Drawing sheet list with more properties
Hi @kresh.bell . Yes, it is possible. Using the DrawingDocument.Sheets method you can get all your sheets and make a list of them. An example of solving a problem: Link, Link, GitHub.
We can help you implement a more personalized iLogic code if you share with us more information about your case and your needs.
Andrii Humeniuk - CAD Coordinator, Autodesk Certified Instructor
LinkedIn | My free Inventor Addin | My Repositories
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This is ok for me iLogic.
Dim oDoc As DrawingDocument
oDoc = ThisApplication.ActiveDocument
Dim oSheet, oIndexSheet As Sheet
Dim sSheetName, sSheetNo, sSheetRev As String
Dim oTitleBlock As TitleBlock
Dim oTextBox As Inventor.TextBox
oIndexSheet = oDoc.Sheets(1)'In order to put table on sheet 1
'[Table Setup
Dim oColumns, oRows, oCells, i As Integer
oColumns = 3
i = 0
oRows = oDoc.Sheets.Count
oCells = oColumns * oRows 'calculate number of cells
Dim oContents(oCells - 1) As String 'Minus 1 as array will start from zero
Dim oTitles(oColumns - 1) As String 'Minus 1 as array will start from zero
'Hardcoded titles
oTitles(2) = "DESCRIPTION"
oTitles(1) = "SHEET #"
oTitles(0) = "SHEET REV"
']
iCount = 1
For Each oSheet In oDoc.Sheets
sSplit = Split(oSheet.Name, ":")
Try : sSheetName = sSplit(0) : Catch : sSheetName = oSheet.Name : End Try
sSheetNo = iCount
sSheetRev = oSheet.Revision
Try 'to get title block
oTitleBlock = oSheet.TitleBlock
For Each oTextBox In oTitleBlock.Definition.Sketch.TextBoxes
If oTextBox.Text = "SHEET-NAME" Then
Call oTitleBlock.SetPromptResultText(oTextBox, sSheetName)
End If
Next
Catch
'handle error when no title block is on the sheet
End Try
'[Table Data
oContents(i) = sSheetRev 'Add to string
i = i + 1
oContents(i) = sSheetNo 'Add to string
i = i + 1
oContents(i) = sSheetName 'Add to string
i = i + 1
']
iCount = iCount +1
Next
Dim InsP As Point2d
InsP = ThisApplication.TransientGeometry.CreatePoint2d(10, 15)
Dim oCustomTable As CustomTable
oTableName = "DRAWING INDEX"
Try : oIndexSheet.CustomTables.Item(1).Delete : Catch : End Try
oCustomTable = oIndexSheet.CustomTables.Add(oTableName, InsP, oColumns, oRows, oTitles, oContents)
Can I use custom properties from the title block to populate the Description column?
Also Revision number.
Just a tip...
Be careful using a 'For Each...Next' type of loop, with a separate Index counter, if that Index is important. When iterating through a collection that way, the order of that iteration is not guaranteed. If Index is important, then you should use a 'For i = # to #...Next' type of loop. That ensures that the items will be encountered in their 'natural' order. In a drawing, the Sheets collection seems to be ordered a bit differently than most types of collections, because the 'sheet number' will always be in the order they are seen in the model browser tree. If you physically drag the first sheet down to the next position after the current sheet 3, it will become Sheet 3 itself, because the original sheet 2 will become sheet 1, and the original sheet 3 will become sheet 2. The first part of the sheet's name will stay the same, but the Index number is managed automatically by Inventor.
Also, you are likely aware of this, but there is a document level revision level (in the standard iProperties), then there is also a sheet level revision level (Sheet.Revision ). However, sheets do not have their own PropertySets, like Documents do. So, if you have a different model file being referenced on each sheet of your drawing, and have the description of that model file in the title block of that sheet, but want that information to be shown in a table cell on the first sheet, it will be relatively complicated to gather that information in the first place, and will likely be 'static' information within the table cell, instead of 'linked'. Because it would require iterating through each TextBox within the sketch, within the definition of each title block, and somehow knowing which TextBox is for which property (because a TextBox does not have a name), and retrieving its 'Text' value.
Wesley Crihfield
(Not an Autodesk Employee)
If I understood you correctly. Your code should look like this:
Dim oDoc As DrawingDocument
oDoc = ThisApplication.ActiveDocument
Dim oSheet, oIndexSheet As Sheet
Dim sSheetName, sSheetNo, sSheetRev As String
Dim oTitleBlock As TitleBlock
Dim oTextBox As Inventor.TextBox
oIndexSheet = oDoc.Sheets(1)'In order to put table on sheet 1
'[Table Setup
Dim oColumns, oRows, oCells, i As Integer
oColumns = 3
i = 0
oRows = oDoc.Sheets.Count
oCells = oColumns * oRows 'calculate number of cells
Dim oContents(oCells - 1) As String 'Minus 1 as array will start from zero
Dim oTitles(oColumns - 1) As String 'Minus 1 as array will start from zero
'Hardcoded titles
oTitles(2) = "DESCRIPTION"
oTitles(1) = "SHEET NAME"
oTitles(0) = "SHEET №"
']
iCount = 1
For Each oSheet In oDoc.Sheets
sSplit = Split(oSheet.Name, ":")
Try : sSheetName = sSplit(0) : Catch : sSheetName = oSheet.Name : End Try
sSheetNo = iCount
sSheetRev = oSheet.Revision
Try 'to get title block
Dim oTB As TitleBlock = oSheet.TitleBlock
Dim oTextBoxes As TextBoxes = oTB.Definition.Sketch.TextBoxes
For Each oTBox As Inventor.TextBox In oTextBoxes
Dim sData As String = oTB.GetResultText(oTBox)
If Not oTBox.Text = "<DESCRIPTION>" Then Continue For
sSheetRev = oTB.GetResultText(oTBox)
Next
Catch
'handle error when no title block is on the sheet
End Try
'[Table Data
oContents(i) = sSheetNo 'Add to string
i = i + 1
oContents(i) = sSheetName 'Add to string
i = i + 1
oContents(i) = sSheetRev 'Add to string
i = i + 1
']
iCount = iCount +1
Next
Dim InsP As Point2d
InsP = ThisApplication.TransientGeometry.CreatePoint2d(10, 15)
Dim oCustomTable As CustomTable
oTableName = "DRAWING INDEX"
Try : oIndexSheet.CustomTables.Item(1).Delete : Catch : End Try
oCustomTable = oIndexSheet.CustomTables.Add(oTableName, InsP, oColumns, oRows, oTitles, oContents)Andrii Humeniuk - CAD Coordinator, Autodesk Certified Instructor
LinkedIn | My free Inventor Addin | My Repositories
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Sorry for the delay. Changed the 3rd column from the description column to the revision number column and added an additional 4 columns.
Dim oInvApp As Inventor.Application = ThisApplication
Dim oDoc As DrawingDocument = oInvApp.ActiveDocument
Dim oSheet, oIndexSheet As Sheet
Dim sSheetName, sSheetNo, sSheetRev As String
Dim oTitleBlock As TitleBlock
Dim oTextBox As Inventor.TextBox
oIndexSheet = oDoc.Sheets(1)'In order to put table on sheet 1
'[Table Setup
Dim oColumns, oRows, oCells, i As Integer
oColumns = 7
i = 0
oRows = oDoc.Sheets.Count
oCells = oColumns * oRows 'calculate number of cells
Dim oContents(oCells - 1) As String 'Minus 1 as array will start from zero
Dim oTitles(oColumns - 1) As String 'Minus 1 as array will start from zero
'Hardcoded titles
oTitles(6) = "Text4"
oTitles(5) = "Text3"
oTitles(4) = "Text2"
oTitles(3) = "Text1"
oTitles(2) = "REVISION"
oTitles(1) = "SHEET NAME"
oTitles(0) = "SHEET №"
']
iCount = 1
For Each oSheet In oDoc.Sheets
sSplit = Split(oSheet.Name, ":")
Try : sSheetName = sSplit(0) : Catch : sSheetName = oSheet.Name : End Try
sSheetNo = iCount
sSheetRev = oSheet.Revision
'[Table Data
oContents(i) = sSheetNo 'Add to string
i += 1
oContents(i) = sSheetName 'Add to string
i += 1
oContents(i) = sSheetRev 'Add to string
i += 1
oContents(i) = "" 'Add to string Text1
i += 1
oContents(i) = "" 'Add to string Text2
i += 1
oContents(i) = "" 'Add to string Text3
i += 1
oContents(i) = "" 'Add to string Text4
i += 1
']
iCount += 1
Next
Dim InsP As Point2d = oInvApp.TransientGeometry.CreatePoint2d(10, 15)
Dim oCustomTable As CustomTable
oTableName = "DRAWING INDEX"
Try : oIndexSheet.CustomTables.Item(1).Delete : Catch : End Try
oCustomTable = oIndexSheet.CustomTables.Add(oTableName, InsP, oColumns, oRows, oTitles, oContents)Andrii Humeniuk - CAD Coordinator, Autodesk Certified Instructor
LinkedIn | My free Inventor Addin | My Repositories
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Hello,
if you add a revision label to the sheet, it will be overwritten in the revision table.
