Hi!
In a drawing, i had include the model skeches.
I have several sketches, and deppending the situation, i need to include or exclude one of the sketches.
Since i can't use the sketch layer visibility on/off, because it will show/ide all the sketches, so the question is.
There's some iLogic code to include/exclude sketches in the drawing views? Or turning the visibility on/off?
Hi Carlos,
The VB.Net code from this blog post should help implement a similar sketch retrieval using iLogic.
Regards,
Balaji
Hi!
I don't need to have in the code the possibility to include the sketches when i create a view.
I have the view already placed in the drawing, and i have all the part sketches already included in the view.
Example:
Let's say the view has two included sketchs; A and B.
Now i want to make an if then else rule to do this:
If parameter=1 then
show included sketch A
Hide included sketch B
elseif parameter=2
hide included sketch A
SHow included sketch B
end if
Hi Carlos,
The code from that blog post can also be used to change the visibility of sketches already included in the drawing view.
Here is an iLogic code example and a recording :
Dim oDrawingDoc As DrawingDocument
oDrawingDoc = ThisDoc.Document
oView = oDrawingDoc.ActiveSheet.DrawingViews(1)
Dim oDoc As Document
oDoc = oView.ReferencedDocumentDescriptor.ReferencedDocument
If oDoc.DocumentType <> kAssemblyDocumentObject Then
MsgBox ("View's Referenced doc needs to be an assembly")
Return
End If
Dim oAssy As AssemblyDocument
oAssy = oView.ReferencedDocumentDescriptor.ReferencedDocument
' Dim oSubOcc As ComponentOccurrence
' For Each oSubOcc In oAssy.ComponentDefinition.Occurrences
'
' If oSubOcc.DefinitionDocumentType = kAssemblyDocumentObject Then
'
' Dim oSubAssyDef As AssemblyComponentDefinition
' Set oSubAssyDef = oSubOcc.Definition
'
' Dim oSketch As PlanarSketch
' Debug.Print (oSubAssyDef.Sketches.Count)
' For Each oSketch In oSubAssyDef.Sketches
'
' Dim oSketchProxy As PlanarSketchProxy
' Call oSubOcc.CreateGeometryProxy(oSketch, oSketchProxy)
'
' Call oView.SetVisibility(oSketchProxy, True)
' Next
' End If
' Next
Dim oAssyDef As AssemblyComponentDefinition
oAssyDef = oAssy.ComponentDefinition
Dim oSketch As PlanarSketch
For Each oSketch In oAssyDef.Sketches
Call oView.SetVisibility(oSketch, False)
If oSketch.Name = "HorizontalSlot" Then
If SlotPosition = "Horizontal" Then
Call oView.SetVisibility(oSketch, True)
End If
End If
If oSketch.Name = "VerticalSlot" Then
If SlotPosition = "Vertical" Then
Call oView.SetVisibility(oSketch, True)
End If
End If
Next
Regards,
Balaji
