	Millimetres given where metres are expected	Divide by 1000
FeatureExtrusion2 returns Nothing	The sketch was not selected, or is still open	Close the sketch with InsertSketch True, then select it by name