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inventor 12 multiple hole tables in drawing

Message 1 of 8
3483 Views, 7 Replies

inventor 12 multiple hole tables in drawing

I put in 3 seperate hole tables in a drawing, labeld one counter bore holes, one dowel hles and one jack screws.  used the selection hole method and all the tags were the same starting with A1 ...


Any way to control multiple hole tables so they use different tag numbers

Message 2 of 8

You can manually edit the hole tags and have them update in the table. If the holes are the same size and type, you may consider using the rollup feature in the edit table dialogue to reduce the number of unique tags. I've attached an example for your review.



Nathan Chandler
Principal Specialist
Message 3 of 8

had a bit of trouble reading files,  said it was created in a new version. I haven't updated my inv. 2012 yet to any service packs. any ideas how to do that.



Message 4 of 8
in reply to: DaleDavis3738

Hi Dale

Have you tried the way to create a hole table including all of those holes, then split the hole table?  Make sure you check the option to group hole type, then it will be easy to spilt them into three tables as you want.


It will be helpful to solve your problem on tag,  since it only support tagging according to hole position OR hole size, maybe it's a little different with your requirement, but I thought it still could save efforts on retagging.

Split a hole table

You can split a hole table into two sections. After creating the sections, you can move each section independently of the other.

  1. In the graphics window, click to select the hole table.
  2. Right-click the row where the table is to split and select TableSplit from the menu. The sections of the split table are placed in vertical alignment.


Hole Table-Group.png

Jingyi Liu

Inventor Product Manager
Tags (1)
Message 5 of 8
in reply to: jingyi.liu




Try this solution here. Its some iLogic code to auto renumber 1.1, 1.2, 1.3. Then 2.1, 2.2, 2.3 etc.



Message 6 of 8

Try running this ilogic. It is a modified version of what @LukeDavenport suggested. Except it identifies each hole by 'A1' format and Increments to 'B1' for table 2, so on. 


SyntaxEditor Code Snippet

' Start of iLogic code.....

' This iLogic code will renumber hole tags for all hole tables in all sheets of the active drawing
        ' Define document
        Dim oDoc As DrawingDocument
        ' Is the currently active document a drawing?
            oDoc = ThisApplication.ActiveDocument
            MsgBox("This rule can only be run in a drawing document")
        End Try
        ' Define Variables....
        Dim oSheets As Inventor.Sheets = oDoc.Sheets
        Dim oSheet As Sheet = Nothing
        Dim RowNo As Integer
        Dim oTable As HoleTable
        Dim HoleTableNo As Integer = 1
        Dim SheetNo As Integer = 1
        Dim Letter As String = "A"
        ' Loop through all sheets
        For Each oSheet In oSheets
            ' Loop through all holetables
            For Each oTable In oSheet.HoleTables
                ThisApplication.StatusBarText = "Sheet " & SheetNo & ". Processing Hole Table No. " & HoleTableNo & "...."
                ' Loop through all rows in hole table
                For RowNo = 1 To oTable.HoleTableRows.Count
                    ' Change hole tag for this row in table
                    oTable.HoleTableRows.Item(RowNo).HoleTag.Text = Letter &  RowNo
                'Increment Alphabet for each hole table
                Letter = Chr(Asc(Letter)+1)
            SheetNo += 1


Message 7 of 8

Is there any way that I can ID holes similar to how Inventor already does it?
For example, I have 4 different types of holes on a table on sheet one of a DWG, they are labeled A1, B1, C1, D1.

I am wondering if there is a way to have iLogic do this across sheets and have the next hole table on sheet 2 pick up at E1? It would also be nice if every subsequent sheet would pick up where the last sheet left off.

Message 8 of 8
in reply to: npachecoMR3YB

i answered the question on the new thread.

Jelte de Jong
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