Create Trimmed Surface Feature Example (VBA)

This example shows how to create a trimmed surface feature.

' ******************************************************************************
' Preconditions:
' 1. Specified part document template exists.
' 2. Run the macro.
'
' Postconditions:
' 1. Creates two intersecting surfaces.
' 2. Selects Surface-Extrude2 as the trim tool and sets the trimming options.
' 3. Trims Surface-Extrude1.
' ******************************************************************************

Option Explicit

Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swSketchMgr As SldWorks.SketchManager
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSketchSegment As SldWorks.SketchSegment
Dim swFeatureMgr As SldWorks.FeatureManager
Dim swSelMgr As SldWorks.SelectionMgr
Dim swFeat As SldWorks.Feature
Dim status As Boolean


Sub main()

	Set swApp = Application.SldWorks

	' Create new part document
	Set swModel = swApp.NewDocument("C:\ProgramData\SolidWorks\SolidWorks 2013\templates\Part.prtdot", 0, 0, 0)
	Set swSketchMgr = swModel.SketchManager
	Set swModelDocExt = swModel.Extension
	Set swFeatureMgr = swModel.FeatureManager
	Set swSelMgr = swModel.SelectionManager

	' Create two intersecting surfaces
	status = swModelDocExt.SelectByID2("Right Plane", "Plane", 0, 0, 0, False, 0, Nothing, 0)
	swSketchMgr.InsertSketch True
	Set swSketchSegment = swSketchMgr.CreateLine(-0.068922, 0.023964, 0#, 0.042733, 0.005543, 0#)
	swModel.ClearSelection2 True
	status = swModelDocExt.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, 0)
	swFeatureMgr.FeatureExtruRefSurface2 True, False, False, 0, 0, 0.06604, 0.00254, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, False, False, False, False
	swSelMgr.EnableContourSelection = False

	status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, 0)
	swSketchMgr.InsertSketch True
	Set swSketchSegment = swSketchMgr.CreateLine(-0.041529, 0.023059, 0#, -0.052625, -0.081662, 0#)
	swModel.ClearSelection2 True
	status = swModelDocExt.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, 0)
	swFeatureMgr.FeatureExtruRefSurface2 False, False, False, 0, 0, 0.0889, 0.06604, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, False, False, False, False
	swSelMgr.EnableContourSelection = False

	' Set the trimming options
	status = swFeatureMgr.PreTrimSurface(False, True, False, False)

	' Trim the surface
	status = swModelDocExt.SelectByID2("", "SURFACEBODY", 2.89416986472588E-02, 7.81827749557351E-03, 2.90635845400971E-02, True, 0, Nothing, 0)
	Set swFeat = swFeatureMgr.PostTrimSurface(True)

End Sub