How to add a primitive sphere in sketch vb.net
The API doesn't provide a simple equivalent to the primitive creation commands you see in the user interface. However, those commands just simplify the create of a sketch and feature so you can get the same results using the API. Sketches are 2D so it doesn't make sense to say you want to create a sphere in a sketch. However, we can create a semi-circle that we then use as input for a revolve feature to create a 3D sphere. The code below demonstrates this and ends up creating the same result as the sphere primitive command.
Public Sub CreateRevolution()
Dim partDoc As PartDocument
Set partDoc = ThisApplication.ActiveDocument
Dim partDef As PartComponentDefinition
Set partDef = partDoc.ComponentDefinition
Dim tg As TransientGeometry
Set tg = ThisApplication.TransientGeometry
' Create a new sketch on the X-Y base plane.
Dim sketch As PlanarSketch
Set sketch = partDef.Sketches.Add(partDef.WorkPlanes.Item(3))
' Draw a circle.
Dim radius As Double
radius = 5
Dim circ As SketchCircle
Set circ = sketch.SketchCircles.AddByCenterRadius(tg.CreatePoint2d(0, 0), radius)
' Draw a center line through the circle.
Dim lin As SketchLine
Set lin = sketch.SketchLines.AddByTwoPoints(tg.CreatePoint2d(-radius, 0), tg.CreatePoint2d(radius, 0))
lin.Centerline = True
' Constrain the line to circle.
Call sketch.GeometricConstraints.AddCoincident(circ.CenterSketchPoint, lin)
Call sketch.GeometricConstraints.AddCoincident(lin.StartSketchPoint, circ)
Call sketch.GeometricConstraints.AddCoincident(lin.EndSketchPoint, circ)
' Create a profile from the sketch.
Dim prof As Profile
Set prof = sketch.Profiles.AddForSolid()
' Two paths were created in the profile but we only need one (half of the circle)
' so delete one of the paths.
prof.Item(1).Delete
' Create a revolve feature.
Dim revolve As RevolveFeature
Set revolve = partDef.Features.RevolveFeatures.AddFull(prof, lin, kNewBodyOperation)
End Sub
In fact, I did something like that. I used arcs, and it works, but I want to move that revolve. I want to put it on a point (x,y,z). and planarskets is only 2Dpoints. There is a way to move the sphere after drawing? Thank you for your help. 
To move the sphere within the part, there are a couple of options, probably neither one being ideal. The first is to edit the skectch and change the position of the circle within the sketch. This is limiting because you can only move the circle on the sketch plane, not anywhere in space. It's also possible to redefine the sketch to change which plane it is based on but that's very practical either if you need to position the sphere anywhere in 3D space.
The second approach is to use the Move feature and move the spherical body that was created. This allows you to reposition it at any location and you can control that position afterword by using three parameters that are created with the feature to control the X, Y, and Z offset.
The typical approach to move things around is to create each thing as an individual part and then reposition them within an assembly.
Accepted solution
The problem is that you're using the Join operation when you create each sphere so it's joining that sphere to the existing sphere(s). You need to be creating a new body for each sphere. Here's a modified version of the previous program that does that. I've created a function where I can pass in the position and radius and it will create a sphere at that location. It also modifies the names of the parameters so it's easy to find which parameters control the position of which sphere. By changing the parameters you can reposition any sphere at any location after it's been created.
Public Sub CreateRevolutions()
Dim tg As TransientGeometry
Set tg = ThisApplication.TransientGeometry
Dim points(5) As Point
Set points(0) = tg.CreatePoint(4, 0, 0)
Set points(1) = tg.CreatePoint(0, -4, 0)
Set points(2) = tg.CreatePoint(0, 4, 0)
Set points(3) = tg.CreatePoint(4, 4, 0)
Set points(4) = tg.CreatePoint(-4, 4, 0)
Dim moves(5) As MoveFeature
Dim i As Integer
For i = 0 To 4
Set moves(i) = CreateSphere(1.5, points(i))
Next
End Sub
Public Function CreateSphere(Radius As Double, Position As Point) As MoveFeature
Dim partDoc As PartDocument
Set partDoc = ThisApplication.ActiveDocument
Dim partDef As PartComponentDefinition
Set partDef = partDoc.ComponentDefinition
Dim tg As TransientGeometry
Set tg = ThisApplication.TransientGeometry
' Create a new sketch on the X-Y base plane.
Dim sketch As PlanarSketch
Set sketch = partDef.Sketches.Add(partDef.WorkPlanes.Item(3))
' Draw a circle.
Dim circ As SketchCircle
Set circ = sketch.SketchCircles.AddByCenterRadius(tg.CreatePoint2d(0, 0), Radius)
' Draw a center line through the circle.
Dim lin As SketchLine
Set lin = sketch.SketchLines.AddByTwoPoints(tg.CreatePoint2d(-Radius, 0), tg.CreatePoint2d(Radius, 0))
lin.Centerline = True
' Constrain the line to circle.
Call sketch.GeometricConstraints.AddCoincident(circ.CenterSketchPoint, lin)
Call sketch.GeometricConstraints.AddCoincident(lin.StartSketchPoint, circ)
Call sketch.GeometricConstraints.AddCoincident(lin.EndSketchPoint, circ)
' Create a profile from the sketch.
Dim prof As Profile
Set prof = sketch.Profiles.AddForSolid()
' Two paths were created in the profile but we only need one (half of the circle)
' so delete one of the paths.
prof.Item(1).Delete
' Create a revolve feature.
Dim revolve As RevolveFeature
Set revolve = partDef.Features.RevolveFeatures.AddFull(prof, lin, kNewBodyOperation)
' Move it to the specified position.
Dim objColl As ObjectCollection
Set objColl = ThisApplication.TransientObjects.CreateObjectCollection
Call objColl.Add(revolve.Faces.Item(1).SurfaceBody)
Dim moveDef As MoveDefinition
Set moveDef = partDef.Features.MoveFeatures.CreateMoveDefinition(objColl)
Call moveDef.AddFreeDrag(Position.x, Position.y, Position.Z)
Set CreateSphere = partDef.Features.MoveFeatures.Add(moveDef)
' Rename the parameters to they're easily identified in the parameters dialog.
Dim freeDrag As FreeDragMoveOperation
Set freeDrag = CreateSphere.Definition.MoveOperation(1)
Dim name As String
name = CreateSphere.name & " X"
name = Replace(name, " ", "_")
freeDrag.XOffset.name = name
name = CreateSphere.name & " Y"
name = Replace(name, " ", "_")
freeDrag.YOffset.name = name
name = CreateSphere.name & " Z"
name = Replace(name, " ", "_")
freeDrag.ZOffset.name = name
End Function