通过单击 Excel 按钮在 Catia 中设计零件

Question

我已经在宏编辑器内置的 Catia V5 中编写了一些宏，但我不知道如何从 Excel 访问 Catia 命令。

我想知道如何通过仅在 excel 文件中圆柱体的半径和长度来创建一个简单的直圆柱体。

我想在 Catia 中制作不同的压力容器，方法是在 Excel 中输入它们的直径和高度，然后单击该 Excel 表中的按钮后容器应该出现在 Catia 中。如果我已经需要在 Catia 中打开一个空的部分，我没有问题，但最好只打开 Catia，其中没有加载任何内容。

如果我有开始，看看如何从 Excel 访问 Catia 方法，我想我可以找出完成容器所需的其他方法，如颈部、帽等。

谢谢。

编辑： 我设法测试了一些东西，我遇到了一个问题，我不知道如何在 Excel vba 中设置约束。我将代码从 Catia vb 移到 Visual Express 并设法让它在那里工作，但在 excel 中我找不到有关如何使用驱动尺寸的链接。

这是我的代码：

Sub Main()

    Dim CATIA As Object
    Set CATIA = GetObject(, "CATIA.Application")

    Set openDocument = CATIA.ActiveDocument

    Set currentPart = openDocument.Part

    Set currentHybridBodies = currentPart.HybridBodies

    Set currentHybridBody = currentHybridBodies.Add()

    Set referenceHybridBody = currentPart.CreateReferenceFromObject(currentHybridBody)

    currentPart.HybridShapeFactory.ChangeFeatureName referenceHybridBody, "GeometricalSet"

    Set partOriginElements = currentPart.OriginElements

    Set plnYZ = currentPart.OriginElements.PlaneYZ

    Set currentGeometricalSet = currentPart.HybridShapeFactory

    Dim currentOffset As Integer
    Dim circleDiameter As Integer
    Dim cylinderLength As Integer

    currentOffset = 0

    circleDiameter = Range("B2").Value

    cylinderLength = Range("B3").Value

    Call CreateCylinder(0, 0, circleDiameter, cylinderLength, currentOffset)

    currentPart.Update

    currentOffset = currentOffset + cylinderLength

    circleDiameter = Range("B5").Value

    cylinderLength = Range("B6").Value


    Call CreateCylinder(0, 0, circleDiameter, cylinderLength, currentOffset)

    openDocument.Part.Update

    currentOffset = currentOffset + cylinderLength

    circleDiameter = Range("B8").Value

    cylinderLength = Range("B9").Value

    Call CreateCylinder(0, 0, circleDiameter, cylinderLength, currentOffset)

    currentPart.Update

    currentOffset = currentOffset + cylinderLength

    CATIA.ActiveWindow.ActiveViewer.Reframe

End Sub




Sub CreateCylinder(iCenterX, iCenterY, iDiameter, iLength, iPlaneOffset)

    Set CATIA = GetObject(, "CATIA.Application")
    Set openDocument = CATIA.ActiveDocument
    Set currentPart = openDocument.Part
    Set plnYZ = currentPart.OriginElements.PlaneYZ
    Set currentGeometricalSet = currentPart.HybridShapeFactory

    Set planeOffset1 = currentGeometricalSet.AddNewPlaneOffset(plnYZ, iPlaneOffset, False)

    Set currentHybridBody = currentPart.HybridBodies.Item("GeometricalSet")

    currentHybridBody.AppendHybridShape (planeOffset1)

    openDocument.Part.Update

    Set currentBodies = currentPart.Bodies

    Set currentBody = currentBodies.Add()

    Set currentSketch = currentBody.Sketches.Add(planeOffset1)

    Dim Factory2D As Object

    Set Factory2D = currentSketch.OpenEdition

    Set geometricElements1 = currentSketch.GeometricElements

    Dim axis2D1 As Object

    Set axis2D1 = geometricElements1.Item("AbsoluteAxis")

    Dim line2D1 As Object

    Set line2D1 = axis2D1.GetItem("HDirection")

    Dim line2D2 As Object

    Set line2D2 = axis2D1.GetItem("VDirection")

    Set currentCircle = Factory2D.CreateClosedCircle(iCenterX, iCenterY, iDiameter / 2)

    Dim point2D1 As Object

    Set point2D1 = axis2D1.GetItem("Origin")

    Dim constraints1 As Object

    Set constraints1 = currentSketch.Constraints

    Dim reference2 As Object

    Set reference2 = currentPart.CreateReferenceFromObject(currentCircle)

    Dim constraint1 As Object

    Set constraint1 = constraints1.AddMonoEltCst(catCstTypeRadius, reference2)

    Dim catCstModeDrivingDimensions As Object

    'Set constraint1.Mode = catCstModeDrivingDimensions  'Here I get the error

    Dim iRadius As Double

    iRadius = iDiameter / 2       

    currentCircle.CenterPoint = point2D1

    currentSketch.CloseEdition

    Dim newPad As Object

    Set newPad = currentPart.ShapeFactory.AddNewPad(currentSketch, iLength)

End Sub

在该注释行上，我收到错误 438：对象不支持此属性或方法。

代码在没有该行的情况下工作，但几何元素不受约束，相反它们看起来是固定的，我不想要这个。

该代码在 Visual Express 中运行良好，并将所有约束放在应有的位置。

谁能告诉我如何将 Catia 命令链接到 excel vb。

这是来自 v5 自动化文档：

枚举 CatConstraintMode { catCstModeDrivingDimension, catCstModeDrivenDimension }

感谢您对我的代码提供任何反馈。

谢谢。

excel sheet

编辑： 我似乎被允许导入的唯一参考是这些： references

如果我选择其他人，我会收到错误：加载 DLL 时出错。 Catia 安装在服务器上，但我可以使用 Browse 指向它...我仍然不确定在那里选择什么，因为有很多文件。

Answer 1

这是创建螺栓的代码。将代码粘贴到 Excel 中的模块中，并为宏分配一个按钮。

Sub Button1_Click()
  Dim CATIA As Object
    
  'Get CATIA or Launch it if necessary.
  On Error Resume Next
  Set CATIA = GetObject(, "CATIA.Application")
  If CATIA Is Nothing Then
     Set CATIA = CreateObject("CATIA.Application")
    CATIA.Visible = True
  End If
  On Error GoTo 0
  
  ' Add a new Part
  Set MyDocument = CATIA.documents.Add("Part")
  Set PartFactory = MyDocument.part.ShapeFactory  ' Retrieve the Part Factory.
  Set MyBody1 = MyDocument.part.Bodies.Item("PartBody")
  CATIA.ActiveDocument.part.InWorkObject = MyBody1 ' Activate "PartDesign"
  
' Creating the Shaft
  Set ReferencePlane1 = MyDocument.part.CreateReferenceFromGeometry(MyDocument.part.OriginElements.PlaneYZ)
  
  ' Create the sketch1 on ReferencePlane1
  Set Sketch1 = MyBody1.Sketches.Add(ReferencePlane1)
  Set MyFactory1 = Sketch1.OpenEdition() ' Define the sketch


  
  h1 = Range("E6").Value ' height of the bolt
  h2 = Range("E7").Value ' total height
  r1 = Range("E8").Value ' external radius
  r2 = Range("E9").Value ' Internal radius
  s1 = Range("E10").Value ' Size of the chamfer
  
  Set l101 = MyFactory1.CreateLine(0, 0, r1 - 20, 0)
  Set l102 = MyFactory1.CreateLine(r1 - 20, 0, r1, -20)
  Set l103 = MyFactory1.CreateLine(r1, -20, r1, -h1 + 20)
  Set l104 = MyFactory1.CreateLine(r1, -h1 + 20, r1 - 20, -h1)
  Set l105 = MyFactory1.CreateLine(r1 - 20, -h1, r2, -h1)
  Set l106 = MyFactory1.CreateLine(r2, -h1, r2, -h2 + s1)
  Set l107 = MyFactory1.CreateLine(r2, -h2 + s1, r2 - s1, -h2)
  Set l108 = MyFactory1.CreateLine(r2 - s1, -h2, 0, -h2)
  Set l109 = MyFactory1.CreateLine(0, -h2, 0, 0)
  Sketch1.CenterLine = l109
  
  Sketch1.CloseEdition
  Set AxisPad1 = PartFactory.AddNewShaft(Sketch1)
  
' Creating the Pocket
  Set ReferencePlane2 = MyDocument.part.CreateReferenceFromGeometry(MyDocument.part.OriginElements.PlaneXY)
    
  ' Create the sketch2 on ReferencePlane2
  Set Sketch2 = MyBody1.Sketches.Add(ReferencePlane2)
  Set MyFactory2 = Sketch2.OpenEdition() ' Define the sketch
  D = 1 / 0.866
  
  Set l201 = MyFactory2.CreateLine(D * 100, 0, D * 50, D * 86.6)
  Set l202 = MyFactory2.CreateLine(D * 50, D * 86.6, D * -50, D * 86.6)
  Set l203 = MyFactory2.CreateLine(D * -50, D * 86.6, D * -100, 0)
  Set l204 = MyFactory2.CreateLine(D * -100, 0, D * -50, D * -86.6)
  Set l205 = MyFactory2.CreateLine(D * -50, D * -86.6, D * 50, D * -86.6)
  Set l206 = MyFactory2.CreateLine(D * 50, D * -86.6, D * 100, 0)

  ' Create a big circle around the form to get a Hole
  Set c2 = MyFactory2.CreateClosedCircle(0, 0, 300)
  
  Sketch2.CloseEdition
  Set AxisHole2 = PartFactory.AddNewPocket(Sketch2, h1)
  
  MyDocument.part.Update


End Sub

https://www.dropbox.com/s/rjuadpmsso8fe1p/20160423_2208_36.avi?dl=0