Create Revolve Features Example (VBA)

This example shows how to create revolves features.

 

'----------------------------------------------------

'

' Preconditions: Open a new part document.

'

' Postconditions: Two revolve and one cut-revolve features are created.

'

'-----------------------------------------------------

Option Explicit

 

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swModelDocExt As SldWorks.ModelDocExtension

Dim FeatureData As SldWorks.RevolveFeatureData2

Dim Feature As Feature

Dim swFeatMgr As SldWorks.FeatureManager

Dim swSelMgr As SldWorks.SelectionMgr

Dim boolstatus As Boolean

 

 

Sub main()

 

Set swApp = Application.SldWorks

Set swModel = swApp.ActiveDoc

Set swModelDocExt = swModel.Extension

Set swSelMgr = swModel.SelectionManager

 

' Create an axis

boolstatus = swModelDocExt.SelectByID2("Right Plane", "PLANE", 0, 0, 0, True, 0, Nothing, swSelectOptionDefault)

boolstatus = swModelDocExt.SelectByID2("Top Plane", "PLANE", 0, 0, 0, True, 0, Nothing, swSelectOptionDefault)

swModel.InsertAxis2 True

 

' Create a rectangle

boolstatus = swModelDocExt.SelectByID("Top Plane", "PLANE", -0.08954836342753, 4.336873289503E-04, 0.006720765739942, False, 0, Nothing, swSelectOptionDefault)

swModel.InsertSketch2 True

swModel.ClearSelection2 True

swModel.SketchRectangle -0.05668466821757, -0.02198379306525, 0, -0.01330857427717, 0.03972855876814, 0, 1

 

' Create the first revolve feature

swModel.InsertSketch2 True

swModel.ShowNamedView2 "*Trimetric", 8

boolstatus = swModelDocExt.SelectByID("Axis1", "AXIS", 0, 0, 0, True, 0, Nothing, swSelectOptionDefault)

swModel.ClearSelection2 True

boolstatus = swModelDocExt.SelectByID("Sketch1", "SKETCH", 0, 0, 0, False, 0, Nothing, swSelectOptionDefault)

boolstatus = swModelDocExt.SelectByID("Axis1", "AXIS", 0, 0, 0, True, 4, Nothing, swSelectOptionDefault)

Set swFeatMgr = swModel.FeatureManager

swFeatMgr.FeatureRevolve 6.28318530718, False, 0, 0, 0, 1, 1, 1

 

' Create a cut-revolve feature using a face on the revolve feature

swSelMgr.EnableContourSelection = 0

boolstatus = swModelDocExt.SelectByID("", "FACE", -0.03095803920934, 0.01509536510872, 0.02198379306526, False, 0, Nothing, swSelectOptionDefault)

swModel.InsertSketch2 True

swModel.ClearSelection2 True

swModel.SketchRectangle -0.04194874421597, 0.01774859621099, 0, -0.01883036471929, -0.01265654504095, 0, 1

swModel.InsertSketch2 True

boolstatus = swModelDocExt.SelectByID("Line4@Sketch2", "EXTSKETCHSEGMENT", -0.01883036471929, 0.003802500010693, 0, True, 0, Nothing, swSelectOptionDefault)

swModel.ClearSelection2 True

boolstatus = swModelDocExt.SelectByID("Sketch2", "SKETCH", 0, 0, 0, False, 0, Nothing, swSelectOptionDefault)

boolstatus = swModelDocExt.SelectByID("Line4@Sketch2", "EXTSKETCHSEGMENT", -0.01883036471929, 0.003802500010693, 0, True, 4, Nothing, swSelectOptionDefault)

swFeatMgr.FeatureRevolveCut 6.26573201466, False, 0, 0, 0, 1, 1

 

' Create the second revolve feature using a face on the first revolve feature

swSelMgr.EnableContourSelection = 0

boolstatus = swModelDocExt.SelectByID("", "FACE", -0.02333512246603, 0.03472018719853, 0.0219837930652, False, 0, Nothing, swSelectOptionDefault)

swModel.InsertSketch2 True

swModel.ClearSelection2 True

swModel.CreateCircle2 -0.02232361399104, 0.03354683337932, 0, -0.01445073476016, 0.02795861773112, 0

swModel.InsertSketch2 True

boolstatus = swModelDocExt.SelectByID("", "EDGE", -0.02437300231541, 0.01770755773555, 0.02200276940169, True, 0, Nothing, swSelectOptionDefault)

swModel.ClearSelection2 True

boolstatus = swModelDocExt.SelectByID("Sketch3", "SKETCH", 0, 0, 0, False, 0, Nothing, swSelectOptionDefault)

boolstatus = swModelDocExt.SelectByID("", "EDGE", -0.02437300231541, 0.01770755773555, 0.02200276940169, True, 4, Nothing, swSelectOptionDefault)

swFeatMgr.FeatureRevolve 6.28318530718, False, 0, 0, 0, 1, 1, 1

swSelMgr.EnableContourSelection = 0

 

End Sub