Auto Ordinate Dimensions

[Anonymous]

I'm trying to use iLogic or VBA to add ordinate dimensions to a drawing. This picture explains it.

Here is the code I'm working with so far.

Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

Dim oActiveSheet As Sheet
oActiveSheet = oDrawDoc.ActiveSheet

Dim oIntentCollection As ObjectCollection
oIntentCollection = ThisApplication.TransientObjects.CreateObjectCollection

' Get all the selected drawing curve segments.
Dim oDrawingCurveSegment As DrawingCurveSegment
Dim oDrawingCurve As DrawingCurve

For Each oDrawingCurveSegment In oDrawDoc.SelectSet
    
    ' Set a reference to the drawing curve.
    oDrawingCurve = oDrawingCurveSegment.Parent
    
    Dim oDimIntent As GeometryIntent
    oDimIntent = oActiveSheet.CreateGeometryIntent(oDrawingCurve)
    
    Call oIntentCollection.Add(oDimIntent)
Next

' Set a reference to the view to which the curve belongs.
Dim oDrawingView As DrawingView
oDrawingView = oDrawingCurve.Parent

'  a reference to the ordinate dimensions collection.
Dim oOrdinateDimensions As OrdinateDimensions
oOrdinateDimensions = oActiveSheet.DrawingDimensions.OrdinateDimensions

' Determine the placement point
Dim oPlacementPoint As Point2d
oPlacementPoint = ThisApplication.TransientGeometry.CreatePoint2d(oDrawingView.Left - 5, oDrawingView.Center.Y)

' Create a vertical ordinate set dimension.
Dim oOrdinateSet As OrdinateDimensionSet
oOrdinateSet = OrdinateDimensionSet.AddMember(oIntentCollection)

Any help is appreciated.

[mbaltazarJTZL6]

Hello,

I've tried to use lines instead of drill holes, but it doesn't work. Do you know how to change it so it's done in lines, something like this one I'm attaching?

[BM_Ashraf · Accepted solution]

Hi, 

The previous script is a VBA Code and you are using it in ilogic. 

Here is the iLogic one

Public Sub Main()
    ' Set a reference to the drawing document.
    ' This assumes a drawing document is active.
    Dim oDrawDoc As DrawingDocument = ThisApplication.ActiveDocument
    
    ' Set a reference to the active sheet.
    Dim oActiveSheet As Sheet = oDrawDoc.ActiveSheet
    
    Dim oDoc As Document = oActiveSheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocument
    
    If oDoc.DocumentType = kAssemblyDocumentObject Then
    
        '   a reference to the drawing curve segment.
        ' This assumes that a linear drawing curve is selected.
        Dim oDrawingCurveSegment As DrawingCurveSegment = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingCurveSegmentFilter, "Select start line to find occurrence")
        
        '   a reference to the drawing curve.
        Dim oDrawingCurve As DrawingCurve = oDrawingCurveSegment.Parent
        
        Dim oReferDef As AssemblyComponentDefinition = oDoc.ComponentDefinition
        
        Dim pt As WorkPoint = oReferDef.WorkPoints.Item(1)
        
        Call oActiveSheet.DrawingViews.Item(1).SetIncludeStatus(pt, True)
        
        If Not oDrawingCurve.CurveType = CurveTypeEnum.kLineSegmentCurve Then
            MsgBox ("A linear curve should be selected for this sample.")
            Exit Sub
        End If
        
        Dim oCenterMark As Centermark = oActiveSheet.Centermarks.Item(oActiveSheet.Centermarks.Count)
        ' Create point intents to anchor the dimension to.
        Dim oDimIntent  As GeometryIntent = oActiveSheet.CreateGeometryIntent(oCenterMark, kCenterPointIntent)
        
        '   a reference to the view to which the curve belongs.
        Dim oDrawingView As DrawingView= oDrawingCurve.Parent
        
        ' If origin indicator has not been already created, create it first.
        If Not oDrawingView.HasOriginIndicator Then
            ' The indicator will be located at the start point of the selected curve.
            Call oDrawingView.CreateOriginIndicator(oDimIntent)
        End If
        
        '   a reference to the ordinate dimensions collection.
        Dim oOrdinateDimensions As OrdinateDimensions = oActiveSheet.DrawingDimensions.OrdinateDimensions
        
        Dim oTextOrigin  As Point2d
        Dim DimType As DimensionTypeEnum
        
        ' Selected curve is vertical or at an angle.
        DimType = DimensionTypeEnum.kVerticalDimensionType
        
        '   the text points for the 2 dimensions.
        
         oTextOrigin = ThisApplication.TransientGeometry.CreatePoint2d(oCenterMark.Position.X, oCenterMark.Position.Y - 2)
        
        ' Create the first ordinate dimension.
        Dim oOrdinateDimension1 As OrdinateDimension = oOrdinateDimensions.Add(oDimIntent, oTextOrigin, DimType)
        
        Dim LArray() As String
        LArray = Split(oDrawingCurve.ModelGeometry.ContainingOccurrence.Name, ":")
        
        Dim occ As ComponentOccurrence
        For Each occ In oReferDef.Occurrences
            Dim occName() As String
            occName = Split(occ.Name, ":")
            If occName(0) = LArray(0) Then
                 pt = occ.Definition.WorkPoints.Item(1)
                
                Dim oProxy As WorkPointProxy
                Call occ.CreateGeometryProxy(pt, oProxy)
                
                Call oActiveSheet.DrawingViews.Item(1).SetIncludeStatus(oProxy, True)
                
                 oCenterMark = oActiveSheet.Centermarks.Item(oActiveSheet.Centermarks.Count)
                
                Dim oIntent As GeometryIntent
                 oIntent = oActiveSheet.CreateGeometryIntent(oCenterMark, kCenterPointIntent)
                
                Dim origin As Point2d
                 origin = ThisApplication.TransientGeometry.CreatePoint2d(oCenterMark.Position.X, oCenterMark.Position.Y - 2)
                
                Call oOrdinateDimensions.Add(oIntent, origin, DimType)
            End If
        Next
         
    
    Else
        MsgBox ("Referenced document is not an assembly document")
    End If
  
End Sub