Base and Projected View Label Name to match Orientation Name

Anonymous · ‎04-26-2012

I would like to know if there is a way to have each view name to be set to the orientation names/ the 3D view cube's name. Is there a way to do this without manually changing each one?

Dennis.Ossadnik · ‎04-30-2012

Hi jbauer,

you could manage this with a little macro like this:

Sub OrientationToLabel()

Dim odoc As DrawingDocument
Set odoc = ThisApplication.ActiveDocument

'active sheet
Dim tmpSheet As Sheet
Set tmpSheet = odoc.ActiveSheet


Dim tmpView As DrawingView
'every draring view

For Each tmpView In tmpSheet.DrawingViews

Dim myDrawingViewName As String


'Which text for which orientation
Select Case tmpView.Camera.ViewOrientationType
    Case ViewOrientationTypeEnum.kBackViewOrientation
        myDrawingViewName = "Back View"
    Case ViewOrientationTypeEnum.kBottomViewOrientation
        myDrawingViewName = "Bottom View"
    Case ViewOrientationTypeEnum.kFrontViewOrientation
        myDrawingViewName = "Front View"
    Case ViewOrientationTypeEnum.kIsoBottomLeftViewOrientation
        myDrawingViewName = "Iso - Bottom Left View"
    Case ViewOrientationTypeEnum.kIsoBottomRightViewOrientation
        myDrawingViewName = "Iso - Bottom Right View"
    Case ViewOrientationTypeEnum.kIsoTopLeftViewOrientation
        myDrawingViewName = "Iso - Top Left View"
    Case ViewOrientationTypeEnum.kIsoTopRightViewOrientation
        myDrawingViewName = "Iso - Top Right View"
    Case ViewOrientationTypeEnum.kLeftViewOrientation
        myDrawingViewName = "Left View"
    Case ViewOrientationTypeEnum.kRightViewOrientation
        myDrawingViewName = "Right View"
    Case ViewOrientationTypeEnum.kTopViewOrientation
        myDrawingViewName = "Top View"
    Case Else
        myDrawingViewName = ""
    End Select

'Chang if view orientation was found
If Not myDrawingViewName = "" Then
    'change drawing view name
    tmpView.Name = myDrawingViewName
End If

Next

End Sub

bofore:

After using the macro:

The macro will change the name of the drawing view of all view on that sheet.

You can adjust the code and replace the names of the orientation with names you like.

Do you think, this would work for you?

Please use the button "Accept as Solution" if it works.

Dennis Ossadnik
Senior Technical Support Specialist

Anonymous · ‎04-30-2012

When I paste this code into the iLogic Browser, I get an error message. I attached a screenshot image of it.

Dennis.Ossadnik · ‎05-02-2012

Hi jbauer,

sorry, i was not aware that you wanted to use it in iLogic. The code above is for using as a macro in VBA.

I changed the code. Now you should be able to use it with iLogic:

Here is the code for iLogic:

Sub Main()

Dim odoc As DrawingDocument
odoc = ThisApplication.ActiveDocument

'active sheet
Dim tmpSheet As Sheet
tmpSheet = odoc.ActiveSheet


Dim tmpView As DrawingView
'every draring view

For Each tmpView In tmpSheet.DrawingViews

Dim myDrawingViewName As String


'Which text for which orientation
Select Case tmpView.Camera.ViewOrientationType
    Case ViewOrientationTypeEnum.kBackViewOrientation
        myDrawingViewName = "Back View"
    Case ViewOrientationTypeEnum.kBottomViewOrientation
        myDrawingViewName = "Bottom View"
    Case ViewOrientationTypeEnum.kFrontViewOrientation
        myDrawingViewName = "Front View"
    Case ViewOrientationTypeEnum.kIsoBottomLeftViewOrientation
        myDrawingViewName = "Iso - Bottom Left View"
    Case ViewOrientationTypeEnum.kIsoBottomRightViewOrientation
        myDrawingViewName = "Iso - Bottom Right View"
    Case ViewOrientationTypeEnum.kIsoTopLeftViewOrientation
        myDrawingViewName = "Iso - Top Left View"
    Case ViewOrientationTypeEnum.kIsoTopRightViewOrientation
        myDrawingViewName = "Iso - Top Right View"
    Case ViewOrientationTypeEnum.kLeftViewOrientation
        myDrawingViewName = "Left View"
    Case ViewOrientationTypeEnum.kRightViewOrientation
        myDrawingViewName = "Right View"
    Case ViewOrientationTypeEnum.kTopViewOrientation
        myDrawingViewName = "Top View"
    Case Else
        myDrawingViewName = ""
    End Select

'Chang if view orientation was found
If Not myDrawingViewName = "" Then
    'change drawing view name
    tmpView.Name = myDrawingViewName
End If

Next

End Sub

Please use the button "Accept as Solution" if it works.

Thanks.

Dennis Ossadnik
Senior Technical Support Specialist

Anonymous · ‎05-02-2012

Thanks for your help,

It's greatly appreciated.

Anonymous · ‎11-07-2013

hi 🙂

work great, but is you have a section in your drawing, put side view in view label name????

Anonymous · ‎02-05-2018

Hey Dennis, nice bit of code - works really well! Would it be difficult to modify it to ignore detail and section views? At the moment if you have any in the drawing they get modified too so you wind up with things like "DETAIL TOP" and "LEFT-LEFT SECTION"!

Cheers,

Kevin

Dennis.Ossadnik · ‎02-05-2018

Hi Kevin,

could you please give this code a try:

VBA:

Sub IDW_OrientationToLabel()

Dim odoc As DrawingDocument
Set odoc = ThisApplication.ActiveDocument

'active sheet
Dim tmpSheet As Sheet
Set tmpSheet = odoc.ActiveSheet


Dim tmpView As DrawingView

For Each tmpView In tmpSheet.DrawingViews

    Dim myDrawingViewName As String
    
    If tmpView.Type = kDrawingViewObject Then
    
        'Which text for which orientation
        Select Case tmpView.Camera.ViewOrientationType
            Case ViewOrientationTypeEnum.kBackViewOrientation
                myDrawingViewName = "Back View"
            Case ViewOrientationTypeEnum.kBottomViewOrientation
                myDrawingViewName = "Bottom View"
            Case ViewOrientationTypeEnum.kFrontViewOrientation
                myDrawingViewName = "Front View"
            Case ViewOrientationTypeEnum.kIsoBottomLeftViewOrientation
                myDrawingViewName = "Iso - Bottom Left View"
            Case ViewOrientationTypeEnum.kIsoBottomRightViewOrientation
                myDrawingViewName = "Iso - Bottom Right View"
            Case ViewOrientationTypeEnum.kIsoTopLeftViewOrientation
                myDrawingViewName = "Iso - Top Left View"
            Case ViewOrientationTypeEnum.kIsoTopRightViewOrientation
                myDrawingViewName = "Iso - Top Right View"
            Case ViewOrientationTypeEnum.kLeftViewOrientation
                myDrawingViewName = "Left View"
            Case ViewOrientationTypeEnum.kRightViewOrientation
                myDrawingViewName = "Right View"
            Case ViewOrientationTypeEnum.kTopViewOrientation
                myDrawingViewName = "Top View"
            Case Else
                myDrawingViewName = ""
            End Select
        
        'Change if view orientation was found
        If Not myDrawingViewName = "" Then
            'change drawing view name
            tmpView.Name = myDrawingViewName
        End If
    
    End If

    myDrawingViewName = ""

Next

End Sub

iLogic:

'active sheet
Dim tmpSheet As Sheet = ThisDrawing.ActiveSheet.Sheet


Dim tmpView As DrawingView

For Each tmpView In tmpSheet.DrawingViews

    Dim myDrawingViewName As String = ""
    
	If tmpView.Type = ObjectTypeEnum.kDrawingViewObject Then
    
        'Which text for which orientation
        Select Case tmpView.Camera.ViewOrientationType
            Case ViewOrientationTypeEnum.kBackViewOrientation
                myDrawingViewName = "Back View"
            Case ViewOrientationTypeEnum.kBottomViewOrientation
                myDrawingViewName = "Bottom View"
            Case ViewOrientationTypeEnum.kFrontViewOrientation
                myDrawingViewName = "Front View"
            Case ViewOrientationTypeEnum.kIsoBottomLeftViewOrientation
                myDrawingViewName = "Iso - Bottom Left View"
            Case ViewOrientationTypeEnum.kIsoBottomRightViewOrientation
                myDrawingViewName = "Iso - Bottom Right View"
            Case ViewOrientationTypeEnum.kIsoTopLeftViewOrientation
                myDrawingViewName = "Iso - Top Left View"
            Case ViewOrientationTypeEnum.kIsoTopRightViewOrientation
                myDrawingViewName = "Iso - Top Right View"
            Case ViewOrientationTypeEnum.kLeftViewOrientation
                myDrawingViewName = "Left View"
            Case ViewOrientationTypeEnum.kRightViewOrientation
                myDrawingViewName = "Right View"
            Case ViewOrientationTypeEnum.kTopViewOrientation
                myDrawingViewName = "Top View"
            Case Else
                myDrawingViewName = ""
            End Select
        
        'Change if view orientation was found
        If Not myDrawingViewName = "" Then
            'change drawing view name
            tmpView.Name = myDrawingViewName
        End If
    
    End If

    myDrawingViewName = ""

Next

Better now?

Dennis Ossadnik
Senior Technical Support Specialist

Anonymous · ‎04-29-2018

Hello,

I have a 'twist' on this thread.

In the model representations you can create views. Is it possible to collect and use the name of the view in the title block of a sheet?

jpchaisson · ‎02-15-2019

Dennis,

im into a problem with your code. when i create the Left View it labels it as Front View and Front View as Right View.

Thanks,

Jeremy

johnsonshiue · ‎02-15-2019

Hi! I guess you may need to check your Style setting and see if the view is based on model XY plane or Front. Open the idw/dwg file and go to Manage -> Styles Editor -> View Preference -> Front View Plane. Is it set to "From Model" or one of the origin planes?

Many thanks!

Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

jpchaisson · ‎02-15-2019

Johnson,

thank you, thats what it is my work computer is set to "XY" and not "From Model".

is there any way i can work around this leaving it set as "XY" ?

Thanks,

Jeremy

johnsonshiue · ‎02-18-2019

Hi! I guess it may work but you will have to modify the code/rule so that it is changing the view you want to change. It can be a bit tricky.

Many thanks!

Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

Anonymous · ‎07-28-2020

I am using this Code and its working well for me. I was just wondering if there was a way to update the rule so that the view label scale is overridden to show NTS for the ISO views? I have tried unsuccessfully.

marcel.coufreur · ‎03-31-2023

Is it normal that you have to "Regenerate All Rules" before this takes effect? Or did i do something wrong?

WCrihfield · ‎04-03-2023

Hi @marcel.coufreur. That should not be needed. However, you may just need to add an extra line of code in there at the end to update the drawing document before you will see the changes. If using an internal iLogic rule, you can use the line:

InventorVb.DocumentUpdate

...for that purpose. Or if using VBA, you would use the variable for the document to update the document, similar to the following, where 'oDoc' is the variable that the DrawingDocument is assigned to:

oDoc.Update

There is also a setting within the Document Settings of drawings, on the Drawing tab, named 'Defer Updates', which may be on (checked). When that is checked, some changes will require you to click the update button before the changes will show on your screen.

https://help.autodesk.com/view/INVNTOR/2022/ENU/?guid=GUID-1E32149E-D99B-4875-AEEC-849A36DE5023

Wesley Crihfield

(Not an Autodesk Employee)

marcel.coufreur · ‎06-15-2023

@WCrihfield Where exactly do I write this? I'm not really familiar with Ilogic.

WCrihfield · ‎06-23-2023

Hi @marcel.coufreur. I am not sure which of the codes above you may be trying to use, but I was referring to an iLogic rule, not a VBA macro. If the code you are using starts with "Sub Main", and ends with "End Sub" (both unquoted), then you would need to put the code to update the document on a line just above the "End Sub". But if your code does not have those terms enclosing the code, you could just put the line of code for updating the document at the very end, on its own line. The "InventorVb.DocumentUpdate" line will only work within an iLogic rule, and will not be recognized in a VBA macro. But both iLogic and VBA would both recognize a line like the following.

ThisApplication.ActiveDocument.Update

But to explain a bit more about the 'regenerate rules' thing, I am not sure there is an official online help page for this, but it is basically used to reconnect parameter recognition within internal iLogic rules. What that means is, when the iLogic rule is an internal one (saved within an Inventor document), and you include the unquoted names of parameters (that exist within that same document) within that rule, that will cause the rule to be triggered to run any time the value of any of those parameters changes. Sometimes either that triggering action, or the rule's ability to recognize that unquoted parameter name as representing a parameter gets broken some reason, clicking that tool will fix that association, recognition, and triggering behavior.

Below is a link to some online help documentation that mentions this.

To Work with Rules in iLogic (and scroll to the heading "Run Rules", where this is mentioned)

You can also see a description of it when you hover your mouse over the Regenerate All Rules button for a while.

When you use that tool, not only will it try to fix any problems, but it will run all of the internal iLogic rules within that document, and within any referenced documents too. So be very careful using that tool while a large assembly may be open on your screen, and it may contain many other components that contain some internal iLogic rules.

Wesley Crihfield

(Not an Autodesk Employee)

marcel.coufreur · ‎08-01-2023

@WCrihfield right now I have this.

Sub Main()

'active sheet
Dim tmpSheet As Sheet = ThisDrawing.ActiveSheet.Sheet


Dim tmpView As DrawingView

For Each tmpView In tmpSheet.DrawingViews

    Dim myDrawingViewName As String = ""
    
	If tmpView.Type = ObjectTypeEnum.kDrawingViewObject Then
    
        'Which text for which orientation
        Select Case tmpView.Camera.ViewOrientationType
            Case ViewOrientationTypeEnum.kBackViewOrientation
                myDrawingViewName = "Achteraanzicht"
            Case ViewOrientationTypeEnum.kBottomViewOrientation
                myDrawingViewName = "Onderaanzicht"
            Case ViewOrientationTypeEnum.kFrontViewOrientation
                myDrawingViewName = "Vooraanzicht"
            Case ViewOrientationTypeEnum.kIsoBottomLeftViewOrientation
                myDrawingViewName = "3D indruk"
            Case ViewOrientationTypeEnum.kIsoBottomRightViewOrientation
                myDrawingViewName = "3D indruk"
            Case ViewOrientationTypeEnum.kIsoTopLeftViewOrientation
                myDrawingViewName = "3D indruk"
            Case ViewOrientationTypeEnum.kIsoTopRightViewOrientation
                myDrawingViewName = "3D indruk"
            Case ViewOrientationTypeEnum.kLeftViewOrientation
                myDrawingViewName = "Linker zijaanzicht"
            Case ViewOrientationTypeEnum.kRightViewOrientation
                myDrawingViewName = "Rechter zijaanzicht"
            Case ViewOrientationTypeEnum.kTopViewOrientation
                myDrawingViewName = "Bovenaanzicht"
            Case Else
                myDrawingViewName = ""
            End Select
        
        'Change if view orientation was found
        If Not myDrawingViewName = "" Then
            'change drawing view name
            tmpView.Name = myDrawingViewName
        End If
    
    End If

    myDrawingViewName = ""

Next

ThisApplication.ActiveDocument.Update

End Sub

But It doesn't automatically update what am I missing?

WCrihfield · ‎08-01-2023

Hi @marcel.coufreur. I slightly edit your code a bit in an attempt to maybe being able to help with the updating. The terms 'ThisDrawing' and 'ThisApplication.ActiveDocument' can potentially be pointing to two different documents in certain situations, so eliminated both terms, and am now using the 'ThisDoc.Document' term to refer to the drawing document in the first two lines, then once I store that document reference to a variable (oDDoc), I use that same document variable at the end, to make sure I am working with the exact same document. I also included a line to update the drawing sheet itself. And I am using an Inventor API method of that document to update it directly, while accepting any errors that might arise, and continue. I am also checking a related Document Setting within that drawing called Defer Updates, and if it is turned ON, that code will turn it OFF. Give this a try, and hopefully it will update better for you.

Sub Main()
	If ThisDoc.Document.DocumentType <> DocumentTypeEnum.kDrawingDocumentObject Then Exit Sub
	Dim oDDoc As DrawingDocument = ThisDoc.Document
	If oDDoc.IsModifiable = False Then
		MsgBox("This drawing is not modifiable.  Exiting rule.", , "")
		Exit Sub
	End If
	If oDDoc.DrawingSettings.DeferUpdates = True Then
		oDDoc.DrawingSettings.DeferUpdates = False
	End If
	Dim oSheet As Inventor.Sheet = oDDoc.ActiveSheet
	Dim oViews As DrawingViews = oSheet.DrawingViews
	For Each oView As DrawingView In oViews
		Select Case oView.Camera.ViewOrientationType
		Case ViewOrientationTypeEnum.kBackViewOrientation
			oView.Name = "Achteraanzicht"
		Case ViewOrientationTypeEnum.kBottomViewOrientation
			oView.Name = "Onderaanzicht"
		Case ViewOrientationTypeEnum.kFrontViewOrientation
			oView.Name = "Vooraanzicht"
		Case ViewOrientationTypeEnum.kIsoBottomLeftViewOrientation
			oView.Name = "3D indruk"
		Case ViewOrientationTypeEnum.kIsoBottomRightViewOrientation
			oView.Name = "3D indruk"
		Case ViewOrientationTypeEnum.kIsoTopLeftViewOrientation
			oView.Name = "3D indruk"
		Case ViewOrientationTypeEnum.kIsoTopRightViewOrientation
			oView.Name = "3D indruk"
		Case ViewOrientationTypeEnum.kLeftViewOrientation
			oView.Name = "Linker zijaanzicht"
		Case ViewOrientationTypeEnum.kRightViewOrientation
			oView.Name = "Rechter zijaanzicht"
		Case ViewOrientationTypeEnum.kTopViewOrientation
			oView.Name = "Bovenaanzicht"
		Case Else
		End Select
	Next 'oView
	'update the sheet
	oSheet.Update
	'update the drawing, True = accept any errors and continue
	oDDoc.Update2(True)
End Sub

...and by the way, that 'Defer Updates' setting can be found manually by going to the Tools tab > Options panel > click the Document Settings tool, activate the Drawing tab within that dialog, and there is a checkbox for that setting near the top left of that dialog.

If this solved your problem, or answered your question, please click ACCEPT SOLUTION .
Or, if this helped you, please click (LIKE or KUDOS) 👍.

Wesley Crihfield

(Not an Autodesk Employee)

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Base and Projected View Label Name to match Orientation Name

Base and Projected View Label Name to match Orientation Name

Base and Projected View Label Name to match Orientation Name