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
Solved! Go to Solution.
Solved by JelteDeJong. Go to Solution.
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.
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.
Dale
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.
You can split a hole table into two sections. After creating the sections, you can move each section independently of the other.
Hi
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.
https://www.cadlinecommunity.co.uk/hc/en-us/articles/202907191
Thanks,
Luke
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? Try oDoc = ThisApplication.ActiveDocument Catch MsgBox("This rule can only be run in a drawing document") Return 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 Next 'Increment Alphabet for each hole table Letter = Chr(Asc(Letter)+1) Next SheetNo += 1 Next
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.
i answered the question on the new thread.
Jelte de Jong
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