Ilogic to lock views in drawing
What do you mean by "locking a view". Is this possible in the user interface?
This
And I do not know, but I was hoping that it's possible.
Do you know where I might try looking?
In the API help there's a sample titled "Adding Representation Views" that does just this. I've copied the sample below. The thing you're looking for is the "DesignViewAssociative" option that's being set. That's the equivalent of the chain check box that you referenced in the dialog.
Public Sub AddBaseViewWithRepresentations()
' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
Set oDrawDoc = ThisApplication.ActiveDocument
'Set a reference to the active sheet.
Dim oSheet As Sheet
Set oSheet = oDrawDoc.ActiveSheet
' Create a new NameValueMap object
Dim oBaseViewOptions As NameValueMap
Set oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap
' Set the representations to use when creating the base view.
Call oBaseViewOptions.Add("PositionalRepresentation", "MyPositionalRep")
Call oBaseViewOptions.Add("DesignViewRepresentation", "MyDesignViewRep")
Call oBaseViewOptions.Add("DesignViewAssociative", True)
' Open the model document (corresponding to the "MyLODRep" representation).
Dim strFullDocumentName As String
strFullDocumentName = ThisApplication.FileManager.GetFullDocumentName("C:\tempreps.iam", "MyLODRep")
Dim oModel As Document
Set oModel = ThisApplication.Documents.Open(strFullDocumentName, False)
' Create the placement point object.
Dim oPoint As Point2d
Set oPoint = ThisApplication.TransientGeometry.CreatePoint2d(25, 25)
' Create a base view.
Dim oBaseView As DrawingView
Set oBaseView = oSheet.DrawingViews.AddBaseView(oModel, oPoint, 2, _
kIsoTopLeftViewOrientation, kHiddenLineRemovedDrawingViewStyle, _
, , oBaseViewOptions)
End Sub
#1 Why can't I cut and paste the errors from the Edit Rule Dialog?
#2 'oBaseViewOptions' is not declared. It may be inaccessible due to its protection level.
Now, with the "Call"s and the"Public Sub" and all that, it looks kind of like what you posted is VBA or whatever it's called.
I'm trying to use iLogic.
Maybe that's why nobody ever answers, I put iLogic in the subject line, and everybody thinks, "I could do it with Visual Basic but nobody uses iLogic."
So, thanks but, is there a comparable command that will work in iLogic?
Is there an iLogic help where I could find a similar sample?
Are you thinking what I said "Maybe everybody thinks ..." a few lines ago?
Here's an iLogic rule that demonstrates what you're trying to do. You'll need to change the names of the positional and view reps and also the level of detail. Of course you don't have to use all of those but the sample is just demonstrating all of them.
Thanks for this question. I'm working on a class for Autodesk University regarding iLogic and the Inventor API and you've given me a lot more insight about what I should cover.
Public Sub Main()
' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument
'Set a reference to the active sheet.
Dim oSheet As Sheet
oSheet = oDrawDoc.ActiveSheet
' Create a new NameValueMap object
Dim oBaseViewOptions As NameValueMap
oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap
' Set the representations to use when creating the base view.
oBaseViewOptions.Add("PositionalRepresentation", "Position1")
oBaseViewOptions.Add("DesignViewRepresentation", "View1")
oBaseViewOptions.Add("DesignViewAssociative", True)
' Open the model document (corresponding to the "LevelofDetail1" representation).
Dim strFullDocumentName As String
strFullDocumentName = ThisApplication.FileManager.GetFullDocumentName("C:\temp\reps.iam", "LevelofDetail1")
Dim oModel As Document
oModel = ThisApplication.Documents.Open(strFullDocumentName, False)
' Create the placement point object.
Dim oPoint As Point2d
oPoint = ThisApplication.TransientGeometry.CreatePoint2d(25, 25)
' Create a base view.
Dim oBaseView As DrawingView
oBaseView = oSheet.DrawingViews.AddBaseView(oModel, oPoint, 2, _
ViewOrientationTypeEnum.kIsoTopLeftViewOrientation, _
DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle,,, _
oBaseViewOptions)
End Sub
Ok, your latest response helps a lot. Everything so far has been about creating new drawing views. Not changing the settings for an existing drawing view. Here's a modified version of your rule that should do what you want. You'll need to change the name of the design view to the name of a design view that exists or you can use "Default" which will work in all cases.
Dim oDrawDoc As DrawingDocument = ThisDrawing.Document
For Each oSheet As Sheet In oDrawDoc.Sheets
For Each oView As DrawingView In oSheet.DrawingViews
oView.SetDesignViewRepresentation("View1", True)
Next
Next
Unfortunately, the name of the view rep that was used when the view was initially placed is not available through the API. I know that the dialog shows it so Inventor has stored it but the API doesn't currently expose it. iLogic is built on top of the API so if the API doesn't provide access to something it's not possible for iLogic to provide it either.
If the view isn't associative to a view rep (the box is unchecked) then there isn't any kind of association to that name in the field. The view rep could have even been deleted so it's not always possible to use the name that's in the field. Although I do realize that would not be the normal case and it would be nice to have access to that name to be able to create the association but it's currently just not possible.
Are the names of the design view representations consistent or is there some way by looking at the list of design views in the part or assembly to figure out which design view you need?
Otherwise I don't really see a good solution. You basically need to set the view to a specific design view representation (and this time making it associative so you don't have this same problem in the future). From the API we can make a view associative to a design view but we don't know the name of the design view that was used when the view was created. There is not workaround to get that name.
To summarize:
If you have an existing drawing view that was created using a design view representation but is not associative to the design view representation, there is currently no way to make it associative to that design view representation, if you don't know the name of the design view representation.
When using the API to associate a view with a design view representation you have to supply the name of the design view representation and the name that was used when the view was created is not accessible from the API.
If you know the name of the design view representation you can use the SetDesignViewRepresentation method of the DrawingView object where the first argument is the name of the design view representation and the second argument is if it's to be associative or not.
oView.SetDesignViewRepresentation("View1", True)
It is possible to create a new view using the API that is associated to the design view representation. The VBA code below demonstrates that.
Public Sub Main()
' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument
'Set a reference to the active sheet.
Dim oSheet As Sheet
oSheet = oDrawDoc.ActiveSheet
' Create a new NameValueMap object
Dim oBaseViewOptions As NameValueMap
oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap
' Set the representations to use when creating the base view.
oBaseViewOptions.Add("PositionalRepresentation", "Position1")
oBaseViewOptions.Add("DesignViewRepresentation", "View1")
oBaseViewOptions.Add("DesignViewAssociative", True)
' Open the model document (corresponding to the "LevelofDetail1" representation).
Dim strFullDocumentName As String
strFullDocumentName = ThisApplication.FileManager.GetFullDocumentName("C:\temp\reps.iam", "LevelofDetail1")
Dim oModel As Document
oModel = ThisApplication.Documents.Open(strFullDocumentName, False)
' Create the placement point object.
Dim oPoint As Point2d
oPoint = ThisApplication.TransientGeometry.CreatePoint2d(25, 25)
' Create a base view.
Dim oBaseView As DrawingView
oBaseView = oSheet.DrawingViews.AddBaseView(oModel, oPoint, 2, _
ViewOrientationTypeEnum.kIsoTopLeftViewOrientation, _
DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle,,, _
oBaseViewOptions)
End Sub
Yes, you can place views of the different weldment states. For the AdditionalOptions argument of the AddBaseView method you can pass in a value that specifies which weldment state you want. Below is an example creating a view showing the welds but you can also use kAssemblyFeatureGroup, kMachiningFeatureGroup, or kPreperationsFeatureGroup.
options = ThisApplication.TransientObjects.CreateNameValueMap
options.Add("WeldmentFeatureGroup", WeldmentFeatureGroupEnum.kWeldsFeatureGroup)
view = drawViews.AddBaseView(weldment, tg.CreatePoint2d(10, 10), 0.25, kFrontViewOrientation, kHiddenLineDrawingViewStyle, , , options)
If you have VBA code, you need to add "Call" to the beginning of each of the lines. Anytime you call a method with multiple arguments and enclose them in parentheses you need to use the "Call" statement. In VBA the parentheses are optional but if you use them you have to use Call. VB.NET doesn't need the Call statement but it requires parentheses. Personally, I like parentheses so I use the Call statement in VBA.
