‌CATIA宏编译实例：创建并拉伸草图凸台

Language="VBSCRIPT"

Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument '定义当前文档集合

Set part1 = partDocument1.Part '定义Part文档对象

Set hybridBodies1 = part1.HybridBodies '定义混合图形集合

Set hybridBody1 = hybridBodies1.Item("几何图形集.1") '定义几何图形集对象

Set sketches1 = hybridBody1.HybridSketches '定义草图集合

Set originElements1 = part1.OriginElements '定义初始元素集合

Set reference1 = originElements1.PlaneXY '定义XY平面对象

Set sketch1 = sketches1.Add(reference1) '定义基于XY平面的草图对象

Dim arrayOfVariantOfDouble1(8) '定义数组来表示轴系的坐标，0-2为原点，3-5为轴1终点，6-8为轴2终点
arrayOfVariantOfDouble1(0) = 0.000000
arrayOfVariantOfDouble1(1) = 0.000000
arrayOfVariantOfDouble1(2) = 0.000000
arrayOfVariantOfDouble1(3) = 1.000000
arrayOfVariantOfDouble1(4) = 0.000000
arrayOfVariantOfDouble1(5) = 0.000000
arrayOfVariantOfDouble1(6) = 0.000000
arrayOfVariantOfDouble1(7) = 1.000000
arrayOfVariantOfDouble1(8) = 0.000000
sketch1.SetAbsoluteAxisData arrayOfVariantOfDouble1 '定义草图的轴

part1.InWorkObject = sketch1 '定义工作对象为草图

Set factory2D1 = sketch1.OpenEdition() '打开草图编辑并定义草图2D对象

Set geometricElements1 = sketch1.GeometricElements '定义草图的几何元素

Set axis2D1 = geometricElements1.Item("绝对轴") '定义草图2D绝对轴

Set line2D1 = axis2D1.GetItem("横向") '定义草图2D横轴

line2D1.ReportName = 1 '定义横轴在系统内部参数

Set line2D2 = axis2D1.GetItem("纵向") '定义草图2D纵轴

line2D2.ReportName = 2 '定义纵轴在系统内部参数

Set circle2D1 = factory2D1.CreateClosedCircle(0.000000, 0.000000, 50.000000) '创建一个以原点为中心，半径为50mm的圆

Set point2D1 = axis2D1.GetItem("原点") '定义绝对轴原点

circle2D1.CenterPoint = point2D1 '定义圆的圆心基于原点

circle2D1.ReportName = 3 '定义圆在系统内部参数

sketch1.CloseEdition '关闭草图编辑

part1.InWorkObject = hybridBody1 '定义工作对象为几何图形集

part1.Update '更新Part文档对象

Set bodies1 = part1.Bodies '定义几何体集合

Set body1 = bodies1.Item("零件几何体") '定义零件几何体对象

part1.InWorkObject = body1 '定义工作对象为零件几何体

Set shapeFactory1 = part1.ShapeFactory '定义图形命令集合

Set pad1 = shapeFactory1.AddNewPad(sketch1, 20.000000) '创建以草图为截面、拉伸20mm的凸台

part1.Update '更新Part文档对象

End Sub