Move the designator where you click the mouse.

Click on the component and then click at the location where the designator is to be and it moves the designator to that location.


Sub ClickMoveDesPos

Dim Board
Dim Comp
Set Board = PCBServer.GetCurrentPCBBoard
If Board is Nothing Then Exit Sub

While Board.ChooseLocation(x,y, "Click Via To Change") = True
  Set Comp = Board.GetObjectAtXYAskUserIfAmbiguous(x,y,MkSet(_
  eComponentObject),AllLayers,eEditAction_Focus)

  If Not(Comp is Nothing) Then
     Call Board.ChooseLocation(x,y, "Select Location")
     Call PCBServer.PreProcess
     Call PCBServer.SendMessageToRobots(Comp.I_ObjectAddress,_
     c_Broadcast, PCBM_BeginModify, c_NoEventData)

           Comp.ChangeNameAutoposition = eAutoPos_Manual
           Comp.Name.XLocation = x
           Comp.Name.YLocation = y

     Call PCBServer.SendMessageToRobots(Comp.I_ObjectAddress,_
     c_Broadcast, PCBM_EndModify , c_NoEventData)
     Call PCBServer.PostProcess
  End If
Wend


ResetParameters
Call AddStringParameter("Action", "Redraw")
RunProcess("PCB:Zoom")
End Sub

www.tdpcb.com

Change the AutoPosition of the designator

Click on a component and the designator autoposition will cycle around the 8 positions each time you click on the component.


Sub CycleDesPos

Dim Board
Dim Comp
Dim I

Dim eAutoArray
'                 0                               1                                 2
'eAutoPos_TopLeft,eAutoPos_CenterLeft,eAutoPos_BottomLeft,
'                  3                                     4                                    5
'eAutoPos_BottomCenter,eAutoPos_BottomRight,eAutoPos_CenterRight,
'                  6                                7
'eAutoPos_TopRight,eAutoPos_TopCenter
eAutoArray = Array(1,2,3,6,9,8,7,4)

Set Board = PCBServer.GetCurrentPCBBoard
If Board is Nothing Then Exit Sub

Call PCBServer.PreProcess
While Board.ChooseLocation(x,y, "Click Via To Change") = True
  Set Comp = Board.GetObjectAtXYAskUserIfAmbiguous(x,y,MkSet(_
  eComponentObject),AllLayers,eEditAction_Focus)
  I= -1

   If Not(Comp is Nothing) Then

     'Look for the current setting of the autoposition
     For J = 0 to 7
      If  Comp.NameAutoposition = eAutoArray(J) Then
          I = J + 1
          'Set the array to begin again at eAutoPos_TopLeft
          If J = 7 Then
             I = 0
          End If
      End If
     Next
     'Autoposition is either manual or centercenter
     If I = -1 Then
         I = 0
     End If

     Call PCBServer.SendMessageToRobots(Comp.I_ObjectAddress,_
     c_Broadcast, PCBM_BeginModify, c_NoEventData)

           Comp.ChangeNameAutoposition = eAutoArray(I)

     Call PCBServer.SendMessageToRobots(Comp.I_ObjectAddress,_
     c_Broadcast, PCBM_EndModify , c_NoEventData)

  End If

Wend

Call PCBServer.PostProcess

ResetParameters
Call AddStringParameter("Action", "Redraw")
RunProcess("PCB:Zoom")

End Sub

www.tdpcb.com

Clone a vias net to another via

This required a few months of help from Altium, they didn't solve the problem of not being able to add a net to an exsisting via with "not net". But Altium did put me on the right path, the via with "no net" has to be added to the net object, not adding the net to the via (which works if the via already has a net). So this fixes the previous scripts inability to add a net to a via with "no net".

Sub CloneViaNetOBJ
Dim Board
Dim ObjVia
Dim Borg

Set Board = PCBServer.GetCurrentPCBBoard
If Board is Nothing Then Exit Sub
Set ObjVia = Board.GetObjectAtCursor(MkSet(eViaObject)_
,AllLayers,"Select Via to Clone")

NetIterator = Board.BoardIterator_Create
NetIterator.AddFilter_ObjectSet(MkSet(eNetObject))
NetIterator.AddFilter_LayerSet(AllLayers)
NetIterator.AddFilter_Method(eProcessAll)
Set NetFound = NetIterator.FirstPCBObject

While FoundIt = 0 AND Not (NetFound Is Nothing)
      If NetFound.Name = ObjVia.Net.Name Then
         FoundIt = 1
      else
          Set NetFound = NetIterator.NextPCBObject
      End If
Wend

Call PCBServer.PreProcess
While Board.ChooseLocation(x,y, "Click Via To Change") = True
  Set Borg = Board.GetObjectAtXYAskUserIfAmbiguous(x,y,MkSet(_
  eViaObject),AllLayers,eEditAction_Focus)

  If Not(Borg is Nothing) Then
     Call PCBServer.SendMessageToRobots(Borg.I_ObjectAddress,_
     c_Broadcast, PCBM_BeginModify, c_NoEventData)
     'Need to add the via to the net group, not the other way around!
        NetFound.AddPCBObject(borg)
     Call PCBServer.SendMessageToRobots(Borg.I_ObjectAddress,_
     c_Broadcast, PCBM_EndModify , c_NoEventData)
  End If
Wend

Call Board.CleanNet(NetFound) 'How to clean all nets?
Call PCBServer.PostProcess
ResetParameters
Board.BoardIterator_Destroy(NetIterator)
Call AddStringParameter("Action", "Redraw")
RunProcess("PCB:Zoom")
End Sub

Click the via with the net that you want

Then click the ones you want to change.

www.tdpcb.com