iLogic rule to switch Revision Table sizes defined in Styles

[Greatwhitenorth]

Hi. 

I'm hoping someone can help with this.  I have a rule in the .idw drawing template, that displays a dialog box asking for the size (A, B, C, D...).  Once the size is selected, it displays the appropriate border and title block.  There is a small & large title block, so an A or B size gets the small, and a C or larger gets the large.  This works great.

My question is, how can I have the appropriately sized Revision Table (small or large), automatically ready for use, based on the drawing size?  The (2) Revision Tables are defined in the Styles library.

Thanks in advance.

Bob

[Greatwhitenorth]

Can anybody help with this?

TIA

[lynlaysaymo]

of thread - but I have a similar issue.

I have 2 different revision tables and need to be able to swap them out via illogic.

Has anyone done something similar?

TIA

[MechMachineMan · Accepted solution]

Yes, there is a way

RevisionTable.Style Property
Parent Object: RevisionTable
Description 
Property that gets and sets the style associated with this object.
Syntax 
RevisionTable.Style() As RevisionTableStyle

[Curtis_Waguespack]

---

@lynlaysaymo wrote:

of thread - but I have a similar issue.

I have 2 different revision tables and need to be able to swap them out via illogic.

Has anyone done something similar?

TIA

---

Hi lynlaysaymo,

Here is an example that toggles between two named rev table styles.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Dim oDrawDoc As Inventor.DrawingDocument = ThisApplication.ActiveEditDocument
'set rev block style	
Dim oRevTable As RevisionTable	
Dim oRevStyle1 As RevisionTableStyle
oRevStyle1 = oDrawDoc.StylesManager.RevisionTableStyles.Item("RevBlock Style1")
Dim oRevStyle2 As RevisionTableStyle
oRevStyle2 = oDrawDoc.StylesManager.RevisionTableStyles.Item("RevBlock Style2")	

Dim oCurrentNumber  As Sheet
oCurrentNumber = oDrawDoc.ActiveSheet

For Each oSheet In oDrawDoc.Sheets
oSheet.Activate

	Try ' Get the revision table 
		oRevTable = oDrawDoc.ActiveSheet.RevisionTables.Item(1)
		
		'toggle rev style
		If oRevTable.Style.Name = "RevBlock Style1" Then
			oRevTable.Style = oRevStyle2
		Else 
			oRevTable.Style = oRevStyle1
		End If
				
		oSheet.Update
		
	Catch 'catch error
		Return 'exit when no rev table is found
	End Try	

Next 'sheet

[lynlaysaymo]

thanks guys works well, cant accept as solution as I hijacked an old thread 😞

[Curtis_Waguespack · Accepted solution]

Here's a quick update to the last rule I posted.

That one exited the rule if no rev block was found on a sheet, rather than skipping the sheet and moving on to the next one.

This one behaves as expected:

Dim oDrawDoc As Inventor.DrawingDocument = ThisApplication.ActiveEditDocument
'set rev block style	
Dim oRevTable As RevisionTable	
Dim oRevStyle1 As RevisionTableStyle
oRevStyle1 = oDrawDoc.StylesManager.RevisionTableStyles.Item("RevBlock Style1")
Dim oRevStyle2 As RevisionTableStyle
oRevStyle2 = oDrawDoc.StylesManager.RevisionTableStyles.Item("RevBlock Style2")	

Dim oCurrentNumber  As Sheet
oCurrentNumber = oDrawDoc.ActiveSheet

For Each oSheet In oDrawDoc.Sheets
oSheet.Activate

	Try ' Get the revision table 
		oRevTable = oDrawDoc.ActiveSheet.RevisionTables.Item(1)
		
		'toggle rev style
		If oRevTable.Style.Name = "RevBlock Style1" Then
			oRevTable.Style = oRevStyle2
		Else 
			oRevTable.Style = oRevStyle1
		End If
				
		oSheet.Update
		
	Catch 'catch error
		Continue For move on  when no rev table is found
	End Try	

Next 'sheet

oCurrentNumber.Activate