Script Example Analysis in Altium Designer

To provide further insight into the general aspects of the Scripting System, and the use of Delphi and X2 Object Models in scripts, two example projects are examined here from a functionality perspective – a board outline copier and a netlist generating script.

The Board Outline Copier and Netlister scripts are developed using the X2 Object Models to illustrate the capabilities of the scripting system in Altium Designer. These are existing scripts available in the example script collection as follows:

• The Board Outline Copier script utilizes the PCB Object Model to copy the existing PCB board outline as tracks and arcs onto a specified layer.
  See \Scripts\VB Scripts\CopyBoardOutlinePRJ.PRJSCR.
• The Netlist generator script utilizes the WorkSpace Manager Object Model to generate a netlist in the traditional Protel (v1 and v2) format.
  See \Scripts\Delphiscript Scripts\WSM\Protel Netlister\ScripterProtelNetlist.PRJSCR.

Board Outline Copier Project

The aim of the Board Outline Copier is to copy an existing board outline from the PCB document to a different layer in the same document.

The project uses a Script Form so the user can interact with a dialog to nominate the width of the board outline and select its target layer from a drop down menu. Using the PCB Object model and its PCB interfaces from the PCB API, the objects of a board outline are extracted and copied onto the specified layer.

► Script operation example

The main parts of the script are:

• A global PCB_Board (of IPCB_Board type) variable.
• A CopyBoardOutline subroutine that accepts AWidth and ALayer parameters.
• The bOkClick event handler which obtains the width and layer values from the script form and then executes the CopyBoardOutline subroutine.
• The bCancelClick event handler which closes the Board Outline script form (dialog).

Script functionality

The script uses a script Form that needs event handlers to capture the mouse clicks of individual controls such as the OK and Cancel buttons.

The OK button event handler is essentially as below:

Sub bOKClick(Sender)
  Dim Width
  Dim Layer

  Call StringToCoordUnit(eWidth.Text,Width,PCB_Board.DisplayUnit)
  Layer = String2Layer(cbLayers.Items(cbLayers.ItemIndex))
End Sub

Here, the form's mouse OnClick event handler (bOKClick) uses the the StringToCoordUnit function to obtain the entered width of the outline (the eWidth string from the TEdit box) in internal coordinate values. This function applies the current board units (PCB_Board.DisplayUnit property) to the Width variable.

Similarly, the selected layer string (the cbLayers item from the form TComboBox) is passed to the String2Layer function to obtain an enumerated value for the Layer variable. Note that in this project the form's TComboBox is pre-populated with an indexed list of layer strings (cbLayers.Items) – see the Form's CopyBoardOutlineForm.dfm file for the layer list.

The final step in the event handler (bOKClick) calls the CopyBoardOutline subroutine with the Width and Layer variables as passed parameters. The handler for the form's Cancel button (bCancelClick) simply closes the form.

IPCB_Board Interface

Within the OK button handler (bOKClick), the current board is obtained from the IPCB_Board interface through the IPCB_ServerInterface returned by the special PCBServer function. Here, the GetCurrentPCB function sets the current board reference to the PCB_Board variable.

The current board outline (IPC_BoardOutline) then is obtained throughout the script from the IPCB_Board interface BoardOutline property, using the above PCB_Board board reference.

The board outline needs to be initialized before proceeding with copying and creating a new outline. An outline – represented by the IPCB_BoardOutline interface – can be initialized using the interface's rebuilding/validation methods.

PCB_Board.BoardOutline.Invalidate
PCB_Board.BoardOutline.Rebuild
PCB_Board.BoardOutline.Validate

Outline Arc and Track segments

The IPCB_BoardOutline interface, representing the board outline, is inherited from the IPCB_Group interface. An IPCB_Group interface represents a group object that can store child objects. An example of an IPCB_Group interface is a polygon or a board outline, since these can store arcs and tracks as child objects.

A board outline object stores two different type of segments – ePolySegmentLine and ePolySegmentArc which represent a track or arc object respectively. The number of segments is determined by the PointCount property from the IPCB_BoardOutline interface, which extracts each outline vertex to the I variable for the For-To-Next loop.

Each segment of the obtained board outline is checked for tracks and arcs with the If PCB_Board.BoardOutline.Segments(I).Kind = ePolySegmentLine Then statement. If not a track segment (ePolySegmentLine) the Else part of the statement assumes the segment is an arc.

For each segment found and depending on the segment type, a new track or arc object is created using the PCBObjectFactory function.

PCBObjectFactory Function

Creating the new PCB objects employs the PCBObjectFactory function directly from the IPCB_ServerInterface interface.

'Create new Track object
PCBServer.PCBObjectFactory(eTrackObject, eNoDimension, eCreate_Default)

'Create new Arc object
PCBServer.PCBObjectFactory(eArcObject, eNoDimension, eCreate_Default)

The PCBObjectFactory function parameters set the object type (Track, Arc, Via etc), the dimension kind (Linear, Radial etc) and the object creation mode (to a local default or global preferences).

After each track or arc object is created by the PCBObjectFactory procedure, its properties are instantiated by the track/arc statements that follow.

The Track and Arc properties are represented by their respective interfaces, IPCB_Track and IPCB_Arc, where the relevant properties are implemented by the script. For example, the new track coordinates are obtained from the source outline segment vertices, where Track.X1 and Track.Y1 represent the track's initial coordinates and the X2 and Y2 properties are its final coordinates.

Track.X1     = PCB_Board.BoardOutline.Segments(I).vx
Track.Y1     = PCB_Board.BoardOutline.Segments(I).vy
Track.X2     = PCB_Board.BoardOutline.Segments(J).vx
Track.Y2     = PCB_Board.BoardOutline.Segments(J).vy
Track.Layer  = ALayer
Track.Width  = AWidth

As can also be seen in the above code snippet, the track Layer and Width properties are simply defined by the passed values extracted from the user interface dialog – the Form's cbLayers and eWidth variables.

Once fully defined, the new objects are added to a specified layer of the PCB document with the PCB_Board.AddPCBObject(NewObject) statement, where NewObject here is Track or Arc.

PreProcess and PostProcess

When creating a PCB object, the PreProcess method from the IPCB_ServerInterface object interface needs to be first invoked to ready the PCB server. After the object creation, the PostPocess method (also from the IPCB_ServerInterface interface) is applied to inform the server that the object additions are complete.

The PreProcess and PostProcess methods keep the Undo system and other subsystems of the PCB editor up to date and in synchronization. Below is a representative code snippet with the PreProcess and PostProcess statements.

PCBServer.PreProcess
'Create PCB objects
PCBServer.PostProcess

When objects are added to a nominated layer that has not been displayed in the PCB document, the layer needs to be forced to be visible. This is handled by the PCB_Board.LayerIsDisplayed(ALayer) = True statement, where ALayer is the user selected layer.

Document Refresh

Lastly, the PCB document with its new board outline is refreshed by the PCB:Zoom command and its associated Action = Redraw parameters. The zoom command parameters are applied using the AddStringParameter procedure after the parameter buffer is first cleared with the ResetParameters method.

Netlister Project

The aim of this Netlister script project is to generate a standard Protel netlist (in either Version 1 or Version 2 formats) for an Altium Designer project containing schematics. A flat netlist of a schematic project is separated into two sections:

• Component designators and the information associated with each component,
• Net names and the information associated with each net name, along with pin connections (pins of a component).

► Script operation example

The API's WorkSpace Manager Object Model provides interfaces that represent the project and its constituents – the documents, the components and its pins, and the nets. The WorkSpace Manager is a system server coupled tightly with the Client module that deals with projects and their associated documents. It provides compiling, multi sheet design support, connectivity navigation tools, multi-channel support, multiple implementation documents, and so on. To retrieve the WorkSpace Manager interface, invoke the GetWorkspace function which yields the IWorkspace interface.

For the Netlister script the interfaces of interest are the IWorkSpace, IProject, IDocument, IComponent and INet interfaces.

Note that some of the interfaces, especially the design object interfaces, correspond to equivalent Schematic Object interfaces. This is because the logical documents in a project are schematic documents with connectivity information. In fact the Schematic Object model can be used instead of the WorkSpace Manager, but the latter provides the functionality to compile a project and extract documents from a project, as well as retrieving data from schematic objects.

The main parts of Netlister the script are:

• A global TargetFileName string variable. which is the file name of the netlist.
• A global Netlist TStringList collection object which is populated with the netlist data.
• The WriteComponent_Version1 and WriteComponent_Version2 procedures.
• The WriteNet_Version1 and WriteNet_Version2 procedures.
• A ConvertElectricToString function which converts a pin's electrical property to a string
• The GenerateNetlist procedure which manages the data generation and the filename, path and directory housekeeping tasks.

Script functionality

The two parameter-less procedures, GenerateProtelV1FormatNetlist and GenerateProtelV2FormatNetlist, will appear in the Select Item to Run dialog offering the choice of generating a Protel V1 format netlist or a Protel V2 format netlist. These procedures call the GenerateNetlist procedure with the netlist format choice (0 or 1) as a passed parameter.

Procedure GenerateProtelV1FormatNetlist;
Var
 Version : Integer;
Begin
 // Protel 1 Netlist format, pass 0
 GenerateNetlist(0);
End;

Procedure GenerateProtelV2FormatNetlist;
Var
 Version : Integer;
Begin
 // Protel 2 Netlist format, pass 1
 GenerateNetlist(1);
End;

GenerateNetList

The GenerateNetList procedure retrieves the workspace interface so that the project interface can be then extracted for the current project (IWorkspace.DM_FocusedProject).

The project needs to be compiled before nets can be extracted, as the compile process builds the connectivity information of the project. The project interface's DM_Compile method is applied (IProject.DM_Compile) as shown in the code snippet below. Note that recent versions of Altium Designer compile projects automatically, so this step is optional.

WS := GetWorkspace;
 If WS = Nil Then Exit;

Prj := WS.DM_FocusedProject;
 If Prj = Nil Then Exit;

// Compile the project to fetch the connectivity info for design.
 Prj.DM_Compile;

The component and net information is stored in the Netlist object of the TStringList type, which is used later to generate a formatted netlist text file. The TStringList object is a Delphi class which is available to use in scripts.

The Generate procedure is then called with passed parameters that define the current project path and filename, plus the netlist format version.

Generate

The Generate procedure obtains the project path as the target output path for the generated netlist file (from the passed DocumentPath parameter), determines the netlist file name (TargetFileName) and checks the flattened status of the project (IProject.DM_DocumentFlattened).

For all the schematic documents in a project, each document is then checked for nets and components with the WriteNets and WriteComponents procedures, and ultimately extracted to the Netlist object.

Write Nets and Components

A netlist is composed of component and net sections, so two procedures are required to write component data and net data separately.

Only nets with greater than two nodes will be written to a netlist and those with less are discarded. For each net, the net name is based on the Net's DM_CalculatedNetName method, which extracts the net names from the connectivity information of the compiled project.

Two code snippets for the Components and Nets sections of a netlist are shown below for Version 1 netlist format. Note that the component and net data are stored in the NetList object, which is a TStringList type. The generated netlist is composed of two sections; the component information section and the net information section.

Components section

In the WriteComponent procedure each component found from the Project is checked if it is an actual component, and then the physical designator, footprint and part type values are extracted. These are added to the Netlist object container (NetList.Add) to build the netlist itself.

If Component <> Nil Then
Begin
 NetList.Add('[');
 NetList.Add(Component.DM_PhysicalDesignator);
 NetList.Add(Component.DM_FootPrint);
 NetList.Add(Component.DM_PartType);
 NetList.Add('');
 NetList.Add('');
 NetList.Add('');
 NetList.Add(']');
End;

Nets section

For the Nets procedure, the NetName and the Designators are extracted if a net has two or more Pins (INet.DM_PinCount). The net and pin information plus formatting characters are added to the Netlist container to build the netlist. The below snippet is the net writing procedure for the version 1 netlist.

If Net.DM_PinCount >= 2 Then
Begin
 NetList.Add('(');
 NetList.Add(Net.DM_CalculatedNetName);
 For i := 0 To Net.DM_PinCount – 1 Do
 Begin
   Pin := Net.DM_Pins(i);
   PinDsgn := Pin.DM_PhysicalPartDesignator;
   PinNo := Pin.DM_PinNumber;
   NetList.Add(PinDsgn + '-' + PinNo);
 End;
 NetList.Add(')');
End;

Note that the more verbose netlist format, Protel v2, includes the electrical properties for net pins (In, Out, Passive, HiZ etc).

The net writing procedure for the version 2 format (WriteNet_Version2) therefore interrogates each net pin's electrical property (INet.DM_Electical), which is then converted by the called ConvertElectricToString procedure – essentially a string conversion lookup table. These are then added to a local string variable (ElectricalString), which is in turn added to the Netlist container object.

Create Netlist file

Finally with the Netlist container object fully populated with the project component and net information, in the chosen format, the Generate prodedure writes the Netlist data to a file (TStringList.SaveToFile). The file path and name are defined by the TargetFileName string variable, as determined in the Generate procedure.