On my job, I came across a VBa program that consisted of 2 parts. The second part would add dimensions to your drawing. The first part would let you select faces/edges and add properties to it. Pairs of faces/edges are used to create dimensions on a drawing. Those properties included things like the position of the dimension text and to which view the dimension belongs.
This program came across my desk because no one knew how it worked and it stopped working when we migrated to a new version of Inventor. That was a bad decision because I usually have an opinion on how to improve things. And that was also here the case. In my opinion, there were 3 problems:
- Although there was a user interface it was not user-friendly. There was no way of knowing which face where used for a dimension.
- It was written in VBa and we should not be using VBa any more. (Is VBA in Inventor obsolete?)
- It's not very flexible.
All those issues could be solved if they would just use iLogic/named entities. (iLogic add dimensions to drawings) I think creating an iLogic rule is not that complicated but a colleague pointed out to me that this might not be true for everyone. So as a challenge to myself, I created the 2 ilogic rules below that have the same function as the VBa code. But with one big difference. Instead of selecting faces/edges and adding properties to those it makes use of 3D annotations and you can add properties to those. 
With the first rule, you can set up the part for use in the drawing. After you start the rule start by selecting 3D dimension (in a part file). After you select a 3D dimension you will presented with a window. This is a bit special because the window is not native to iLogic. (Credits to Wesley Crihfield for showing off this technique.) In this window, you need to set the sheet and view the name that belongs to the dimension. Also, you need to set the X and Y coordinates on the sheet. The first set is an "iLogic sheet point" coordinate. SheetPoint are normalized view coordinates in the range 0 to 1. x=0, y=0 is at the bottom left corner of the view x=1, y=1 is at the top right corner of the view. So these are relative coordinates to the view. The second set of coordinates are absolute coordinates relative to the first set. 
The second rule is doing all the work. All dimensions are placed by this rule.
You could argue that this rule is not much more than the standard "Retrieve model annotations" but I guess it is more flexible. You can place the dimension text anywhere you like. On the other hand in my experience, if you want to automatically add dimensions then you probably also want to automate other things. In that case, you probably need ilogic anyway and then I think the default iLogic features are easier to maintain.
The first (external) rule is to set up the part.
AddReference "System.Drawing"
Imports System.ComponentModel
Imports System.Drawing
Imports System.Windows.Forms
imports System.Windows
Public Sub Main()
Dim sheetName As String = String.Empty
Dim viewName As String = String.Empty
Dim relativeX, relativeY, absoluteX, absoluteY As Double
Dim annotation As ModelAnnotation = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kModelAnnotationFilter, "Select a dimension")
If (annotation.AttributeSets.NameIsUsed("hjalte.AutoDraw")) Then
Dim attSet = annotation.AttributeSets.Item("hjalte.AutoDraw")
Dim completViewName = "Sheet name:View name"
If (attSet.NameIsUsed("ViewName")) Then completViewName = attSet.Item("ViewName").Value
sheetName = completViewName.Split(":")(0)
viewName = completViewName.Split(":")(1)
If (attSet.NameIsUsed("Text.RelativePosition.X")) Then relativeX = attSet.Item("Text.RelativePosition.X").Value
If (attSet.NameIsUsed("Text.RelativePosition.Y")) Then relativeY = attSet.Item("Text.RelativePosition.Y").Value
If (attSet.NameIsUsed("Text.Position.X")) Then absoluteX = attSet.Item("Text.Position.X").Value
If (attSet.NameIsUsed("Text.Position.Y")) Then absoluteY = attSet.Item("Text.Position.Y").Value
End If
Dim form As New WinForm()
form.TbSheetName.Text = sheetName
form.TbViewtName.Text = viewName
form.TbRelativeX.Text = relativeX
form.TbRelativeY.Text = relativeY
form.TbAbsoluteX.Text = absoluteX
form.TbAbsoluteY.Text = absoluteY
Dim result = form.ShowDialog()
If (result = DialogResult.OK) Then
Dim autoDrawSet As AttributeSet = Nothing
If (annotation.AttributeSets.NameIsUsed("hjalte.AutoDraw")) Then
autoDrawSet = annotation.AttributeSets.Item("hjalte.AutoDraw")
Else
autoDrawSet = annotation.AttributeSets.Add("hjalte.AutoDraw")
End If
SetAttributeValue(autoDrawSet, "ViewName", ValueTypeEnum.kStringType,
String.Format("{0}:{1}", form.TbSheetName.Text, form.TbViewtName.Text))
SetAttributeValue(autoDrawSet, "Text.RelativePosition.X", ValueTypeEnum.kStringType, form.TbRelativeX.Text)
SetAttributeValue(autoDrawSet, "Text.RelativePosition.Y", ValueTypeEnum.kStringType, form.TbRelativeY.Text)
SetAttributeValue(autoDrawSet, "Text.Position.X", ValueTypeEnum.kStringType, form.TbAbsoluteX.Text)
SetAttributeValue(autoDrawSet, "Text.Position.Y", ValueTypeEnum.kStringType, form.TbAbsoluteY.Text)
End If
End Sub
Public Sub SetAttributeValue(attributeSet As AttributeSet, attributeName As String, valueType As ValueTypeEnum, value As Object)
If (attributeSet.NameIsUsed(attributeName)) Then
attributeSet.Item(attributeName).Value = value
Else
attributeSet.Add(attributeName, valueType, value)
End If
End Sub
Public Class WinForm
Inherits System.Windows.Forms.Form
Private _btnOK As Forms.Button = New Forms.Button()
Private _btnCancel As Forms.Button = New Forms.Button()
Public Sub New()
SetupControls()
End Sub
Public Property TbSheetName As Forms.TextBox = New Forms.TextBox()
Public Property TbViewtName As Forms.TextBox = New Forms.TextBox()
Public Property TbRelativeX As Forms.TextBox = New Forms.TextBox()
Public Property TbRelativeY As Forms.TextBox = New Forms.TextBox()
Public Property TbAbsoluteX As Forms.TextBox = New Forms.TextBox()
Public Property TbAbsoluteY As Forms.TextBox = New Forms.TextBox()
Private Sub btnCancel_Click(sender As Object, e As EventArgs)
Me.DialogResult = DialogResult.Cancel
Me.Close()
End Sub
Private Sub btnOK_Click(sender As Object, e As EventArgs)
Me.DialogResult = DialogResult.OK
Me.Close()
End Sub
Private Sub SetupControls()
With Me
.FormBorderStyle = FormBorderStyle.FixedToolWindow
.StartPosition = FormStartPosition.CenterScreen
.Width = 325
.Height = 235
.TopMost = True
.Text = "Drawing position"
.Name = "Drawing position"
End With
' Sheet name controls
CreateLabel(10, 10, 90, 20, "Sheet name")
CreateTextBox(TbSheetName, 10, 100, 200, 20)
' View name controls
CreateLabel(35, 10, 90, 20, "View name")
CreateTextBox(TbViewtName, 35, 100, 200, 20)
' Position controls
CreateLabel(70, 10, 60, 20, "Position")
CreateLabel(70, 120, 60, 20, "X")
CreateLabel(70, 190, 60, 20, "Y")
CreateLabel(95, 10, 90, 20, "Relative")
CreateTextBox(TbRelativeX, 95, 100, 60, 20)
CreateTextBox(TbRelativeY, 95, 170, 60, 20)
CreateLabel(120, 10, 90, 20, "Absolute")
CreateTextBox(TbAbsoluteX, 120, 100, 60, 20)
CreateTextBox(TbAbsoluteY, 120, 170, 60, 20)
' Buttons
With _btnCancel
.Text = "Cancel"
.Top = Me.Height - 80
.Left = Me.Width - 200
.Width = 80
.Height = 30
.Enabled = True
End With
Me.Controls.Add(_btnCancel)
AddHandler _btnCancel.Click, AddressOf btnCancel_Click
With _btnOK
.Text = "Ok"
.Top = Me.Height - 80
.Left = Me.Width - 110
.Width = 80
.Height = 30
.Enabled = True
End With
Me.Controls.Add(_btnOK)
AddHandler _btnOK.Click, AddressOf btnOK_Click
End Sub
Public Sub CreateLabel(top As Integer, left As Integer, width As Integer, height As Integer, text As String)
Dim label As New Forms.Label()
With label
.Top = top
.Left = left
.Width = width
.Height = height
.Text = text
End With
Me.Controls.Add(label)
End Sub
Public Sub CreateTextBox(textBox As Forms.TextBox, top As Integer, left As Integer, width As Integer, height As Integer)
With textBox
.Top = top
.Left = left
.Width = width
.Height = height
End With
Me.Controls.Add(textBox)
End Sub
End ClassThe second rule is to add the dimensions.
Public Sub Main()
Dim doc As DrawingDocument = ThisDoc.Document
ThisDrawing.BeginManage
For Each sheet As Sheet In doc.Sheets
Dim managedSheet As IManagedSheet = ThisDrawing.Sheets.ManagedItem(Sheet)
Dim dimensions As IManagedDrawingDimensions = managedSheet.DrawingDimensions
For Each view As DrawingView In Sheet.DrawingViews
Dim managedView As IManagedDrawingView = managedSheet.DrawingViews.ManagedItem(View)
Dim refDoc As Document = managedView.ModelDocument
Dim sheetName = Sheet.Name.Split(":")(0)
Dim possibleDimensions = refDoc.AttributeManager.FindObjects("hjalte.AutoDraw", "ViewName", String.Format("{0}:{1}",sheetName,View.Name))
For Each possibleDimension As Object In possibleDimensions
If (TypeOf possibleDimension Is LinearModelDimension) Then
Dim dimension As LinearModelDimension = possibleDimension
Dim def As LinearModelDimensionDefinition = dimension.Definition
Dim curve1 = View.DrawingCurves(def.IntentOne.Geometry).Item(1)
Dim curve2 = View.DrawingCurves(def.IntentTwo.Geometry).Item(1)
Dim intent1 = View.Parent.CreateGeometryIntent(curve1, Nothing)
Dim intent2 = View.Parent.CreateGeometryIntent(curve2, Nothing)
Dim x = GetAttributeValue(dimension, "Text.Position.X")
Dim y = GetAttributeValue(dimension, "Text.Position.Y")
Dim xR = GetAttributeValue(dimension, "Text.RelativePosition.X")
Dim yR = GetAttributeValue(dimension, "Text.RelativePosition.Y")
Dim name = String.Format("{0}/{1}", refDoc.DisplayName, dimension.Name)
Dim textPoint = managedView.SheetPoint(xR, yR)
textPoint.X += x
textPoint.Y += y
dimensions.GeneralDimensions.AddLinear(name, textPoint, intent1, intent2)
End If
Next
Next
Next
ThisDrawing.EndManage
End Sub
Public Function GetAttributeValue(annotation As ModelAnnotation, name As String) As Double
Return annotation.AttributeSets.Item("hjalte.AutoDraw").Item(name).Value
End FunctionThis is a variation on the second rule. It also adds the dimensions to the drawing. But it does not use any iLogic API. That could be good news for any one who wants to make an addin out of this code ;-)
Public Sub Main()
Dim doc As DrawingDocument = ThisDoc.Document
For Each sheet As Sheet In doc.Sheets
For Each view As DrawingView In Sheet.DrawingViews
CreateDimensionsForView(View)
Next
Next
End Sub
Public Sub CreateDimensionsForView(view As DrawingView)
Dim refDoc As Document = view.ReferencedDocumentDescriptor.ReferencedDocument
Dim sheet As Sheet = view.Parent
Dim sheetName = sheet.Name.Split(":")(0)
Dim possibleDimensions = refDoc.AttributeManager.FindObjects("hjalte.AutoDraw", "ViewName", String.Format("{0}:{1}",sheetName,view.Name))
For Each item As Object In possibleDimensions
If (TypeOf item Is LinearModelDimension) Then
CreateLinearModelDimension(view, item)
End If
Next
End Sub
Public Sub CreateLinearModelDimension(view As DrawingView, dimension As LinearModelDimension)
Dim sheet As Sheet = view.Parent
Dim def As LinearModelDimensionDefinition = dimension.Definition
Dim curve1 = view.DrawingCurves(def.IntentOne.Geometry).Item(1)
Dim curve2 = view.DrawingCurves(def.IntentTwo.Geometry).Item(1)
Dim intent1 = view.Parent.CreateGeometryIntent(curve1, Nothing)
Dim intent2 = view.Parent.CreateGeometryIntent(curve2, Nothing)
Dim x = GetAttributeValue(dimension, "Text.Position.X")
Dim y = GetAttributeValue(dimension, "Text.Position.Y")
Dim xR = GetAttributeValue(dimension, "Text.RelativePosition.X")
Dim yR = GetAttributeValue(dimension, "Text.RelativePosition.Y")
Dim posX = view.Position.X - (view.Width / 2) + (view.Width * xR) + x
Dim posY = view.Position.Y - (view.Height / 2) + view.Height * yR + y
Dim TextOrigin As Point2d = ThisApplication.TransientGeometry.CreatePoint2d(posX, posY)
sheet.DrawingDimensions.GeneralDimensions.AddLinear(TextOrigin, intent1, intent2)
End Sub
Public Function GetAttributeValue(annotation As ModelAnnotation, name As String) As Double
Return annotation.AttributeSets.Item("hjalte.AutoDraw").Item(name).Value
End Function