Using the PCB API

Old Content - visit

Parent page: Using the Altium Designer API

Using the PCB Editor Interfaces

The PCB API allows a programmer to fetch or modify PCB objects and their attributes from a PCB document. The objects shown on a document are stored in its corresponding design database.

The PCB interfaces exposed by the PCB editor refer to opened PCB documents and the objects on them. The PCB API derives its functionality from the base Altium Designer API which contains interface objects declarations and type declarations. An interface is a means of access to an object in memory. To have access to the PCB server and massage certain PCB design objects, you need to invoke the PCBServer function which extracts the IPCB_ServerInterface interface.

This is the main interface and contains many interfaces within it. With this interface, you can proceed further by iterating for certain PCB objects.

The IPCB_ServerInterface and IPCB_Board interfaces are the main interfaces that you will be dealing with when you are extracting data from a PCB or PCB Library document. Below is the simplified PCB object interface hierarchy.

Simplified PCB Objects Interfaces hierarchy


PCBServer function

When you need to work with PCB design objects in Altium Designer, the starting point is to invoke the PCBServer function and with the IPCB_ServerInterface interface, you can extract the all other derived PCB interfaces that are exposed in the IPCB_ServerInterface interface. For example, to get an access to the current PCB document open in Altium Designer, you would invoke the GetCurrentPCBBoard method from the IPCB_ServerInterface interface object.

  • The IPCB_ServerInterface interface is the main interface in the PCB API. To use PCB interfaces, you need to obtain the IPCB_ServerInterface object by invoking the PCBServer function. The IPCB_ServerInterface interface is the gateway to fetching other PCB objects.
  • The IPCB_Primitive interface is a generic interface used for all PCB design object interfaces.
  • The IPCB_Board interface points to an existing PCB document in Altium Designer.

GetCurrentPCBBoard example

TheServer := PCBServer.GetCurrentPCBBoard;
If TheServer = Nil Then Exit;
TheBoard := PCBBoard. GetCurrentPCBBoard
If TheBoard = Nil The Exit;
TheFileName := TheBoard. GetState_FileName;

For detailed information on PCB API, refer to the Technical Reference - PCB API document.

Invoking Properties and Methods of PCB Interfaces

For each PCB object interface, there will be methods and properties listed (not all interfaces will have both methods and properties listed, that is, some interfaces will only have methods).

A class method is a procedure or function that operates on a class rather than on specific instances of the class.

A property of an object interface is like a variable, you get or set a value in a property, but some properties are read only properties meaning they can only return values but cannot be set. A property is implemented by its Get and Set methods

For example, the IPCB_Component interface has a Height property and two associated methods GetState_Height and SetState_Height:

Function  GetState_Height : TCoord;
Procedure SetState_Height (Value : TCoord);
Property  Height : TCoord  Read GetState_Height  Write SetState_Height;

Another example is that the Selected property has two methods Function GetState_Selected : Boolean; and Procedure SetState_Selected (B : Boolean);

Object Properties example

PCBComponent.Selected := True                  //set the value
ASelected             := PCBComponent.Selected //get the value

The IPCB_Primitive is the base interface for all other PCB design object interfaces such as IPCB_Track and IPCB_Component.

For example the Selected property and its associated Function GetState_Selected : Boolean; and Procedure SetState_Selected (B : Boolean); methods declared in the IPCB_Primitive interface are inherited in the descendant interfaces such as IPCB_Component and IPCB_Pad interfaces.

This Selected property is not in the IPCB_Component, but you will notice that the IPCB_Component is inherited from IPCB_Primitive and this interface has a Selected property along with its associated methods (GetState function and SetState procedure).

If you can't find a method or a property in an object interface that you expect it to be in, the next step is to look into the base IPCB_Primitive interface — defines all the interfaces that are exposed and can be used to access most of the objects in PCB.

The PCB Database system

The database system is the heart of the PCB editor and this system stores all of the information about the PCB document. The objects in the database system are a direct representation of the objects on the PCB document.

The database system of the PCB editor stores primitive objects and group objects such as pads, vias, tracks, arcs, fills, text, components, nets, coordinates, dimensions, polygons, from tos, manual from-tos, classes, rules, violations and embedded objects. This primary database is a flat database which is composed of two different data structures.

The Primary Storage System has an array of linked lists. Each layer represents a linked list of PCB objects.

The first structure on the left of the figure above consists of separate singular linked lists of vias, components, nets, coordinates, dimensions, classes, rules, from-tos and connections. The second structure on the right of the figure above consists of an array of linked lists of the same kind of PCB objects. Each array exists separately for track, arc, fill, text string, pad and polygon objects. This second data structure is optimized for performance reasons.

The secondary database system is a spatial database. For each layer in the spatial database, there is a container which is a spatial or quad tree that can store any kind of PCB object. This secondary database is optimised for fast access of PCB objects. The type of database is chosen automatically depending on which specific PCB functions are being invoked.

The Secondary Storage System has spatial containers for each design layer.

PCB and Library documents

There are two types of documents in the PCB editor, the PCB document and the PCB Library document. Dealing with PCB documents is straightforward.

The concept of handling a PCB Library document is a bit more involved since each PCB footprint (a component with an undefined designator) occupies one PCB library document within a PCB library file. Note that you can only place tracks, arcs, fills, texts, pads and vias on a library document.

Loading PCB or PCB Library documents

There are other situations when you need to programmatically open a specific document. This is facilitated by using the Client object and invoking one of its methods such as Client.OpenDocument and Client.ShowDocument methods.

Opening a text document, you pass in the ‘Text’ string along with the full file name string. For PCB and PCB Library documents, the ‘PCB’ and ‘PCBLIB’ strings respectively need to be passed in along with the full file name string. For Schematic and Schematic Library documents, the ‘SCH’ and ‘SCHLIB’ strings respectively need to be passed in along with the full file name string.

Since the parameters for some of the functions are null terminated types and often the strings are TPCBString types, you will need to typecast these strings as PChar type.
In the code snippet below, the IServerDocument.DM_FullPath method returns a TPCBString, and this parameter is typecasted as a PChar in the Client.OpenDocument method.

Opening a Text Document using Client.OpenDocument method

    ReportDocument : IServerDocument;
    ReportDocument  := Client.OpenDocument('Text',PChar(FileName));
    If ReportDocument <> Nil Then

See the script examples in the Scripts\DelphiScript Scripts\PCB\ folder.

Creating PCB or PCB Library documents

There are situations when you need to programmatically create a blank document, this is facilitated by using the CreateNewDocumentFromDocumentKind function. For example, to creating a text document pass in the ‘Text’ string.

CreateNewDocumentFromDocumentKind code example

    Document : IServerDocument;
    Kind     : TPCBString;
    //The available Kinds are PCB, PCBLib, SCH, SchLib, TEXT,...
    Kind := ‘PCB’;
    Document := CreateNewDocumentFromDocumentKind(Kind);

Create a blank PCB and add to the current Project code example

    Doc     : IServerDocument;
    Project : IProject;
    Path    : TPCBString;
    If PCBServer = Nil then Exit;
    Project := GetWorkSpace.DM_FocusedProject;
    If Project <> Nil Then
        Path := GetWorkSpace.Dm_CreateNewDocument(‘PCB’);
        Doc :=  Client.OpenDocument(Pchar(‘PCB’,PChar(Path));
    // do what you want with the new document.

See the script examples in the Scripts\DelphiScript Scripts\PCB\ folder.

Checking the type of PCB documents

You can use the GetCurrentPCBBoard function from the PCBServer object and with the interface object (IPCB_Board) you can invoke the IsLibrary method to check whether the current PCB document is a PCB Library type document or not.

IsLibrary method example

// check if a PCB Library document exists.
Board := PCBServer.GetCurrentPCBBoard;
If Board = Nil Then Exit;
If Not (Board.IsLibrary) Then
    ShowMessage('This is not a PCBLIB document');

Document Kind method code example

If StrPas(Client.CurrentView.Kind) <> UpperCase('PCBLib') Then Exit;

This code snippet uses the Client.CurrentView.Kind method to find out the current document’s type.

Setting a Document Dirty

There are situations when you need to programmatically set a document dirty so when you close Altium Designer, it prompts you to save this document. This is facilitated by setting the ServerDocument.Modified to true.

Document’s Modified Property code example

    AView           : IServerDocumentView;
    AServerDocument : IServerDocument;
    // grab the current document view.
    AView := Client.GetCurrentView;
    //grab the owner server document.
    AServerDocument := AView.OwnerDocument;
    // set the document dirty.
    AServerDocument.Modified := True;

See the script examples in the Scripts\DelphiScript Scripts\PCB\ folder.

Refreshing a document programmatically

When you place or modify objects on a PCB document, you often need to do a refresh of the document. An example below demonstrates one way to update the document.

Refresh a PCB document in a script

// Refresh PCB screen
Client.SendMessage('PCB:Zoom', 'Action=Redraw' , 255, Client.CurrentView);

PCB Objects

The PCB design objects are stored inside the database of the currently active PCB document in the PCB editor. Each design object has a handle. These handles allow you to access and change the object’s properties.

A PCB object is either a primitive or a group object. A primitive is a basic PCB object which could be one of the following: tracks, pads, fills, vias and so on.

A group object can be a component, dimension, co-ordinate, polygon or a net object and each group object is composed of primitives. Each group object also has its own small database that stores primitives. A component is a group object and is therefore composed of primitives.

Accessing PCB Objects

Iterators provide a way of accessing the elements of an aggregate object sequentially without exposing its underlying representation.  With regards to the PCB editor’s database system, the use of iterators provides a compact method of accessing PCB objects without creating a mirror database across the API.

The main function of an iterator is to traverse through the database to fetch certain PCB objects by traversing the database inside the PCB editor from the outside.

There are four types of iterators:

  • Board iterators
  • Spatial iterators
  • Group iterators
  • Library iterators

Board iterators are used to conduct global searches, while spatial iterators are used to conduct restricted searches within a defined boundary. Group iterators are used to conduct searches for child objects within a group object such as a component and library iterators are used to conduct a search within a PCB library document within a PCB library.

Board Iterator example in a Server project

    Board     : IPCB_Board;
    Pad       : IPCB_Primitive;
    Iterator  : IPCB_BoardIterator;
    // retrieve the current board's handle
    Board     := PCBServer.GetCurrentPCBBoard;
    If Board = Nil Then Exit;
    // retrieve the iterator handle
    Iterator        := Board.BoardIterator_Create;
    // search and count pads
    Pad := Iterator.FirstPCBObject;
    While (Pad <> Nil) Do
        // do what you want with the fetched pad
        Pad := Iterator.NextPCBObject;

See the script examples in the Scripts\DelphiScript Scripts\PCB\ folder.

Creation of a New PCB Object

PCB objects created using the PCB API will need to follow a few simple steps to ensure that the database system of the PCB editor will successfully register these objects. An example is shown to illustrate the steps involved in creating a new PCB object. The code demonstrates the paramount role of the creation of a board object before any PCB objects are to be created, destroyed or modified. If there is no board object, the database system inside the PCB editor will not be updated and the current PCB document will not be affected either.

This code snippet demonstrates the registration and placement of a Via object (which is one of the PCB editor’s design objects) onto a PCB document. This example will also illustrate the concept of object handles.

PCBObjectFactory method example

Procedure CreateAViaObject;
    Board : IPCB_Board;
    Via   : IPCB_Via;
    Board := PCBServer.GetCurrentPCBBoard;
    If Board = Nil Then Exit;
    (* Create a Via object*)
    Via := PCBServer.PCBObjectFactory(eViaObject) As IPCB_Via;
    Via.X         := MilsToCoord(1000);
    Via.Y         := MilsToCoord(1000);
    Via.Size      := MilsToCoord(50);
    Via.HoleSize  := MilsToCoord(20);
    Via.LowLayer  := eTopLayer;
    Via.HighLayer := eBottomLayer;

How the above code works

The board is fetched which is a representation of an actual PCB document and then a PCBObjectFactory method is called from the IPCB_ServerInterface (representing the PCB editor) and a copy of the Via object is created.
You can change the attributes of this new object and then you can add this new object in the PCB database.

To ensure that the PCB editor’s database system registers this new via object, we need to add this via object into the board object, by using the board object’s AddPCBObject method the via object parameter. Once this method has been invoked, this new Via object is now a valid object on the current PCB document.

To actually remove objects from the database, invoke the Board.RemovePCBObject method and pass in the parameter of a reference to an actual PCB object.

See the script examples in the Scripts\DelphiScript Scripts\PCB\ folder.

Creating/deleting Objects and updating the PCB Editor’s Undo system

The CreateAVia addon above example does not refresh the Undo system in the PCB editor, to do this, you will need to employ the SendMessageToRobots method to send messages into the PCB editor server to inform the datastructure that new PCB objects have been added to the PCB document.

One Undo sequence

The sequence is as follows for a one big undo operation:

  1. Invoke the PCBServer.PreProcess method which initializes the robots in the PCB server once
  2. For each new object added, send a PCBM_BoardRegisteration message
  3. Invoke the PCBServer.PostProcess method which cleans up the robots in the PCB server once

Multiple Undos sequence

The sequence is as follows for multiple step undo operation, i.e. for each PCB creation, do the four steps:

  1. Invoke the PreProcess method which initializes the Robots in the PCB server.
  2. Add a new object.
  3. Send a PCBM_BoardRegisteration message.
  4. Invoke the PostProcess method which cleans up the robots in the PCB server.

Repeat Steps 1-4 for each PCB object creation.

Adding two Fill Objects and refreshing the Undo system in PCB Editor

    Board := PCBServer.GetCurrentPCBBoard;
    If Board = Nil Then Exit;
    Fill            := PCBServer.PCBObjectFactory(eFillObject) as IPCB_Fill;
    Fill.X1Location := MilsToCoord(4000);
    Fill.Y1Location := MilsToCoord(4000);
    Fill.X2Location := MilsToCoord(4400);
    Fill.Y2Location := MilsToCoord(4400);
    Fill.Rotation   := 0;
    Fill.Layer      := eTopLayer;
    Fill2     := PCBServer.PCBObjectFactory(eFillObject);
    Fill.X1Location := MilsToCoord(5000);
    Fill.Y1Location := MilsToCoord(3000);
    Fill.X2Location := MilsToCoord(5500);
    Fill.Y2Location := MilsToCoord(4000);
    Fill.Rotation   := 45;
    Fill.Layer      := eTopLayer;

See the script examples in the Scripts\DelphiScript Scripts\PCB\ folder.

Removal of Objects code example

        Track := Iterator.FirstPCBObject As IPCB_Track;
        While Track <> Nil Do
            OldTrack := Track;
            Track := Iterator.NextPCBObject As IPCB_Track;

See the script examples in the Scripts\DelphiScript Scripts\PCB\ folder.

Modifying PCB Design Objects in code

To modify PCB objects on a current PCB document, you will need to invoke certain methods in a certain order to ensure the Undo/Redo system is up to date when a PCB object’s attributes have been modified programmatically.

The Modification of a PCB Object Sequence is as follows:

  1. Invoke the PreProcess method and Initialize the robots in the PCB server
  2. Send a PCBM_BeginModify message
  3. Modify the PCB object
  4. Send a PCBM_EndModify message
  5. Invoke the PostProcess method to clean up the robots in the PCB server

Changing PCB Object’s Attributes example

Procedure ModifyObject;
    PCBServer.SendMessageToRobots(Fill.I_ObjectAddress, c_Broadcast, PCBM_BeginModify ,c_NoEventData);
    Fill.Layer := eBottomLayer;
    PCBServer.SendMessageToRobots(Fill.I_ObjectAddress, c_Broadcast,
 PCBM_EndModify , c_NoEventData);
    //Clean up the robots in the PCB editor.

When you change the properties of a PCB object on a PCB document, it is necessary to employ the PCBServer.SendMessageToRobots function to update the various subsystems of the PCB system such as the Undo/Redo system and setting the document as dirty so the document can be saved. Learn more about the SendMessageToRobots method of the IPCB_ServerInterface in the Technical Reference - PCB API document.

Remember, the PCB API only can be used to work on a currently open PCB document in Altium Designer. If you need to fetch specific PCB documents, you will need the Client object’s OpenDocument and ShowDocument methods to open and display a document.

Procedure OpenAndShowPCBDocument(AFileName : String);
    Document : IServerDocument;
    If Client = Nil Then Exit;
    Document := Client.OpenDocument('PCB',AFileName,False);
    If Document <> Nil Then

See the script examples in the Scripts\DelphiScript Scripts\Sch\ folder.

PCB interactive feedback using the Mouse

To monitor the mouse movement and clicks from your script, the IPCB_Board document interface has several interactive feedback methods:

  • GetObjectAtCursor
  • GetObjectAtXYAskUserIfAmbiguous
  • ChooseRectangleByCorners
  • ChooseLocation

The GetObjectAtCursor returns you the interface of an object where the PCB system has detected that this object has been clicked upon.

The GetObjectAtXYAskUserIfAmbiguous method does the same function as the GetObejctAtCursor except that if there are objects occupying the same region on the PCB document, then this method prompts you with a dialog with a list of objects to choose before returning you the object interface. You have the ability to control which objects can be detected and which layers can be detected and what type of editing action the user has been doing.

The ChooseRectangleByCorners method prompts you to choose the first corner and the final corner and then the X1,Y1, X2 and Y2 parameters are returned.

The ChooseLocation method prompts you to click on the PCB document and then the X1,Y1 coordinates of the mouse click are returned.

ChooseRectangleByCorners example in a Server project

    Board           : IPCB_Board;
    SpatialIterator : IPCB_SpatialIterator;
    X1,Y1,X2,Y2    : TCoord;
    ASetOfLayers   : TLayerSet;
    ASetOfObjects  : TObjectSet;
    Track          : IPCB_Track;
    TrackCount     : Integer;
    //Spatial iterator queries PCB data within X1,Y1,X2,Y2 constraints
    Board := PCBServer.GetCurrentPCBBoard;
    If Board = Nil Then Exit;
    TrackCount := 0;
    If Not (Board.ChooseRectangleByCorners('Please select the first corner',
                                           'Please select the final corner',
                                            X1,Y1,X2,Y2)) Then Exit;
    ASetOfLayers  := [eTopLayer,eBottomLayer];
    ASetOfObjects := [eTrackObject];
    SpatialIterator := Board.SpatialIterator_Create;
    Track := SpatialIterator.FirstPCBObject as IPCB_Track;
    While Track <> Nil Do
        TrackCount := TrackCount + 1;
        Track := SpatialIterator.NextPCBObject as IPCB_Track;

See the script examples in the Scripts\DelphiScript Scripts\PCB\ folder.

Activating the PCB API

There are situations when Altium Designer has no PCB documents opened, meaning that the PCB Editor has not been loaded and that the PCB API is not active.

You will then need to manually start the server to have access to the PCB API. Starting up the PCB server to activate the PCB API is done by invoking the Client.StartServer method.

Starting up the PCB server in Altium Designer

If PCBAPI_GetCurrentEditorWindow = 0 Then
    Board := PCBServer.GetCurrentPCBBoard;
    If Board = Nil Then Exit;

For more information, consult the PCB API Reference document within the Altium Designer API Reference.

You are reporting an issue with the following selected text and/or image within the active document: