Moving Designators

Rotate the designators in one of two ways and center them on the component so they are consistant.
Also detect if the component is on the top or the bottom.

Sub RotateDesignators
Dim Board
Dim Component
Dim CompDes
Dim I
Set Board = PCBServer.GetCurrentPCBBoard
If Board is Nothing Then Exit Sub

Iterator = Board.BoardIterator_Create
Iterator.AddFilter_ObjectSet(MkSet(eComponentObject))
Iterator.AddFilter_LayerSet(AllLayers)
Iterator.AddFilter_Method(eProcessAll)

Set CompDes = Iterator.FirstPCBObject
PCBServer.PreProcess
I = 0
While Not (CompDes Is Nothing)
  Call PCBServer.SendMessageToRobots(CompDes.Name.I_ObjectAddress,_
  c_Broadcast, PCBM_BeginModify, c_NoEventData)
  I = I + 1
  If CompDes.Layer = eTopLayer then           'Component is on the top
    Select Case CompDes.Rotation
    Case 0, 180, 360
       CompDes.Name.Rotation  = 0
    Case 90, 270
       CompDes.Name.Rotation  = 90
    Case Else
       CompDes.Name.Rotation  = 0
    End Select
 Else                                     'Component is on the bottom
   Select Case CompDes.Rotation
    Case 0, 180, 360
       CompDes.Name.Rotation  = 0
    Case 90, 270
       CompDes.Name.Rotation  = 270
    Case Else
       CompDes.Name.Rotation  = 0
    End Select
  End If

  CompDes.ChangeNameAutoposition = eAutoPos_CenterCenter
  Call PCBServer.SendMessageToRobots(CompDes.Name.I_ObjectAddress,_
c_Broadcast, PCBM_EndModify , c_NoEventData)

  Set CompDes = Iterator.NextPCBObject
Wend
'Uncomment next line if you want a message after it has finished.
'ShowMessage(I & " were found")
Board.BoardIterator_Destroy(Iterator)
Pcbserver.PostProcess
ResetParameters
Call AddStringParameter("Action", "Redraw")
RunProcess("PCB:Zoom")
End Sub

http://www.tdpcb.com/

File Name On Visible Layers

Create a sting from the PCB file name and place it on the board but leave off the ending (.pcbdoc). It will place a string on any routing and mechanical layer that is currently enabled and is visible.


Sub AddFileName

Dim Board
Dim ASMSting
Dim Layer
Dim TmpString
Set Board = PCBServer.GetCurrentPCBBoard
If Board is Nothing Then Exit Sub
PCBServer.PreProcess

For Layer = eTopLayer to eMultiLayer
  If Board.LayerIsDisplayed(Layer) AND Board.LayerIsUsed(Layer) Then
   ASMString = PCBServer.PCBObjectFactory(eTextObject,_
eNoDimension, eCreate_Default)
  ASMString.XLocation = Board.XOrigin + MilsToCoord(500) '500 mils from origin in X
  ASMString.YLocation = Board.YOrigin - MilsToCoord(500) '-500 mils from origin in Y
  TmpString = Board.FileName
  'Get rid of the drive and folder portion of the FileName
  While Instr(TmpString, "\") <> 0
    TmpString = Right(TmpString, Len(TmpString)-Instr(TmpString, "\") ) 'removes the path
  Wend

  ASMString.Text = Left(TmpString, Instr(TmpString, ".") - 1 ) 'removes the extension
  ASMString.Size = MilsToCoord(100) 'Size of the string is 10
  ASMString.Layer = Layer

  Board.AddPCBObject(ASMString) ' Put this string on the Board
  Call PCBServer.SendMessageToRobots(ASMString.I_ObjectAddress, c_Broadcast,_

PCBM_BoardRegisteration, ASMString.I_ObjectAddress)

 End If

Next
Pcbserver.PostProcess
ResetParameters
Call AddStringParameter("Action", "Redraw")
RunProcess("PCB:Zoom")

End Sub
 

 
http://www.tdpcb.com/

Make A String

Create a sting of various heights and widths on the PCB.

Sub StringCreation

Dim Board
Dim ASMSting

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

PCBServer.PreProcess
For I = 1 to 10
  ' Create a String object
  ASMString = PCBServer.PCBObjectFactory(eTextObject, eNoDimension, eCreate_Default)
  ASMString.XLocation = Board.XOrigin + I*MilsToCoord(50)
  ASMString.YLocation = Board.YOrigin + I*MilsToCoord(100)
  ASMString.Layer = eMechanical7
  ASMString.Text = "This Is String #" & I & " with a height of " & (10*I) & " a width of " & I & "mils."
  ASMString.Width = MilsToCoord(I)
  ASMString.Size = MilsToCoord(10 * I)

  Call PCBServer.SendMessageToRobots(ASMString.I_ObjectAddress, c_Broadcast,_
  PCBM_BoardRegisteration, ASMString.I_ObjectAddress)

  'Put this string on the Board
  Board.AddPCBObject(ASMString)
Next

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

End Sub
 
 

 
 
http://www.tdpcb.com/

Create a Schematic pin in a library part

Places a pin in a schematic library part. Open a schematic library (or create a new one.)  Run script and in the current part a pin will be placed.

Sub PlacePin

Set CurrentLib = SchServer.GetCurrentSchDocument
If CurrentLib is Nothing Then Exit Sub
If CurrentLib.ObjectID <> eSchLib Then Exit Sub

Set SchComponent = SchServer.SchObjectFactory(eSchComponent, eCreate_Default)
'Set up parameters for the library component.
SchComponent.CurrentPartID = 1
SchComponent.DisplayMode = 0

'Create pin objects for the new library component.
P1 = SchServer.SchObjectFactory(ePin,eCreate_GlobalCopy)

If P1 is Nothing Then Exit Sub
'Define the pin parameters.
P1.Location = Point(MilsToCoord(250), MilsToCoord( -250 ))
P1.Orientation = eRotate180
P1.PinLength = MilsToCoord(250)
P1.Designator = "1"
P1.Name = "Pin Name"
P1.Electrical = Etype(4)  '4=Passive
P1.OwnerPartId = CurrentLib.CurrentSchComponent.CurrentPartID
P1.OwnerPartDisplayMode = CurrentLib.CurrentSchComponent.DisplayMode

SchComponent.AddSchObject(P1)
CurrentLib.RegisterSchObjectInContainer(P1)

'Send a system notification that a new component has been added to the library.
Call AddStringParameter("Action", "Redraw")
RunProcess("SCH:Zoom")

Call SchServer.RobotManager.SendMessage(nil, c_BroadCast, SCHM_PrimitiveRegistration,_ SCHComponent.I_ObjectAddress)

Set CurrentLib.CurrentSchComponent = SchComponent
'Refresh library.
CurrentLib.GraphicallyInvalidate

End Sub

============================
FYI - Electrical definitions for the pin type:
0=Input
1=I/O
2=Output
3=Open Collector
4=Passive
5=HiZ
6=Open Emitter
7=Power



http://www.tdpcb.com/

Is this a schematic file?

Checking if the active file is a schematic document.

Sub IsthisaSCHFile

Set CurrentFile = SchServer.GetCurrentSchDocument
If CurrentFile is Nothing Then
  ShowMessage ("This is not a SCH file!")
Else
  ShowMessage ("This is a SCH file!")
End If

End Sub

http://www.tdpcb.com/

Counting Pads

Learn to use an Iterator that creates a set of objects that meet a certain criteria. This will count the number of pads on the board.  Use the AddFilter's to include only the objects that you need.

Sub CountPads
Dim Board
Dim Pad
Dim PadNumber
Dim TotalObjects

Padnumber = 0
Set Board = PCBServer.GetCurrentPCBBoard
If Board is Nothing Then Exit Sub
Iterator = Board.BoardIterator_Create
Iterator.AddFilter_ObjectSet(MkSet(ePadObject))
Iterator.AddFilter_LayerSet(AllLayers)
Iterator.AddFilter_Method(eProcessAll)

Set Pad = Iterator.FirstPCBObject

While Not (Pad Is Nothing)
  PadNumber = PadNumber + 1
  Set Pad = Iterator.NextPCBObject
Wend

Board.BoardIterator_Destroy(Iterator)
ShowMessage(PadNumber & " Were Found")

End Sub



http://www.tdpcb.com/

Create a Via

Make a few Vias appear on a PCB with the reference being the Board Origin. (FYI learn to decipher TR0138 PCB API Reference.PDF that comes with Altium)


Sub ViaCreation
Dim Board
Dim Via
Set Board = PCBServer.GetCurrentPCBBoard
If Board is Nothing Then Exit Sub
PCBServer.PreProcess
For I = 1 to 10
  ' Create a Via object
  Via = PCBServer.PCBObjectFactory(eViaObject, eNoDimension, eCreate_Default)
  Via.X = MilsToCoord (I * 50) + Board.XOrigin
  Via.Y = MilsToCoord(I * 50) + Board.YOrigin
  Via.Size = MilsToCoord(35)
  Via.HoleSize = MilsToCoord(15)
  Via.LowLayer = eTopLayer
  Via.HighLayer = eBottomLayer

  ' Put this via in the Board object
  Board.AddPCBObject(Via)
  Call PCBServer.SendMessageToRobots(Board.I_ObjectAddress, c_Broadcast,_  PCBM_BoardRegisteration, Via.I_ObjectAddress)

Next

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

End Sub

These just makes the screen do a refresh
Call AddStringParameter("Action", "Redraw")
RunProcess("PCB:Zoom")

"Undo Stuff"
PreProcess and PostProcess and the Call PCBServer.SendMessageToRobots(Board.I_ObjectAddress, c_Broadcast, PCBM_BoardRegisteration, Via.I_ObjectAddress)
allow the "Undo" to work with what was just placed on the board, otherwise is may not know that they were added.

http://www.tdpcb.com/

Is this A PCB file?

Most of the scripts will be for the PCB editor, so I need to check and make sure when I run a script it's actully being run in a PCB file. Access the PCBServer to get things started.

Sub IsthisaPCBFile

Set Board = PCBServer.GetCurrentPCBBoard
If Board is Nothing Then
     ShowMessage ("This is not a PCB file!")
Else
     ShowMessage ("This is a PCB file!")
End I

End Sub
 
 
If a pcb file isn't active in Altium then 
 

Else if a PCB file is active

 
http://www.tdpcb.com/

Alitum Designer Script Notes Visual Basic (VB)

Just some running notes as I learn to write VB scripts for Altium.
Starting with the very basics.
In Altium Designer choose File, New, Script Files, VB Script Unit Paste this:

Sub ShowMessageBox

     ShowMessage ("Hello! It's " & Time )

End Sub

Run the Script (DXP, Run Script, Choose ShowMessageBox) and you get

http://www.tdpcb.com/