CATIA 3DEXPERIENCE R2019x VBA开发介绍

CATIA 3DEXPERIENCE R2019x VBA开发介绍

一、 什么是VBA？

【VBA的官方解释】
VBA（Visual Basic for Applications）是VisualBasic的一种宏语言，是在其桌面应用程序中执行通用的自动化(OLE)任务的编程语言。主要能用来扩展Windows的应用程序功能，特别是MicrosoftOffice软件。它也可说是一种应用程式视觉化的 Basic 脚本。

CATIA提供了多种二次开发的接口，其中包括自动化对象编程（Automation）和开放的基于构件的应用编程接口（CAA）。本文主要介绍Visual Basic进行自动化对象编程。

二、 在宏编辑器中开发

相对Visual Studio等集成编译环境，宏编辑器无需引用API，直接可以调用Automation对象，进行CATIA二次开发。本文以VB.Net语言编写案例，介绍CATIA基本对象及几何元素的构造和运算方法。
下图为宏编辑器图标，快捷键为 Alt+F11

1. 对象

1)当前编辑对象

Dim oActiveEditor As Editor
Set oActiveEditor = CATIA.ActiveEditor

2)当前激活零件

Dim oPart As Part
Set oPart = CATIA.ActiveEditor.ActiveObject

3) 原点要素

Set PlaneXY = oPart.OriginElements.PlaneXY
Set PlaneXZ = oPart.OriginElements.PlaneZX
Set PlaneYZ = oPart.OriginElements.PlaneYZ

4) 参数

a) 获取结构树Part下的参数集

Dim params As Parameters
Set params = oPart.Parameters

b) 新建参数

Dim parameter1 As parameter
Set parameter1 = params.CreateDimension("长度", "Length", 1000)
Set parameter2 = params.CreateReal("实数", 100)

c) 获取参数（可通过序号或者名字来检索参数）

Set parameter3 = parameters1.Item("长度")

5) 几何体

a) 获取到零件几何体

Dim mainBody As Body
Set mainBody= oPart.MainBody

b) 在oPart下新建名为TestBody的几何体

Dim Bodies As Bodies
Set Bodies = part1.Bodies
Dim Body As Body
Set Body = Bodies.Add()
Body.Name = "TestBody"

c) 在oPart下获取到名为TestBody的几何体

Dim Body As Body
Set Body = Bodies.Item("TestBody")

6) 几何图形集

a) 在oPart下新建名为TestHybridBody的几何图形集

Dim hybridBodies1 As HybridBodies
Set hybridBodies1 = oPart.HybridBodies
Set ohybridBody= hybridBodies1.add()
ohybridBody.Name="TestHybridBody"

b) 获取到oPart下的名为process的几何图形集

Dim hybridBodies1 As HybridBodies
Set hybridBodies1 = oPart.HybridBodies
Dim hybridBody1 As HybridBody
Set hybridBody1 = hybridBodies1.Item("process")

7) 有序几何图形集

a) 在oPart下新建名为TestOrderHybridBody的有序几何图形集

Dim orderHybridBodies As OrderedGeometricalSets
Set orderHybridBodies = part1.OrderedGeometricalSets
Dim orderHybridBody As OrderedGeometricalSet
Set orderHybridBody = orderHybridBodies.Add()
orderHybridBody.Name = "TestOrderHybridBody"

b) 获取到oPart下的名为process的几何图形集

Dim orderHybridBody As OrderedGeometricalSet
Set orderHybridBody = orderHybridBodies.Item("process")

2. 几何构造方法

先获取几何构造方法库HybridShapeFactory

Dim oHybridShapeFactory As HybridShapeFactory
Set oHybridShapeFactory = oPart.HybridShapeFactory

1) 点

a) 通过坐标创建点

Dim iPoint1 As HybridShapePointCoord
Set iPoint1= oHybridShapeFactory.AddNewPointCoord(0, 10, 20)

b) 两点之间创建点

Dim iPoint3 As HybridShapePointBetween
Set iPoint3 = oHybridShapeFactory.AddNewPointBetween(iPoint1, iPoint2, 0.5, 0)
AddNewPointBetween（参考点1，参考点2，比率，方向）

c) 曲线上距离创建点

Dim iPoint4 As HybridShapePointOnCurve
Set iPoint4 = oHybridShapeFactory.AddNewPointOnCurveFromDistance(refLine, 20, False)
AddNewPointOnCurveFromDistance（参考线，长度，布尔）

d) 曲线上比率创建点

Dim iPoint5 As HybridShapePointOnCurve
Set iPoint5 = oHybridShapeFactory.AddNewPointOnCurveFromPercent(refLine, 0.5, False)
AddNewPointOnCurveFromPercent（参考线，比率，布尔）

2) 线

a) 两点连线

Dim refLine As HybridShapeLinePtPt
Set refLine = oHybridShapeFactory.AddNewLinePtPt(iPoint1, iPoint2)
AddNewLinePtPt（参考点1，参考点2）

b) 点方向构造线

Dim dirLine As HybridShapeLinePtDir
Set dirLine = oHybridShapeFactory.AddNewLinePtDir(iPoint5, iDirection, 0, 100, False)
AddNewLinePtDir（参考点，方向，起始长度，结束长度，布尔）

c) 曲线的角度线

Dim angleLine As HybridShapeLineAngle
Set angleLine=oHybridShapeFactory. AddNewLineAngle(refLine,oPart.
OriginElements.PlaneYZ, iPoint1, False, 0, 200, 30, False)
AddNewLineAngle(参考线，支持面，起点，布尔，起始长度，结束长度，布尔)

d) 曲面的法线

Dim normalLine As HybridShapeLineNormal
Set normalLine = oHybridShapeFactory.AddNewLineNormal(refSurface, iPoint3, 0, 200, False)
AddNewLineNormal（参考曲面，参考点，起始长度，结束长度，布尔）

e) 3点圆

Dim circle0 As HybridShapeCircle3Points
Set circle0 = oHybridShapeFactory.AddNewCircle3Points(iPoint1, iPoint2, iPoint3)
circle0.SetLimitation 1

3) 面

a) 拉伸

Dim extrudeSurface As HybridShapeExtrude
Set extrudeSurface = oHybridShapeFactory.AddNewExtrude(CurveJoin, 1000, 1000, oHybridShapeFactory.AddNewDirectionByCoord(0, 0, 1))

b) 填充

Dim fillSurface As HybridShapeFill
Set fillSurface = oHybridShapeFactory.AddNewFill()
Dim reference1 As Reference
Set reference1 = part1.CreateReferenceFromObject(circle0)
fillSurface.AddBound reference1

4) 实体

a) 拉伸凸台

Dim reference1 As Reference
Set reference1 = part1.CreateReferenceFromObject(circle0)
Dim pad1 As Pad
Set pad1 = shapeFactory1.AddNewPadFromRef(reference1, 500)

3. 几何运算方法

1) 投影

Dim projectPoint As HybridShapeProject
Set projectPoint = oHybridShapeFactory.AddNewProject(iPoint4, extrudeSurface)

2) 相交

Dim intersection As HybridShapeIntersection
Set intersection = oHybridShapeFactory.AddNewIntersection
(fillSurface, extrudeSurface)

3) 平移

Dim Z As HybridShapeDirection
Set Z = oHybridShapeFactory.AddNewDirectionByCoord(0, 0, 1)
Dim translate1 As HybridShapeTranslate
Set translate1 = oHybridShapeFactory.AddNewTranslate(iPoint4, Z, 100)

4) 分割

Dim splitSurface As HybridShapeSplit
Set splitSurface = oHybridShapeFactory.AddNewHybridSplit(extrudeSurface, intersection, 0)
splitSurface.AddElementToKeep projectPoint2

5) 延伸

Dim extrapolElement As HybridShapeExtrapol
Set extrapolElement = oHybridShapeFactory.AddNewExtrapolLength(iPoint1, intersection, 100)

三、 在Visual Studio中开发

第一步，引用COM组件

Imports INFITF
Imports HybridShapeTypeLib
Imports MECMOD
public static class CatiaMethods
{
   public static Editor GetEditor()
   {
      Application CATIA;
      try
      {
     CATIA= (INFITF.Application)Marshal.GetActiveObject("CATIA.Application");
      }
      catch
      {
        Type oType = System.Type.GetTypeFromProgID("CATIA.Application");
        CATIA = (INFITF.Application)Activator.CreateInstance(oType);
        CATIA.Visible = true;
      }
        Editor ed = CATIA.ActiveEditor;
        return ed;
     }
}

接下来的套路就和宏编辑器里一样了，但是在Visual Studio中，编写代码要比宏编辑器要方便很多，主要是高级，有逼格。。。

这是本人第一篇博客，希望各位读者多多指教，评论区直接留言或者私信，大家互相学习，共同进步。