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Make all values in a revision block non static
Hello All,
For some reason, for the last few releases, updating properties from Vault has updated our rev block (we use vault rev blocks) correctly, however, the operation adds the correct values to the rev block and then leaves everything static.
Is there a way to use ilogic to change all of the cells to Not Static?
I have found a snippet (thanks @jdkriek and @cbenner) that will make them all static, but my programming capability does not allow me to reverse it.
Here is the snippet:
Dim oDrawDoc As DrawingDocument = ThisApplication.ActiveDocument ' Get the revision table Dim oRevTable As RevisionTable = oDrawDoc.ActiveSheet.RevisionTables.Item(1) ' Get last row Dim oRow As RevisionTableRow oRow = oRevTable.RevisionTableRows.Item(oRevTable.RevisionTableRows.Count) ' Make sure we have the active row If oRow.IsActiveRow Then ' Go through all columns in that row For i = 1 To oRevTable.RevisionTableColumns.Count Dim oCell As RevisionTableCell = oRow.Item(i) ' Set all cells to static oCell.Text = oCell.Text Next End If
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wouldn't making them non static mean that the earlier version-lines will get updated to the last revision status?
Kudo's are also appreciated
Succes on your project, and have a nice day
Herm Jan
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To clarify:
My rev block looks like this:
Before
After I un-check Static for all of the cells, it looks like this:
After
What I am after is a way to automate un-checking Static for all the cells in a rev block. If that helps...
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From what I can tell looking at it through the API, there is no direct way to clear the static status of the cells in the Revision table. (neither through an exposed static property, nor through formatted text.
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That is what I was afraid of. It looks like it is available for the partslist but not the rev block: https://forums.autodesk.com/t5/inventor-customization/how-to-get-static-value-in-vba/m-p/6980937/hig...
Thanks for looking into it.
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Unfortunately, Inventor API does not support "static" property for ReviosionTableCell Object. It would be nice to inform at idea station using below link.
https://forums.autodesk.com/t5/inventor-ideas/idb-p/v1232/tab/most-recent
Thanks and regards,
CHANDRA SHEKAR G
Developer Advocate
Autodesk Developer Network

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Hi,
This is default Vault behavior.
if you are using property-mapping in vault to inventor than you don't need the revision table configuration because you use property mapping form vault.
Disable this and you will solve the problem in the base.
And you will always have static values.
regards
Regards,
Arthur Knoors
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found a beautiful way of doing this, you are welcome world.
Dim oDrawDoc As DrawingDocument = ThisApplication.ActiveDocument Dim oSheet As Sheet Dim oRevTable As RevisionTable = oDrawDoc.ActiveSheet.RevisionTables.Item(1) Dim oRows As RevisionTableRows = oRevTable.RevisionTableRows Dim oApp As Inventor.Application = ThisApplication Dim UNDO As Transaction = oApp.TransactionManager.StartGlobalTransaction(oDrawDoc, "Remove Static from Revision Table") P = iProperties.Value("Project", "Revision Number") oRows.Add() Dim oRow As RevisionTableRow = oRevTable.RevisionTableRows.Item(oRevTable.RevisionTableRows.Count) For Each oRow In oRows If oRow.IsActiveRow Then Else oRow.Delete End If Next Dim oCell1 As RevisionTableCell = oRevTable.RevisionTableRows.Item(1).Item(1) Dim sFText As String = oCell1.FormattedText sFText = P'InputBox("What is the Revision?", "RevisionTableCell.FormattedText", P) oCell1.FormattedText = sFText c = "REV" 'just in case it doenst exit recreate it Try : x = iProperties.Value("Custom", c) : Catch : iProperties.Value("Custom", c) = "Job number/Reason Code or ECN #" : End Try iProperties.Value("Custom", c) = sFText iProperties.Value("Project", "Revision Number") = sFText UNDO.End