I can't seem to work out how to add the view label property 'View Identifier' to a view label using ilogic. I can add part iproperties just fine, but this one is allusive.
It needs to be the linked parameter like when a view is created, not a copy of the string.
I wish we had something like this to work with.
https://forums.autodesk.com/t5/inventor-ideas/capture-ilogic-drawing-annotation-code-directly-from-o...
@andrewdroth , I had an example for extracting view label code on here at one point. I think one of these "archived" links might be it, but can't tell. Maybe @Tarek_K can bring them back. Tarek can you please take a look when you have a chance:
In the mean time let me dig through my examples and see it I have a copy of this, if not I'll recreate it... if someone doesn't beat me to it.
@andrewdroth, okay I didn't find what I was looking for but threw this together from memory and another example.
Post back if this isn't what you're after.
Hope this helps,
Curtis
use this utility rule to extract the formatted text, for use in your real rule
Dim oView As DrawingView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select View") oStringScale = oView.Label.FormattedText InputBox("Copy this formatted text", "iLogic", oStringScale)
And then you can use the extracted formatted text to do something like this to set the view string
Dim oViews As DrawingViews Dim oView As DrawingView For Each oSheet As Sheet In ThisDoc.Document.Sheets oViews = oSheet.DrawingViews For Each oView In oViews oView.ShowLabel = True oViewString = "<DrawingViewName/>" & "<Br/>" & "Hello World" 'add to the view label oView.Label.FormattedText = oViewString Next Next
Here is some help info on Formatted Text... it's really buried in the API help, so you kinda' gott'a "know it's there to know it's there" but it's something to be aware of as well. https://help.autodesk.com/view/INVNTOR/2025/ENU/?guid=GUID-915B75BA-4696-4fc7-A2C6-54B2BACDE7E1
Also, keep in mind you can add style overrides, etc, and then the previous utility rule will extract that formatting for you... for the most part ( just noticed the color override didn't extract).
Excellent, that is exactly what I was looking for. Thank you!
Note - even if it seems not needed already anymore but the referred topics are back @Curtis_Waguespack
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Tarek Khodr
Community Manager
Hi @harshkumar_patelGP698. This was sort of shown within the second portion of Curtis' earlier reply (Message 4), but you would have to set the DrawingView.ShowLabel property to True or False. Below is another example code which iterates through each sheet, then each view on each sheet, and makes sure the view label is shown. There are some settings which help with where it will be located by default when it first shows, but we can also move its location if needed (DrawingView.Label.Position property).
Dim oDDoc As DrawingDocument = TryCast(ThisDoc.Document, Inventor.DrawingDocument)
If oDDoc Is Nothing Then Return
Dim oActvSheet As Inventor.Sheet = oDDoc.ActiveSheet
For Each oSheet As Inventor.Sheet In oDDoc.Sheets
oSheet.Activate()
For Each oView As DrawingView In oSheet.DrawingViews
oView.ShowLabel = True
Next
Next
oActvSheet.Activate()
Wesley Crihfield
(Not an Autodesk Employee)
