Altium脚本开发 Y分形天线
用Altium Designer脚本实现Y分形的平面天线
本文介绍了使用Altium Designer脚本程序生成Y型天线的过程，在窗体中线宽、迭代次数、边框长度可以直接设置（可以设置为10mm X 10mm，也可以设置为100mm X 100mm）。
Y分形天线用户界面由一个窗体、1个TImage控件、3个TLable控件、3个TEdit控件、一个TButton控件构成，
窗体步骤如下:
- 新建一个VB Script Form文件，保存脚本文件，将文件命名为Y分形天线设计。
- 将窗体的Caption属性改为“Y分形天线设计”。
- 在窗体中添加1个TImage控件、3个TLable控件、3个TEdit控件、一个TButton控件。
- 在TImage控件中加入图片，将3个TLable控件的Caption分别改为“边长(mm)：”、“线宽(mm)：”、“迭代次数：”。将3个TEdit控件的Text属性分别改为“100”、“2”、“4”，将TButton控件的Caption属性改为“生成”。
窗体如下图所示
图元分析：
Y分形天线的基本结构如下所示。基本的图元由主干M、左分支L、右分支R构成，再一次迭代以左分支的终点和右分支的终点上增加一个基本Y型图元。
Y分形天线的基本图元为Y型，上下左右四个方向都向前生长Y型的分支，向上Y型每次迭代主干M都是垂直向上，左、下、右Y型分支和上Y型分支相同，可由上Y型生成之后将坐标依次变换一下，得到左、下、右Y型分支，生成的图像如下图所示，源码附后。
源程序：
PI = 3.1415926
'启动PCB服务器 Sub Start_PCBServer() Call Client.StartServer("PCB") PcbFileName = "PCB1.PcbDoc" Set Document = Client.OpenDocument("PCB", PcbFileName) If Not (Document Is Nothing) Then 'Add this schematic sheet in the newly created PCB project in DXP. Set Workspace = GetWorkspace
If Not (Workspace Is Nothing) Then Workspace.DM_FocusedProject.DM_AddSourceDocument(Document.FileName) End If Client.ShowDocument(Document) End If End Sub
'在PCB的顶层画直线函数 'Draw Line Function Sub Paint_Line(x1,y1,x2,y2) Dim Board Dim Track Set Board = PCBServer.GetCurrentPCBBoard Track = PCBServer.PCBObjectFactory(eTrackObject,eNoDimension,eCreate_Default) Track.X1 = MMsToCoord(CLng(x1)+Board.GetState_XOrigin/10000*0.0254) Track.Y1 = MMsToCoord(CLng(y1)+Board.GetState_XOrigin/10000*0.0254) Track.X2 = MMsToCoord(CLng(x2)+Board.GetState_XOrigin/10000*0.0254) Track.Y2 = MMsToCoord(CLng(y2)+Board.GetState_XOrigin/10000*0.0254) Track.Layer = eTopLayer Track.Width = MMsToCoord(Round(Edit2.Text)) Board.AddPCBObject(Track) Board.LayerIsDisplayed(ALayer) = True End Sub
'画矩形框函数，这里是画PCB的外框 'Draw rectangle Function Sub Paint_Rectangle(x1,y1,x2,y2) call Paint_Line(x1,y1,x2,y1) call Paint_Line(x1,y1,x1,y2) call Paint_Line(x1,y2,x2,y2) call Paint_Line(x2,y1,x2,y2) End Sub
'刷新视图 Sub Action_Redraw() Call Client.SendMessage("PCB:Zoom","Action=Redraw", 255, Client.CurrentView) Call Client.SendMessage("PCB:Zoom","Action=All", 255, Client.CurrentView) End Sub
'设置相对坐标原点函数 'SetState_Origin Sub Set_Origin() Set Board = PCBServer.GetCurrentPCBBoard Board.SetState_YOrigin(80000000) Board.SetState_XOrigin(80000000) End Sub
'将矩形框作为PCB的外框 Sub Board_Shape() Call AddStringParameter("Scope", "All") RunProcess("PCB:Select") Call AddStringParameter("Mode", "BOARDOUTLINE_FROM_SEL_PRIMS") RunProcess("PCB:PlaceBoardOutline") Call AddStringParameter("Size", "2.500MM") RunProcess("PCB:SnapGrid") Call AddStringParameter("MeasurementUnit", "Toggle") RunProcess("PCB:DocumentPreferences") End Sub
'控件响应函数 Sub Button1Click(Sender) call Start_PCBServer() 'Start PCBServer Board_chang = Round(Edit1.Text) Iter_Num = Round(Edit3.Text) 'Get Iteration Number call Set_Origin() 'Set Shape Relative to the origin call Paint_Rectangle(-Board_chang/2,-Board_chang/2,Board_chang/2,Board_chang/2) Call Board_Shape() Call Y_Shape(0,0,30,4) Action_Redraw() Close End Sub
'关键画基本图元的函数 Sub Y_Shape(x,y,L,Iter_Num) a = PI/4 L1=L*2/3 If Iter_Num=0 Then 'If Iter_Num = 0 Call Y_Xing(x,y,L,L1,a) 'Draw Y Else Call Y_Xing(x,y,L,L1,a) 'Draw Y Call Y_Shape(x-L1*sin(a),y+L+L1*cos(a),L/2,Iter_Num-1) Call Y_Shape(x+L1*sin(a),y+L+L1*cos(a),L/2,Iter_Num-1) End If End Sub Sub Y_Xing(x,y,L,L1,a) Call Paint_Line(x,y,x,y+L) 'Draw Vertical Line Call Paint_Line(x,y+L,x-L1*sin(a),y+L+L1*cos(a)) 'Draw Left Diagonal Line Call Paint_Line(x,y+L,x+L1*sin(a),y+L+L1*cos(a)) 'Draw Right Diagonal Line 'Draw Left Y Call Paint_Line(-y,x,-(y+L),x) 'Draw Vertical Line Call Paint_Line(-(y+L),x,-(y+L+L1*cos(a)),x-L1*sin(a)) 'Draw Left Diagonal Line Call Paint_Line(-(y+L),x,-(y+L+L1*cos(a)),x+L1*sin(a)) 'Draw Right Diagonal Line 'DraW Down Y Call Paint_Line(x,-y,x,-(y+L)) 'Draw Vertical Line Call Paint_Line(x,-(y+L),x-L1*sin(a),-(y+L+L1*cos(a))) 'Draw Left Diagonal Line Call Paint_Line(x,-(y+L),x+L1*sin(a),-(y+L+L1*cos(a))) 'Draw Right Diagonal Line 'Draw Right Y Call Paint_Line(y,-x,y+L,-x) 'Draw Vertical Line Call Paint_Line(y+L,-x,y+L+L1*cos(a),-(x-L1*sin(a))) 'Draw Left Diagonal Line Call Paint_Line(y+L,-x,y+L+L1*cos(a),-(x+L1*sin(a))) 'Draw Right Diagonal Line End Sub
代码：
https://files.cnblogs.com/files/xiongshuang/Y%E5%88%86%E5%BD%A2%E5%A4%A9%E7%BA%BF%E7%9A%84%E8%AE%BE%E8%AE%A1.zip
参考资料：
[1]付丽华.一种基于Y分形的平面微带天线设计与优化[EB/OL].http://www.elecfans.com/soft/69/2019/20190412905256.html,2019.
[2] Altium Limited.PCB API Design Objects Interfaces[EB/OL].https://techdocs.altium.com/display/SCRT/PCB+API+Design+Objects+Interfaces,2017-9-13.
