目录
- 引出
- vb.net和vb6.0
- 进程外开发环境搭建
- vb.net开发环境搭建
- 《CATIA二次开发技术基础》模板
- 添加宏库引用
- vs开发环境初步
- vs中的立即窗口
- 对象浏览器
- 建立模板
- 案例：创建一堆圆柱曲面
- 第一步：录制宏
- 第二步：代码精简
- 第三步：for循环改造
- 第四步：人机交互改造
- 窗口模态设置
- 导出窗口fm
- 第五步：搭建vs的开发环境
- 窗口布局设置
- 第六步：改造录制的宏
- 第七步：进行测试
- 报错：关于非窗体转换成窗体报错Model1中找不到sub main
- 总结
- 认识CATIA二次开发
- 刘瑞欣 vb程序设计教程
- Excel中的vba开发
- catia中的vba开发
- 宏的录制、回放和编辑
- 宏代码精简
- 画圆柱阵列
- 宏Macro文件的3种类型
- 宏的保存：文件夹，项目，catia文件
- 宏加入到工具条中
- 插曲：工具条的恢复
- 发生肾么事了？？
- 鼠标中键旋转不了
- 解决：特征树不显示参数关系
- 我的窗口去哪了？
- 插曲：草图工具的调出
- 插曲：颜色工具栏显示
- 弹窗警告
- 警告：创建约束是临时的
- 操作技巧
- 技巧：快速隐藏不相关元素
- 异形弹簧
- 新建几何体
- 草图编辑，画一条样条线
- 进行扫掠，圆心和半径
- 画出曲面上的螺旋线
- 再次选择扫掠，圆心和半径
引出
最近在研究catia二次开发，发现网上的资料非常有限，尤其是博客文件比较少，这个系列文章是本人的学习笔记，分享出来，只为抛砖引玉，希望对你有帮助。
CATIA二次开发VBA入门（3）——进程外开发环境搭建，vb.net在Visual Studio中开发，创建圆柱曲面的宏录制到二次开发案例
vb.net和vb6.0
VB.NET一种简单，现代，面向对象计算机编程语言，有微软开发，VB.NET是一种基于.NET Framework的面向对象编程语言，它是Visual Basic语言的继承者，但是与早期版本的Visual Basic有很大的不同。VB.NET是一种强类型语言，支持类、接口委托、异常处理、LINQ等现代编程特性，可以开发Windows应用程序、Web应用程序、服务和组价。它还支持多线程和异步编程，并且可以与其他的.NET语言(如C#)进行交互。VB.NET是一种易学易用的语言,适合初学者和专业开发人员
特点:
1.面向对象：VB.NET 是一种完全面向对象的语言，支持封装、继承和多态等面向对象的特性。
2.强类型：VB.NET 是一种强类型语言，需要在编译时进行类型检查，避免在运行时出现类型错误。
3.安全性：VB.NET 具有良好的安全性，支持代码访问权限控制、类型安全、内存管理等功能，可以有效地防止程序运行时出现安全问题。
4.可扩展性：VB.NET 可以轻松地扩展和定制，可以使用 COM 组件、.NET 组件和自定义组件等方式扩展应用程序的功能。
5.多平台支持：VB.NET 可以运行在多个操作系统上，包括 Windows、Linux 和 macOS 等。
6.集成开发环境：VB.NET 可以与 Visual Studio 集成使用，提供了丰富的开发工具和调试功能，可以提高开发效率和代码质量。
7.数据库支持：VB.NET 提供了对多种数据库的支持，包括 ADO.NET、OLE DB 和 ODBC 等，可以方便地访问和操作数据库
VB.NET和VB6.两种不同的Visual Basic版本，它们在语言、架构、开发环境、应用场景等方面都有很大的差异。
| 不同之处 | ||||||
|---|---|---|---|---|---|---|
| 类型 | 语言 | 架构 | 开发环境 | 应用场景 | 编译器 | 文件格式 |
| VB.NET | 完全面向对象语言支持更多语言:泛型,LINNQ,匿名来类型 | .NET Framework支持更多.NET Framework特性：Windows Forms,WPF,ASP.NET | Visual Studio | 构建大型的企业级应用用程序 | .NET | VB或VB.ET |
| VB6.0 | 基于事件语言 | COM | 集成开发环境(IDE) | 小型的应用程序和系统内的维护和升级 | Microsoft Vissual Basic 6.0 | .frm、.cls.bas等 |
进程外开发环境搭建
vb.net开发环境搭建
- 新建模块
创建了窗口和模块
《CATIA二次开发技术基础》模板
Imports INFITF
Module Module1
Public CATIA As INFITF.Application
Public Sub Main()
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
End Sub
End Module
添加宏库引用
catia自带的vba开发环境已经引用了很多库
需要在vb中引入import
vs开发环境初步
vs中的立即窗口
Imports MECMOD
Module Module1
Public CATIA As INFITF.Application
Public oPartDoc As PartDocument
Sub Main()
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
oPartDoc = CATIA.ActiveDocument
MsgBox(oPartDoc.Name)
End Sub
End Module
对象浏览器
Imports MECMOD
Module Module1
Public CATIA As INFITF.Application
Public oPartDoc As PartDocument
Public oPart As Part
Public oBodies As Bodies
Public oBody As Body
Sub Main()
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
oPartDoc = CATIA.ActiveDocument
'MsgBox(oPartDoc.Name)
oPart = oPartDoc.Part
oBodies = oPart.Bodies
oBody = oBodies.Item(1)
MsgBox(oBody.Name)
End Sub
End Module
建立模板
可以把设置好库函数的引用的工程文件，作为一个标准的模板，后面直接复制这个标准模板，然后在这上面开发，就不需要每次都要创建各种引用了。
案例：创建一堆圆柱曲面
先创建一个宏库，用于保存接下来要录制的宏程序
第一步：录制宏
然后，工具，宏，启动录制，新建一个part，草图编辑，然后拉升，获得一个圆柱
编辑录制的宏
Sub CATMain()
Dim documents1 As Documents
Set documents1 = CATIA.Documents
Dim partDocument1 As PartDocument
Set partDocument1 = documents1.Add("Part")
Dim part1 As Part
Set part1 = partDocument1.Part
Dim bodies1 As Bodies
Set bodies1 = part1.Bodies
Dim body1 As Body
Set body1 = bodies1.Item("零件几何体")
Dim sketches1 As Sketches
Set sketches1 = body1.Sketches
Dim originElements1 As OriginElements
Set originElements1 = part1.OriginElements
Dim reference1 As Reference
Set reference1 = originElements1.PlaneXY
Dim sketch1 As Sketch
Set sketch1 = sketches1.Add(reference1)
Dim arrayOfVariantOfDouble1(8)
arrayOfVariantOfDouble1(0) = 0#
arrayOfVariantOfDouble1(1) = 0#
arrayOfVariantOfDouble1(2) = 0#
arrayOfVariantOfDouble1(3) = 1#
arrayOfVariantOfDouble1(4) = 0#
arrayOfVariantOfDouble1(5) = 0#
arrayOfVariantOfDouble1(6) = 0#
arrayOfVariantOfDouble1(7) = 1#
arrayOfVariantOfDouble1(8) = 0#
Set sketch1Variant = sketch1
sketch1Variant.SetAbsoluteAxisData arrayOfVariantOfDouble1
part1.InWorkObject = sketch1
Dim factory2D1 As Factory2D
Set factory2D1 = sketch1.OpenEdition()
Dim geometricElements1 As GeometricElements
Set geometricElements1 = sketch1.GeometricElements
Dim axis2D1 As Axis2D
Set axis2D1 = geometricElements1.Item("绝对轴")
Dim line2D1 As Line2D
Set line2D1 = axis2D1.GetItem("横向")
line2D1.ReportName = 1
Dim line2D2 As Line2D
Set line2D2 = axis2D1.GetItem("纵向")
line2D2.ReportName = 2
Dim circle2D1 As Circle2D
Set circle2D1 = factory2D1.CreateClosedCircle(0#, 0#, 25#)
circle2D1.ReportName = 3
Dim constraints1 As Constraints
Set constraints1 = sketch1.Constraints
Dim reference2 As Reference
Set reference2 = part1.CreateReferenceFromObject(circle2D1)
Dim constraint1 As Constraint
Set constraint1 = constraints1.AddMonoEltCst(catCstTypeRadius, reference2)
constraint1.Mode = catCstModeDrivingDimension
Dim length1 As Length
Set length1 = constraint1.Dimension
length1.Value = 25#
sketch1.CloseEdition
part1.InWorkObject = sketch1
part1.UpdateObject sketch1
Dim hybridShapeFactory1 As HybridShapeFactory
Set hybridShapeFactory1 = part1.HybridShapeFactory
Dim hybridShapeDirection1 As HybridShapeDirection
Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(0#, 0#, 0#)
Dim reference3 As Reference
Set reference3 = part1.CreateReferenceFromObject(sketch1)
Dim hybridShapeExtrude1 As HybridShapeExtrude
Set hybridShapeExtrude1 = hybridShapeFactory1.AddNewExtrude(reference3, 20#, 0#, hybridShapeDirection1)
hybridShapeExtrude1.SymmetricalExtension = 0
body1.InsertHybridShape hybridShapeExtrude1
part1.InWorkObject = hybridShapeExtrude1
part1.Update
End Sub
第二步：代码精简
代码精简
Sub CATMain()
Set documents1 = CATIA.Documents
Set partDocument1 = documents1.Add("Part")
Set part1 = partDocument1.Part
Set bodies1 = part1.Bodies
Set body1 = bodies1.Item("零件几何体")
Set sketches1 = body1.Sketches
Set originElements1 = part1.OriginElements
Set reference1 = originElements1.PlaneXY
Set sketch1 = sketches1.Add(reference1)
Set factory2D1 = sketch1.OpenEdition()
Set circle2D1 = factory2D1.CreateClosedCircle(0#, 0#, 5#)
Set constraints1 = sketch1.Constraints
Set reference2 = part1.CreateReferenceFromObject(circle2D1)
Set constraint1 = constraints1.AddMonoEltCst(catCstTypeRadius, reference2)
Set length1 = constraint1.Dimension
length1.Value = 5#
sketch1.CloseEdition
part1.InWorkObject = sketch1
part1.Update
Set hybridShapeFactory1 = part1.HybridShapeFactory
Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(0#, 0#, 0#)
Set reference3 = part1.CreateReferenceFromObject(sketch1)
Set hybridShapeExtrude1 = hybridShapeFactory1.AddNewExtrude(reference3, 20#, 0#, hybridShapeDirection1)
'hybridShapeExtrude1.SymmetricalExtension = 0
body1.InsertHybridShape hybridShapeExtrude1
part1.InWorkObject = hybridShapeExtrude1 '需要加上，不然不会自动更新
part1.Update
End Sub
第三步：for循环改造
for循环改造
Sub CATMain()
Set documents1 = CATIA.Documents
Set partDocument1 = documents1.Add("Part")
Set part1 = partDocument1.Part
Set bodies1 = part1.Bodies
Set body1 = bodies1.Item("零件几何体")
X = 0
For i = 1 To 5
Set sketches1 = body1.Sketches
Set originElements1 = part1.OriginElements
Set reference1 = originElements1.PlaneXY
Set sketch1 = sketches1.Add(reference1)
Set factory2D1 = sketch1.OpenEdition()
Set circle2D1 = factory2D1.CreateClosedCircle(X, 0#, 5#)
Set constraints1 = sketch1.Constraints
Set reference2 = part1.CreateReferenceFromObject(circle2D1)
Set constraint1 = constraints1.AddMonoEltCst(catCstTypeRadius, reference2)
Set length1 = constraint1.Dimension
length1.Value = 5#
sketch1.CloseEdition
part1.InWorkObject = sketch1
part1.Update
Set hybridShapeFactory1 = part1.HybridShapeFactory
Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(0#, 0#, 0#)
Set reference3 = part1.CreateReferenceFromObject(sketch1)
Set hybridShapeExtrude1 = hybridShapeFactory1.AddNewExtrude(reference3, 20#, 0#, hybridShapeDirection1)
'hybridShapeExtrude1.SymmetricalExtension = 0
body1.InsertHybridShape hybridShapeExtrude1
part1.InWorkObject = hybridShapeExtrude1 '需要加上，不然不会自动更新
part1.Update
X = X + 20
Next
part1.Update
End Sub
第四步：人机交互改造
顶部对齐
Private Sub CommandButton1_Click()
Set documents1 = CATIA.Documents
Set partDocument1 = documents1.Add("Part")
Set part1 = partDocument1.Part
Set bodies1 = part1.Bodies
Set body1 = bodies1.Item("零件几何体")
X = 0
For i = 1 To TextBox1.Value
Set sketches1 = body1.Sketches
Set originElements1 = part1.OriginElements
Set reference1 = originElements1.PlaneXY
Set sketch1 = sketches1.Add(reference1)
Set factory2D1 = sketch1.OpenEdition()
Set circle2D1 = factory2D1.CreateClosedCircle(X, 0#, 5#)
Set constraints1 = sketch1.Constraints
Set reference2 = part1.CreateReferenceFromObject(circle2D1)
Set constraint1 = constraints1.AddMonoEltCst(catCstTypeRadius, reference2)
Set length1 = constraint1.Dimension
length1.Value = 5#
sketch1.CloseEdition
part1.InWorkObject = sketch1
part1.Update
Set hybridShapeFactory1 = part1.HybridShapeFactory
Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(0#, 0#, 0#)
Set reference3 = part1.CreateReferenceFromObject(sketch1)
Set hybridShapeExtrude1 = hybridShapeFactory1.AddNewExtrude(reference3, 20#, 0#, hybridShapeDirection1)
'hybridShapeExtrude1.SymmetricalExtension = 0
body1.InsertHybridShape hybridShapeExtrude1
part1.InWorkObject = hybridShapeExtrude1 '需要加上，不然不会自动更新
part1.Update
X = X + TextBox2.Value
Next
part1.Update
End Sub
窗口模态设置
导出窗口fm
这里本来想导出vba中创建的窗口，然后在vb.net中导入，直接使用，但是两个版本的vb差别较大，并没有成功
添加现有项失败，可能是版本的问题，毕竟vb是很老的，我这里用的是vs
第五步：搭建vs的开发环境
Imports MECMOD
Imports PARTITF
Imports HybridShapeTypeLib
Module Module1
Public CATIA As INFITF.Application
Public oPartDoc As PartDocument
Public oPart As Part
Public oBodies As Bodies
Public oBody As Body
Public oHBodies As HybridBodies
Public oHBody As HybridBody
Public oSF As ShapeFactory
Public oHSF As HybridShapeFactory
' ***********************************************************************
' 目的： 初始化CATIA产品文档，并初始化必要的基本变量
'
' 输入： bNewProduct: 初始化时是否新建产品文件
' 可选，默认新建文件
' strProduct: 初始化时是否打开已经存在的产品文件
' 可选，默认新建文件
' ***********************************************************************
Sub InitCATIAPart(Optional ByVal bNewPart As Boolean = True,
Optional ByVal strPart As String = "")
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
If bNewPart Then
oPartDoc = CATIA.Documents.Add("Part")
Else
If strPart = "" Then
oPartDoc = CATIA.ActiveDocument
If oPartDoc Is Nothing Then
Err.Clear()
oPartDoc = CATIA.Documents.Add("Part")
End If
Else
If Dir(strPart) <> "" Then
oPartDoc = CATIA.Documents.Open(strPart)
Else
MsgBox("指定的文件不存在！")
End
End If
End If
End If
On Error GoTo 0
oPartDoc = CATIA.ActiveDocument
oPart = oPartDoc.Part
oBodies = oPart.Bodies
oBody = oBodies.Item(1)
oHBodies = oPart.HybridBodies
oHBody = oHBodies.Add()
oSF = oPart.ShapeFactory
oHSF = oPart.HybridShapeFactory
End Sub
End Module
窗口布局设置
第六步：改造录制的宏
Imports MECMOD
Imports HybridShapeTypeLib
Imports INFITF
Public Class Form1
Private Sub Button1_Click(sender As Object, e As EventArgs) Handles Button1.Click
InitCATIAPart(True) 'true表示新建一个part
Dim XDis As Integer = 0
For iCount = 1 To Val(TextBox1.Text)
Dim sketches1 As Sketches = oBody.Sketches
Dim originElements1 As OriginElements = oPart.OriginElements
Dim reference1 As Reference = originElements1.PlaneXY
Dim sketch1 As Sketch = sketches1.Add(reference1)
Dim factory2D1 As Factory2D = sketch1.OpenEdition()
Dim circle2D1 As Circle2D = factory2D1.CreateClosedCircle(XDis, 0#, 5.0#)
Dim constraints1 As Constraints = sketch1.Constraints
Dim reference2 As Reference = oPart.CreateReferenceFromObject(circle2D1)
Dim constraint1 = constraints1.AddMonoEltCst(CatConstraintType.catCstTypeRadius, reference2)
Dim length1 = constraint1.Dimension
length1.Value = 5.0#
sketch1.CloseEdition()
oPart.InWorkObject = sketch1
oPart.Update()
Dim hybridShapeDirection1 As HybridShapeDirection = oHSF.AddNewDirectionByCoord(0#, 0#, 0#)
Dim reference3 As Reference = oPart.CreateReferenceFromObject(sketch1)
Dim hybridShapeExtrude1 = oHSF.AddNewExtrude(reference3, 20.0#, 0#, hybridShapeDirection1)
'hybridShapeExtrude1.SymmetricalExtension = 0
oBody.InsertHybridShape(hybridShapeExtrude1)
oPart.InWorkObject = hybridShapeExtrude1 '需要加上，不然不会自动更新
oPart.Update()
XDis = XDis + Val(TextBox2.Text)
Next
oPart.Update()
End Sub
End Class
第七步：进行测试
报错：关于非窗体转换成窗体报错Model1中找不到sub main
启动成功
总结
CATIA二次开发VBA入门（3）——进程外开发环境搭建，vb.net在Visual Studio中开发，创建圆柱曲面的宏录制到二次开发案例
其他内容
认识CATIA二次开发
V5 AUTOMATION开发
刘瑞欣 vb程序设计教程
Excel中的vba开发
catia中的vba开发
宏的录制、回放和编辑
宏代码精简
录制到项目中，录制成一个模块
catia的vba开发环境设置，取消dim的限值，这样就可以不用定义变量，便于简化录制的宏程序
Sub CATMain()
Set partDocument2 = CATIA.Documents.Add("Part")
Set part2 = partDocument2.Part
Set body1 = part2.Bodies.Item("零件几何体")
Set sketches1 = body1.Sketches
Set originElements1 = part2.OriginElements
Set reference1 = originElements1.PlaneYZ
Set sketch1 = sketches1.Add(reference1)
part2.InWorkObject = sketch1
Set factory2D1 = sketch1.OpenEdition()
Set circle2D1 = factory2D1.CreateClosedCircle(0#, 0#, 20)
sketch1.CloseEdition
part2.InWorkObject = sketch1
Set hybridShapeFactory1 = part2.HybridShapeFactory
Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(0#, 0#, 0#)
Set reference2 = part2.CreateReferenceFromObject(sketch1)
Set hybridShapeExtrude1 = hybridShapeFactory1.AddNewExtrude(reference2, 60#, 60#, hybridShapeDirection1)
hybridShapeExtrude1.SymmetricalExtension = 0
body1.InsertHybridShape hybridShapeExtrude1
part2.InWorkObject = hybridShapeExtrude1
part2.Update
End Sub
画圆柱阵列
Sub CATMain()
Set partDocument2 = CATIA.Documents.Add("Part")
Set part2 = partDocument2.Part
Set body1 = part2.Bodies.Item("零件几何体")
Set sketches1 = body1.Sketches
Set originElements1 = part2.OriginElements
Set reference1 = originElements1.PlaneYZ
Set sketch1 = sketches1.Add(reference1)
part2.InWorkObject = sketch1
Set factory2D1 = sketch1.OpenEdition()
'--------------------------------------------
For i = 0 To 99
Set circle2D1 = factory2D1.CreateClosedCircle(50 * i, 0#, 20)
Next
'--------------------------------------------
sketch1.CloseEdition
part2.InWorkObject = sketch1
Set hybridShapeFactory1 = part2.HybridShapeFactory
Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(0#, 0#, 0#)
Set reference2 = part2.CreateReferenceFromObject(sketch1)
Set hybridShapeExtrude1 = hybridShapeFactory1.AddNewExtrude(reference2, 60#, 60#, hybridShapeDirection1)
hybridShapeExtrude1.SymmetricalExtension = 0
body1.InsertHybridShape hybridShapeExtrude1
part2.InWorkObject = hybridShapeExtrude1
part2.Update
End Sub
每次画完都自动更新，这样能实时看到caita的变化
宏Macro文件的3种类型
宏的保存：文件夹，项目，catia文件
保存到文件中的两种后缀格式，catiaScript和vbScript，即catia脚本和vb脚本
catvba模式的导出
宏的默认编辑器设置
宏加入到工具条中
选择catiavba项目作为当前的宏库
工具，自定义选项卡
可以设置图标
按住，拖到工具条中
方式一：工具条中，点击图标运行，显示弹窗
方式二：作为catia脚本，直接双击运行
插曲：工具条的恢复
发生肾么事了？？
鼠标中键旋转不了
解决：特征树不显示参数关系
我的窗口去哪了？
插曲：草图工具的调出
插曲：颜色工具栏显示
如果没有看到能更改颜色的工具栏，则点击如下
弹窗警告
警告：创建约束是临时的
操作技巧
技巧：快速隐藏不相关元素
快速隐藏不相关的元素
异形弹簧
新建几何体
草图编辑，画一条样条线
进行扫掠，圆心和半径
画出曲面上的螺旋线
定义直线，选择曲线的角度/法线
在曲线上创建点
支持面选择扫掠面，角度7度，终点设置大一点，选中支持面上的几何图形
再次选择扫掠，圆心和半径
双击修改，调整一下样条曲线
