CATIA二次开发（VB.NET）——零件设计模块以及草图模块

Sub mi()
Dim plnxy As Plane
Dim opart As Part

Set opart = CATIA.ActiveDocument.Part
Set plnxy = opart.OriginElements.PlaneXY

Dim obody As Body
Set obody = opart.Bodies.Item(3)
Set osketch = obody.Sketches.Add(plnxy)

Dim oHRef As Line2D, oVRef As Line2D

Set oHRef = osketch.AbsoluteAxis.HorizontalReference
Set oVRef = osketch.AbsoluteAxis.VerticalReference

End Sub

Sub mi()
Dim plnxy As Plane
Dim opart As Part

Set opart = CATIA.ActiveDocument.Part
Set plnxy = opart.OriginElements.PlaneXY

Dim obody As Body, osketch As Sketch
Set obody = opart.Bodies.Item(3)
Set osketch = obody.Sketches.Add(plnxy)

'打开草图编辑
Dim factory2D1 As Factory2D
Set factory2D1 = osketch.OpenEdition()

Set oline = factory2D1.CreateLine(0, 0, 10, 20)

'关闭草图编辑
osketch.CloseEdition
opart.Update

End Sub

Sub mi()
Dim plnxy As Plane
Dim opart As Part

Set opart = CATIA.ActiveDocument.Part
Set plnxy = opart.OriginElements.PlaneXY

Dim obody As Body, osketch As Sketch
Set obody = opart.Bodies.Item(3)
Set osketch = obody.Sketches.Add(plnxy)

'打开草图编辑
Dim factory2D1 As Factory2D
Set factory2D1 = osketch.OpenEdition()

Set oline = factory2D1.CreateLine(0, 0, 10, 20)

'进行尺寸约束
Dim olineh As Line2D
Set olineh = osketch.AbsoluteAxis.HorizontalReference

Dim rf1 As Reference, rf2 As Reference '进行引用的创建
Set rf1 = opart.CreateReferenceFromObject(oline)
Set rf2 = opart.CreateReferenceFromObject(olineh)


Dim oconstraints As Constraints, ocinstraint As Constraint
Set oconstraints = osketch.Constraints

Set ocinstraint = oconstraints.AddBiEltCst(catCstTypeAngle, rf1, rf2)

ocinstraint.Dimension.Value = 30 '定义角度是30


'关闭草图编辑
osketch.CloseEdition
opart.Update

End Sub

Imports MECMOD
Imports HybridShapeTypeLib
Imports INFITF
Imports PARTITF

Public Class Form1

    ' 窗体初始化的函数
    Private Sub Form1_Load(sender As Object, e As EventArgs) Handles Me.Load
        On Error Resume Next '有错误的话会忽略，继续执行下一句 
        ' 如果打开catia，就获取当前的这个

        CATIA = GetObject(, "CATIA.Application")
        If Err.Number <> 0 Then
            ' 如果没有打开catia，则打开新的catia
            CATIA = CreateObject("CATIA.Application")
            CATIA.Visible = True
        End If
        On Error GoTo 0

        ' 让catia始终在最上层
        MakeMeOnTop(Me.Handle, True)
    End Sub


    Private Sub Button2_Click(sender As Object, e As EventArgs) Handles Button2.Click
        InitCATIAPart(True) 'true表示新建一个part

        '创建草绘特征
        Dim oPlaneYZ As Plane, oSketch As Sketch
        oPlaneYZ = oPart.OriginElements.PlaneYZ
        oSketch = oBody.Sketches.Add(oPlaneYZ)

        '编辑草绘特征
        Dim oFactory2D As Factory2D
        oFactory2D = oSketch.OpenEdition

        '创建直线
        Dim oLine As Line2D
        oLine = oFactory2D.CreateLine(0, 0, 10, 20)

        Dim oLineH As Line2D
        oLineH = oSketch.AbsoluteAxis.HorizontalReference
        Dim oRef1 As Reference, oRef2 As Reference
        oRef1 = oPart.CreateReferenceFromObject(oLine)
        oRef2 = oPart.CreateReferenceFromObject(oLineH)

        '创建约束
        Dim oConstraints As Constraints, oConstraint As Constraint
        oConstraints = oSketch.Constraints

        'oConstraint = oConstraints.AddBiEltCst(catCstTypeAngle, oRef1, oRef2) '改成如下
        oConstraint = oConstraints.AddBiEltCst(CatConstraintType.catCstTypeAngle, oRef1, oRef2)
        oConstraint.Dimension.Value = 30

        oSketch.CloseEdition()

        '创建Pad特征 需要import PARTITF
        Dim oSF As ShapeFactory, oPad As Pad

        ' 教材上代码会报错，注释掉
        'oSF = oPart.ShapeFactory
        'oPad = oSF.AddNewPad(oSketch, 20)
        'oPad.IsThin = True

        '更新零件
        oPart.Update()

    End Sub
End Class

Sub kn()
Dim opart As Part
Set opart = CATIA.ActiveDocument.Part

Set obody = CATIA.ActiveDocument.Part.Bodies.Item(3)
Set osketch = obody.Sketches.Item(2)

'获得工厂对象
Dim shapefactory1 As ShapeFactory
Set shapefactory1 = opart.ShapeFactory

Set oPad = shapefactory1.AddNewPad(osketch, 10)
opart.Update

End Sub