Autodesk Inventor 2013 - iLogic Custom Drawing Symbol

by Luke Davenport

I couldn’t resist this challenge – On a recent training course an Inventor user confided the following Inventor problem. For each large assembly drawing he was having to manually place dozens of drawing symbols, numbered from 1 to XX (depending on the size of the assembly) in order to identify each component in a large rectangular layout. Identical components needed a separate designation, and leaders weren’t required, so balloons weren’t an option. Anyway, you won’t have to have read many of my blogs to know that manual repetition makes me angry (kind of like a nerdy CAD hulk) and this prompted a crash course in coding skills to write a little iLogic routine. Check out my video showing it in action, and you can copy and paste the entire code from below.

Just to mention – one limitation of the code is that the view scale recognition will only work for first-view drawing scales between 1:1 and 1:99 – shouldn’t be a huge problem.

itrigger = iTrigger0

' This is the code taken straight from the Being Inventive Blog to find the

‘ view scale

Dim odrawdoc As DrawingDocument

odrawdoc = ThisApplication.ActiveDocument

customPropertySet = odrawdoc.PropertySets.Item("Inventor User Defined Properties")

For i = 1 To odrawdoc.Sheets.Count

' Make sure the desired property exists

Try

 prop = customPropertySet.Item("Scale" + Str(i))

Catch

 ' Assume error means not found

 customPropertySet.Add("", "Scale" + Str(i))

End Try

Try

iProperties.Value("Custom", "Scale" + Str(i)) = odrawdoc.sheets.item(i).DrawingViews.Item(1).ScaleString

Catch

End Try

Next i

InventorVb.DocumentUpdate()

 'This section of code finds the highest symbol already placed

 '[

' Set a reference to the drawing document.

' This assumes a drawing document is active.

oSymbols = oDrawDoc.ActiveSheet.SketchedSymbols

For Each oSymbol In oSymbols 'Find highest placed symbol (assumes the last placed symbol is the highest)

    If Left(oSymbol.Name,7) = "CADline" Then 'Only concerned with CADline symbols

        Dim symbol_number As String = Right(oSymbol.Name,3) 'Find RHS 3 digits (as string)

        Dim InputString As String = symbol_number 'Convert to number

        Dim Result As System.Text.RegularExpressions.Match = System.Text.RegularExpressions.Regex.Match(InputString, "\d+")

        symbol_number_int =(Result.Value)

        symbol_number_int_plus_one = symbol_number_int + 1 'Create variable for next symbol to place

        symbol_number_int_plus_one_str = CStr(symbol_number_int_plus_one) 'Make this variable a string

    End If

Next

']

 'This section of code allows user to decide starting value for symbols

 '[

If symbol_number_int = "" Then 'If there are no symbols placed already

symbol_number_int = 0

start_value = 1

Else

'Allow user to select starting value for pattern

iftruestartfrom1 = InputRadioBox("Starting Number?", "1", symbol_number_int_plus_one & " (Symbols 1-" & symbol_number_int & " are already placed)", iftruestartfrom1, Title := "Select Starting Number")

    If iftruestartfrom1 = True Then

    start_value = 1

    Else

    start_value = symbol_number_int_plus_one

    End If

End If

']

 'This section of code creates pattern variables using using input

 '[

 'Allow user to enter pattern values

 Dim Row_Qty As Double = InputBox("No. of Rows?", "Pattern Values", Row_Qty)

 Dim Col_Qty As Double = InputBox("No. of Columns?", "Pattern Values", Col_Qty)

 Dim Col_Spacing As Double = InputBox("Column Spacing?", "Pattern Values", Col_Spacing)

 Dim Row_Spacing As Double = InputBox("Row Spacing?", "Pattern Values", Row_Spacing)

 Dim View_Scale_Fraction As String 'Get scale of first drawing view

 View_Scale_Fraction = iProperties.Value("Custom", "Scale 1") 'Create iProperty with this value

 View_Scale = Right(View_Scale_Fraction,2)  'Get the RHS of scale value

 View_Scale_Num = Val(View_Scale) 'Convert to value

 Scale_Actual = 1/View_Scale_Num 'Create conversion factor to multiply pattern values

 Col_Spacing_Actual = (Col_Spacing*Scale_Actual)/10 'Set correct column spacing based on view scale

 Row_Spacing_Actual = (Row_Spacing*Scale_Actual)/10 'Set correct row spacing based on view scale

']

 'This section of code places sketch symbols

 '[

Dim oSketchedSymbolDef As SketchedSymbolDefinition

Dim oTG As TransientGeometry

oTG = ThisApplication.TransientGeometry

i_y = 1 'Set variables for x and y positions of pattern

i_x = 1

i_count = 0

For i_y = 1 To Row_Qty 'Create loop for rows

    y_pos = i_y * Row_Spacing_Actual ' Set row spacing increment

    For i_x = 1 To Col_Qty 'Create loop for columns

        x_pos = i_x * Col_Spacing_Actual 'Set column spacing increment

        Try 'the following code creates a new sketched symbol definition, assuming an error here means it already exists.

        oSketchedSymbolDef = oDrawDoc.SketchedSymbolDefinitions.Add("CADline_Callout" & (start_value + i_count))

        ' Open the sketched symbol definition's sketch for edit. This is done by calling the Edit

        ' method of the SketchedSymbolDefinition to obtain a DrawingSketch. This actually creates

        ' a copy of the sketched symbol definition's and opens it for edit.

        Dim oSketch As DrawingSketch

        Call oSketchedSymbolDef.Edit(oSketch)

        Dim oSketchCircle As SketchCircle

        If (start_value + i_count) < 100 Then 'Place circle in sketch definition (with larger size if value it contains is larger than 99)

            oSketchCircle = oSketch.SketchCircles.AddByCenterRadius(oTG.CreatePoint2d(20, 20), 0.5)

            Else

            oSketchCircle = oSketch.SketchCircles.AddByCenterRadius(oTG.CreatePoint2d(20, 20), 0.7)

        End If

        Dim sText As String 'Create string to put the symbol value into

        sText = (start_value + i_count)

        If (start_value + i_count) < 10 Then ' Change position of placed sketch text depending on whether it is 1, 2 or 3 digits.

        oTextBox = oSketch.TextBoxes.AddFitted(oTG.CreatePoint2d(19.82, 20.25), sText)

        Else If (start_value + i_count) < 100 Then

        oTextBox = oSketch.TextBoxes.AddFitted(oTG.CreatePoint2d(19.60, 20.25), sText)

        Else

        oTextBox = oSketch.TextBoxes.AddFitted(oTG.CreatePoint2d(19.40, 20.25), sText)

        End If

        oStyle = oTextBox.Style 'Set properties of sketch text

        oStyle.Font = "Tahoma"

        oStyle.FontSize = 0.5

        oSketchedSymbolDef.ExitEdit 'Exit sketch symbol edit

        Catch 'Do nothing if there was an error with the above

        End Try

        ' Obtain a reference to the desired sketched symbol definition.

        oSketchedSymbolDef = oDrawDoc.SketchedSymbolDefinitions.Item(("CADline_Callout" & (start_value + i_count)))

        '

        Dim oSheet As Sheet

        oSheet = oDrawDoc.ActiveSheet

        '

        oATG = ThisApplication.TransientGeometry

        '

        Dim oSketchedSymbol As SketchedSymbol 'Set position of first placed sketched symbol

        oSketchedSymbol = oSheet.SketchedSymbols.Add(oSketchedSymbolDef, oATG.CreatePoint2d((20 + x_pos), (40 - y_pos)), (0), 1,)

        i_count = i_count+1

     Next

Next

']