This is a question of math, but I think it may help for some developers who may not have time to dig into by Inventor API. The VBA code below is written by my colleague Brian Ekins long time ago for one case. It self explains the workflow.
Public Sub TestSphere()
Dim oTG As TransientGeometry
Set oTG = ThisApplication.TransientGeometry
'prepare 3 points
Dim oPoint1 As Point
Set oPoint1 = oTG.CreatePoint(0, 10, 0.1)
Dim oPoint2 As Point
Set oPoint2 = oTG.CreatePoint(0, 10.1, 0.2)
Dim oPoint3 As Point
Set oPoint3 = oTG.CreatePoint(0, 10.2, 0.4)
Dim oCompDef As PartComponentDefinition
Set oCompDef = ThisApplication.ActiveDocument.ComponentDefinition
'create the sphere
Dim oSphere As RevolveFeature
Set oSphere = CreateSphere(oCompDef, oPoint1, oPoint2, oPoint3)
End Sub
Public Function CreateSphere(PartCompDef As PartComponentDefinition, Pnt1 As Point, Pnt2 As Point, Pnt3 As Point) As RevolveFeature
Dim oTG As TransientGeometry
Set oTG = ThisApplication.TransientGeometry
' Calculate the normal of the plane defined by the three points.
Dim oVec1 As UnitVector
Set oVec1 = oTG.CreateUnitVector(Pnt2.X - Pnt1.X, Pnt2.Y - Pnt1.Y, Pnt2.Z - Pnt1.Z)
Dim oVec2 As UnitVector
Set oVec2 = oTG.CreateUnitVector(Pnt3.X - Pnt1.X, Pnt3.Y - Pnt1.Y, Pnt3.Z - Pnt1.Z)
If oVec1.IsParallelTo(oVec2) Then
MsgBox "The three points are collinear"
Exit Function
End If
Dim oNormalVec As UnitVector
Set oNormalVec = oVec1.CrossProduct(oVec2)
' Use vector one as the X axis of the plane, but calculate
' a new Y axis.
Set oVec2 = oNormalVec.CrossProduct(oVec1)
' Create a fixed work plane and make it invisible.
Dim oWP As WorkPlane
Set oWP = PartCompDef.WorkPlanes.AddFixed(Pnt1, oVec1, oVec2)
oWP.Visible = False
' Create a sketch.
Dim oSketch As PlanarSketch
Set oSketch = PartCompDef.Sketches.Add(oWP)
' Create an arc through the three input points.
Dim oArc As SketchArc
Set oArc = oSketch.SketchArcs.AddByThreePoints(oSketch.ModelToSketchSpace(Pnt1), _
oSketch.ModelToSketchSpace(Pnt2), oSketch.ModelToSketchSpace(Pnt3))
Call oSketch.GeometricConstraints.AddGround(oArc.CenterSketchPoint)
Call oSketch.GeometricConstraints.AddGround(oArc.StartSketchPoint)
' Calculate the required position of the end point to get a 180 degree sweep.
Dim dEndAngle As Double
dEndAngle = oArc.StartAngle + Val("3.1415926535897932384626433832795")
Dim oNewPoint As Point2d
Set oNewPoint = oTG.CreatePoint2d(oArc.Radius * Cos(dEndAngle) + oArc.CenterSketchPoint.Geometry.X, _
oArc.Radius * Sin(dEndAngle) + oArc.CenterSketchPoint.Geometry.Y)
' Move the point.
oArc.EndSketchPoint.MoveTo oNewPoint
' Connect the start and end points with a line.
Dim oLine As SketchLine
Set oLine = oSketch.SketchLines.AddByTwoPoints(oArc.StartSketchPoint, oArc.EndSketchPoint)
' Create the revolved feature.
Dim oProfile As Profile
Set oProfile = oSketch.Profiles.AddForSolid
Set CreateSphere = PartCompDef.Features.RevolveFeatures.AddFull(oProfile, oLine, kJoinOperation)
End Function
