Hi Arun
Is it because you are not giving any input to macro like Sketch/Surface for profile and Axis for rotation of Shaft.
You have recorded the macro but need to provide the input.
This is my opinion and hope that it answers your question.
I have created a MACRO with sketch - Rectangular Profile and Vertical direction line of the sketch as rotation axis.
Hope this is full to you.
Language="VBSCRIPT"
Sub CATMain()
Set partDocument1 = CATIA.ActiveDocument
Set part1 = partDocument1.Part
Set hybridBodies1 = part1.HybridBodies
'----->with below line the Sketch will always be created in GS1.
'Set hybridBody1 = hybridBodies1.Item("Open_body.1")
'---->>> with below line sketch will always be created in acitve GS
Set hybridBody1 = CATIA.ActiveDocument.Part.InWorkObject
MsgBox ("This Macro is to create sketch for Shaft creation")
Msgbox("Pickup the reference plane for sketch")
Dim InputObjectType(0), Status1
Set selection1 = partDocument1.Selection
selection1.Clear
InputObjectType(0)="Plane"
Status1=selection1.SelectElement2(InputObjectType,"Select plane",false)
If Status1 = "Cancel" Then selection1.Clear: Exit Sub
Set reference1 = selection1.Item(1).Reference
MsgBox reference1.Name
Msgbox("Pickup the reference point to sketch reference")
InputObjectType(0)="Point"
Status1=selection1.SelectElement2(InputObjectType,"Reference point",false)
If Status1 = "Cancel" Then selection1.Clear: Exit Sub
Set reference2 = selection1.Item(1).Reference
MsgBox reference2.Name
Set sketches1 = hybridBody1.HybridSketches
Set originElements1 = part1.OriginElements
Set sketch1 = sketches1.Add(reference1)
part1.InWorkObject = sketch1
Set factory2D1 = sketch1.OpenEdition()
Set geometricElements1 = sketch1.GeometricElements
Set axis2D1 = geometricElements1.Item("AbsoluteAxis")
Set line2D1 = axis2D1.GetItem("HDirection")
line2D1.ReportName = 1
Set line2D2 = axis2D1.GetItem("VDirection")
line2D2.ReportName = 2
Set point2D1 = factory2D1.CreatePoint(15.000000, 40.000000)
point2D1.ReportName = 3
Set point2D2 = factory2D1.CreatePoint(65.000000, 40.000000)
point2D2.ReportName = 4
Set line2D3 = factory2D1.CreateLine(15.000000, 40.000000, 65.000000, 40.000000)
line2D3.ReportName = 5
line2D3.StartPoint = point2D1
line2D3.EndPoint = point2D2
Set point2D3 = factory2D1.CreatePoint(65.000000, 15.000000)
point2D3.ReportName = 6
Set line2D4 = factory2D1.CreateLine(65.000000, 40.000000, 65.000000, 15.000000)
line2D4.ReportName = 7
line2D4.EndPoint = point2D2
line2D4.StartPoint = point2D3
Set point2D4 = factory2D1.CreatePoint(15.000000, 15.000000)
point2D4.ReportName = 8
Set line2D5 = factory2D1.CreateLine(65.000000, 15.000000, 15.000000, 15.000000)
line2D5.ReportName = 9
line2D5.StartPoint = point2D3
line2D5.EndPoint = point2D4
Set line2D6 = factory2D1.CreateLine(15.000000, 15.000000, 15.000000, 40.000000)
line2D6.ReportName = 10
line2D6.EndPoint = point2D4
line2D6.StartPoint = point2D1
Set constraints1 = sketch1.Constraints
Set reference1 = part1.CreateReferenceFromObject(line2D3)
Set reference2 = part1.CreateReferenceFromObject(line2D1)
Set constraint1 = constraints1.AddBiEltCst(catCstTypeHorizontality, reference1, reference2)
constraint1.Mode = catCstModeDrivingDimension
Set reference3 = part1.CreateReferenceFromObject(line2D5)
Set reference4 = part1.CreateReferenceFromObject(line2D1)
Set constraint2 = constraints1.AddBiEltCst(catCstTypeHorizontality, reference3, reference4)
constraint2.Mode = catCstModeDrivingDimension
Set reference5 = part1.CreateReferenceFromObject(line2D4)
Set reference6 = part1.CreateReferenceFromObject(line2D2)
Set constraint3 = constraints1.AddBiEltCst(catCstTypeVerticality, reference5, reference6)
constraint3.Mode = catCstModeDrivingDimension
Set reference7 = part1.CreateReferenceFromObject(line2D6)
Set reference8 = part1.CreateReferenceFromObject(line2D2)
Set constraint4 = constraints1.AddBiEltCst(catCstTypeVerticality, reference7, reference8)
constraint4.Mode = catCstModeDrivingDimension
Set reference9 = part1.CreateReferenceFromObject(line2D1)
Set reference10 = part1.CreateReferenceFromObject(line2D5)
Set constraint5 = constraints1.AddBiEltCst(catCstTypeDistance, reference9, reference10)
constraint5.Mode = catCstModeDrivingDimension
Set length1 = constraint5.Dimension
length1.Value = 15.000000
Set reference11 = part1.CreateReferenceFromObject(line2D2)
Set reference12 = part1.CreateReferenceFromObject(line2D6)
Set constraint6 = constraints1.AddBiEltCst(catCstTypeDistance, reference11, reference12)
constraint6.Mode = catCstModeDrivingDimension
Set length2 = constraint6.Dimension
length2.Value = 15.000000
Set reference13 = part1.CreateReferenceFromObject(line2D4)
Set constraint7 = constraints1.AddMonoEltCst(catCstTypeLength, reference13)
constraint7.Mode = catCstModeDrivingDimension
Set length3 = constraint7.Dimension
length3.Value = 25.000000
Set reference14 = part1.CreateReferenceFromObject(line2D6)
Set reference15 = part1.CreateReferenceFromObject(line2D4)
Set constraint8 = constraints1.AddBiEltCst(catCstTypeDistance, reference14, reference15)
constraint8.Mode = catCstModeDrivingDimension
Set length4 = constraint8.Dimension
length4.Value = 50.000000
sketch1.CloseEdition
part1.InWorkObject = hybridBody1
part1.UpdateObject sketch1
part1.Update
' - - This roation is done only for reference - need not be used
Set hybridShapeFactory1 = part1.HybridShapeFactory
Set hybridShapeRotate1 = hybridShapeFactory1.AddNewEmptyRotate()
Set reference15 = part1.CreateReferenceFromObject(sketch1)
hybridShapeRotate1.ElemToRotate = reference15
hybridShapeRotate1.VolumeResult = False
hybridShapeRotate1.RotationType = 0
Set reference16 = axis2D1.GetItem("HDirection")
hybridShapeRotate1.Axis = reference16
hybridShapeRotate1.AngleValue = 90.000000
hybridBody1.AppendHybridShape hybridShapeRotate1
part1.InWorkObject = hybridShapeRotate1
part1.Update
Shaft = Msgbox("Do you want to create PAD" , vbYesNo+vbQuestion, "Tell me")
If Shaft = vbYes Then
'Msgbox "Shaft"
Set bodies1 = part1.Bodies
Set body1 = bodies1.Add()
part1.InWorkObject = body1
Set shapeFactory1 = part1.ShapeFactory
Set reference1 = part1.CreateReferenceFromName("")
Set shaft1 = shapeFactory1.AddNewShaftFromRef(reference1)
Set angle1 = shaft1.FirstAngle
angle1.Value = 360.000000
Set parameters1 = part1.Parameters
Set reference2 = part1.CreateReferenceFromObject(sketch1)
shaft1.SetProfileElement reference2
Set geometricElements1 = sketch1.GeometricElements
Set axis2D1 = geometricElements1.Item("AbsoluteAxis")
Set reference3 = axis2D1.GetItem("VDirection")
shaft1.RevoluteAxis = reference3
part1.UpdateObject shaft1
part1.UpdateObject body1
Else
MsgBox " Thank you for using this macro"
End if
part1.Update
End Sub