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Hello all,
i have point/axis, from that i need to create the surface extrusion for dia of 5mm through vba.
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Hi @gopinathmY575P,
The code below let you select a surface (planar) and a work axis, then create the sketch and extrude the circle (cut operation) :
Dim s As Inventor.Face = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick face")
Dim w As Inventor.WorkAxis = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kWorkAxisFilter, "Pick work axis")
Dim tg As Inventor.TransientGeometry = ThisApplication.TransientGeometry
Dim Doc As Inventor.PartDocument = ThisApplication.ActiveDocument
Dim PartCompDef As Inventor.PartComponentDefinition = Doc.ComponentDefinition
Dim NewSketch As Inventor.PlanarSketch = PartCompDef.Sketches.Add(s, False)
Dim p As Inventor.SketchPoint = NewSketch.AddByProjectingEntity(w)
Dim c As Inventor.SketchCircle = NewSketch.SketchCircles.AddByCenterRadius(p, 0.25)
NewSketch.DimensionConstraints.AddDiameter(c, tg.CreatePoint2d(0,0), False)
NewSketch.Solve
Dim def As Inventor.ExtrudeDefinition = PartCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(NewSketch.Profiles.AddForSolid, PartFeatureOperationEnum.kCutOperation)
'def.SetDistanceExtent(10, PartFeatureExtentDirectionEnum.kSymmetricExtentDirection)
def.SetThroughAllExtent(PartFeatureExtentDirectionEnum.kSymmetricExtentDirection)
Dim f As Inventor.ExtrudeFeature = PartCompDef.Features.ExtrudeFeatures.Add(def)
Here is the end result :
Kind regards,
FINET L.
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And here is the file with the code.
Kind regards,
FINET L.
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Actually very similar :
Dim s As Inventor.Face = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick face")
Dim w As Inventor.WorkAxis = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kWorkAxisFilter, "Pick work axis")
Dim tg As Inventor.TransientGeometry = ThisApplication.TransientGeometry
Dim Doc As Inventor.PartDocument = ThisApplication.ActiveDocument
Dim PartCompDef As Inventor.PartComponentDefinition = Doc.ComponentDefinition
Dim NewSketch As Inventor.PlanarSketch = PartCompDef.Sketches.Add(s, False)
Dim p As Inventor.SketchPoint = NewSketch.AddByProjectingEntity(w)
Dim c As Inventor.SketchCircle = NewSketch.SketchCircles.AddByCenterRadius(p, 0.25)
NewSketch.DimensionConstraints.AddDiameter(c, tg.CreatePoint2d(0,0), False)
NewSketch.Solve
Dim def As Inventor.ExtrudeDefinition = PartCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(NewSketch.Profiles.AddForSurface, PartFeatureOperationEnum.kSurfaceOperation)
def.SetDistanceExtent(5, PartFeatureExtentDirectionEnum.kSymmetricExtentDirection)
'def.SetThroughAllExtent(PartFeatureExtentDirectionEnum.kSymmetricExtentDirection)
Dim f As Inventor.ExtrudeFeature = PartCompDef.Features.ExtrudeFeatures.Add(def)
Kind regards,
FINET L.
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You just have to change here as stated above :
NewSketch.Profiles.AddForSurface, PartFeatureOperationEnum.kSurfaceOperation
Kind regards,
FINET L.
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