Drawing sheet iLogic Question

[ComputerGuru666]

Ok I have 2 questions

1.) If you look at the attached screenshot in the Edit Sheet form there is a sheet "Revision" input field is it possible to fill this out via iLogic?

2.) We have some custom E size sheets (height always 34in width varies 5ft, 6ft, and 8ft) when we select on of these sheet sizes that we created  it will display "Custom Size (inch)" when using the sheet property <sheet size> in the title block not the name of that we gave these sheets (Which creatively enough is "E-5ft", "E-6ft", and "E-8ft"). I thought I had this solved by doing this:

Dim oSheetSize As String

oSheetSize = ActiveSheet.Size

If oSheetSize = "Custom" Then

iProperties.Value("Custom", "SheetSize") = "E"

Else iProperties.Value("Custom", "SheetSize") = oSheetSize

End If

then change the titleblock sheet size field from sheet property <sheet size> to custom drawing properties <SheetSize>

this all works great if there is only 1 sheet in the IDW where it fails is if there is more then one sheet. Any ideas on how to fix this?

Thank you

[Anonymous]

I'd also like to know about the sheet revisions.

[Vladimir.Ananyev]

1. Sheet Revision

Revision information is stored in revision tables.  Each table has one or more revision rows. One column stores revision numbers.  In the following sample rule I assume that revision numbers are located in the second column.  The property Text of the RevisionTableCellObject contains revision number.  You may change it.  This  sample rule changes the revision to “777”.

'Get the active drawing document 
Dim oDrawDoc As DrawingDocument = ThisDrawing.Document
'active sheet
Dim oSheet As Sheet = oDrawDoc.ActiveSheet

'the 1st revision table in a sheet
Dim oTable As RevisionTable = oSheet.RevisionTables.Item(1)

'total number of revision rows
Dim N As Integer = oTable.RevisionTableRows.Count

'the last row in the table
Dim oRow As RevisionTableRow = oTable.RevisionTableRows.Item(N)

‘set new revision (in this sample it is found in 2nd column)

oRow.Item(2).Text = "777"

'read the current revision value 
Dim RevNo As String = oRow.Item(2).Text

If oTable.IsSheetScope Then
   MsgBox( "Sheet Scope.     RevNo = " & RevNo)
Else
   MsgBox( "Drawing Document Scope.     RevNo = " & RevNo)
End If

2. Custom sheet width 

Inventor API Sheet object has property Width that returns sheet width in the base length units (always cm). You may convert this value to ft with a help of UnitsOfMeasure object (as shown below) or via direct conversion.

'UnitsOfMeasure object  
Dim oUOM As UnitsOfMeasure = ThisDrawing.Document.UnitsOfMeasure

Dim SheetWidth As Double =  ActiveSheet.Sheet.Width  ‘in cm !!!
Dim St As String = oUOM.GetPreciseStringFromValue(SheetWidth, "ft")
MsgBox("Sheet format:  E-" & St.Replace(" ",""))

 Cheers,