How to determine what is included in a Drawing Section View that has a section depth?

[wfajber]

I am not sure how to proceed in this rule to place some automated leaders in a drawing view. The leaders point to WorkPoints in the assembly file that fit a specific naming convention.  It works unless the view is a section view, and the depth of the section view is short enough that some of the workpoints are in the field of view, but should not be included because they are farther away than the section depth.

The specifics of my problem is that I have a large assembly of outdoor equipment that is all mounted on independent concrete foundations. At the early stages of the project, the same part file is used for many of the concrete pieces. In order to identify the concrete foundations, I came up with the idea of adding a named workpoints, ie a workpoint with a specific naming convention.  In this case workpoints are named WPFTG-N-0001, WPFTG-N-0002, etc. 

I find the assembly file by getting the referenced document for the view. I scan the assembly file and find the workpoints with names that contain the string "WPFTG-N" and add them to a collection.  Then on the drawing view, I add a sketch and add text 0001, 0002 etc on the locations where they are.

This worked great in plan view. I then made a version with a section view where I showed the elevation of of the concrete foundations. This time I got the elevation of the workpoint, added it to some reference value and added a leader with the text. This also worked great in elevation view or an isometric view. I check to ensure that it appears within the boundaries of the view on the sheet. I am happy to this point.

Where I am stuck is when I have a larger assembly. Then I need to create a section view that has a section depth to limit what is seen. In my drawing section, this is a large value like 5m, when my assembly could be 30 meters deep.

Here where things do not work as expected. All of the workpoints are included generating lots of unnecessary leaders in the view. I do not know how to determine if a point should be within the volume shown in the section view, or if it is too far and outside the depth of the section view. The DrawingView has a method to find GetIncludeStatus, but my experiment with checking this value show the Include Status as true, and the rule faithfully

So how do I determine if this workpoint or a point in X,Y,Z space should be included in the section view?

I have included the rule that I have and apologize for the length (and maybe the poor style). I have attached a screen shot of the drawing note leaders pointing to a spot in space where something would show if I had the section view depth set to full. And a view of the assembly and the browser. 

' show elevation of named workpoints as leadernotes

' select a drawing view on a drawing. Goes to the underlying assembly and finds a named point, in the form 

' wpname = "WPFTG-N-001"

' then determines the height of the workpoint, adds a leader with  the elevation of the workpoint/foundation

' since adding leaders, now I am working on sheetspace not drawing view space. No sketch required.

Sub  main()

If ThisApplication.ActiveDocumentType <> Inventor.DocumentTypeEnum.kDrawingDocumentObject Then

MsgBox("This rule needs to run on the drawing file", , "Wrong file warning")

Exit Sub

End If

Dim selectedDrawingView As Inventor.DrawingView

selectedDrawingView = ThisApplication.CommandManager.Pick(Inventor.SelectionFilterEnum.kDrawingViewFilter, "Select a drawing view that needs elevations added as leader notes")

Dim oTG As TransientGeometry = ThisApplication.TransientGeometry

'Dim ftgSketch As Inventor.Sketch =Nothing

'ftgSketch = selectedDrawingView.Sketches.Add()

'ftgSketch.Edit

' expecting to find workpoint name of the form wpname = "WPFTG-N-001"

Dim wpmatchstring As String  = "WPFTG-N-"

Dim foundarray As New ArrayList

Dim foundcount As Integer

foundcount = FindAllTopLevelPointsMatch(selectedDrawingView, wpmatchstring, foundarray) 

If foundcount = 0 Then 

MsgBox("found nothing, early exit")

Exit Sub

End If

Dim inputtext As String

Dim referenceElevation As Double

inputtext= InputBox("Enter the elevation in meters that cooresponds to the assembly zero elevation", "Enter reference elevation", "0")

referenceElevation = CDblAny(Val(inputtext))

'MsgBox("foundcount =" & foundcount, , "debug")

For Each foundpoint As Inventor.WorkPoint In foundarray

'MsgBox("found this point X= " & foundpoint.Point.X & "Y= " & foundpoint.Point.Y)

' convert from model to drawing view coordinate in 2D. Not the same as sheet space coordinates.

Dim PointOnDrawingView As Point2d = selectedDrawingView.ModelToDrawingViewSpace(foundpoint.Point)

' need to check if within the current view boundaries.

If checkwithinview(selectedDrawingView, PointOnDrawingView) Then

Dim nametxt As String

nametxt = foundpoint.Name

numtext = nametxt.Remove(0, wpmatchstring.Length)

Dim elevstr As String

Dim elev As Double 

elev = referenceElevation + foundpoint.Point.Z / 100.0  ' convert from centimeters to meters

elev = Round(elev, 3)

elevstr = elev.ToString("F")

'numtext = "Ftg:" & numtext & vbLf & "Elev:" & elevstr

numtext = "EL " & elevstr

'ftgSketch.TextBoxes.AddFitted(oShtPt1, numtext)

CreateElevationLeader( ActiveSheet.Sheet,  selectedDrawingView, oTG , foundpoint, elevstr )

' we can add a text style to the function here as an option

End If 

Next 

End Sub

' this needs the drawing view, and a string that will match the names of workpoints. It is passed an array that will be modified.

Private Function FindAllTopLevelPointsMatch(selectedDrawingView As Inventor.DrawingView, wpname As String, ByRef foundarray As ArrayList )

Dim oAssyDoc As AssemblyDocument = selectedDrawingView.ReferencedDocumentDescriptor.ReferencedDocument

Dim somethingFound As Boolean = False

' find workpoints that are in the top level of the assembly

For Each oWorkPoint As WorkPoint In oAssyDoc.ComponentDefinition.WorkPoints

If oWorkPoint.Name.Contains(wpname) Then

foundworkpoint = oWorkPoint

foundarray.Add(oWorkPoint)

somethingFound = True

End If

Next

' still to do, change this to traverse occurrences because will still miss subassemblies.

' return size of arraylist

Dim numberOfWorkPoints As Integer

numberOfWorkPoints = foundarray.Count

Return numberOfWorkPoints

End Function  

Private Function CheckWithinView(selectedDrawingView As Inventor.DrawingView, checkthis2Dpoint As Inventor.Point2d)

Dim PointOnSheet As Inventor.Point2d = selectedDrawingView.DrawingViewToSheetSpace(checkthis2Dpoint)

If PointOnSheet.X > selectedDrawingView.Left And PointOnSheet.X< (selectedDrawingView.Left + 2 * (selectedDrawingView.Center.X - selectedDrawingView.Left)) Then

' x is ok

If PointOnSheet.Y < selectedDrawingView.Top And PointOnSheet.Y>(selectedDrawingView.Top - 2 * (selectedDrawingView.Top - selectedDrawingView.Center.Y)) Then

'y is ok too

Return True

End If

End If

Return False

End Function

Public Function CreateElevationLeader(oActiveSheet As Sheet, oDrawingView As DrawingView, oTG As TransientGeometry, targetpoint As Inventor.WorkPoint, elevstr As String)

Dim oLeaderPoints As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection

' place a centermark on the workpoint to tie it to the model location

Dim mypointcenter As Inventor.Centermark = oActiveSheet.Centermarks.AddByWorkFeature(targetpoint, oDrawingView)

mypointcenter.Visible=False  ' can set to invisible if it bothers you

Dim mypointonsheet As Point2d = oDrawingView.ModelToSheetSpace(targetpoint.Point)

oLeaderPoints.Add(oTG.CreatePoint2d(mypointonsheet.X+1, mypointonsheet.Y+1))

'*** Must be the LAST point added to the array. This is the Balloon Leader attachment point.

Dim geoIntent As Inventor.GeometryIntent = oActiveSheet.CreateGeometryIntent(mypointcenter) 

oLeaderPoints.Add(geoIntent)

'*** Create the leader

Dim myLeader As Inventor.LeaderNote

myLeader = oActiveSheet.DrawingNotes.LeaderNotes.Add(oLeaderPoints,elevstr)

End Function

[wfajber]

And I use Inventor Professional 2021 Release 2021.3.3 build 353.

[Michael.Navara]

You can test this code snippet. It calculates the coordinate system of the sectionView in model space and decide if the workpoint is in visible part of model or not. 

Sub Main
	Dim drw As DrawingDocument = ThisDoc.Document
	Dim sectionDrawingView As SectionDrawingView=drw.ActiveSheet.DrawingViews(2)
	Dim workpointsInSectionView = GetPointsInSectionViewWithDepth(sectionDrawingView)

	'TEST
	For Each keyValuePair As KeyValuePair(Of WorkPoint, Boolean) In workpointsInSectionView
		SectionDrawingView.SetIncludeStatus(keyValuePair.Key, keyValuePair.Value)
	Next

End Sub


Function GetPointsInSectionViewWithDepth(sectionDrawingView As SectionDrawingView) As Dictionary(Of WorkPoint, Boolean)
	Dim parentView As DrawingView = sectionDrawingView.ParentView
	Dim sectionDrawingViewDirection As Vector = sectionDrawingView.Camera.Eye.VectorTo(sectionDrawingView.Camera.Target)
	Dim upVector As Vector = sectionDrawingView.Camera.UpVector.AsVector()
	Dim sectionDepth As Double = sectionDrawingView.SectionDepth

	'Build coordinate system by sectionDrawingView
	Dim sectionLineSketch As DrawingSketch = sectionDrawingView.SectionLineSketch
	Dim sectionRootPoint As Point
	For Each sketchLine As SketchLine In sectionLineSketch.SketchLines
		If SketchLine.Reference Then Continue For
		Dim startSketchPoint = SketchLine.StartSketchPoint

		Dim startSketchPointInSheetSpace = sectionLineSketch.SketchToSheetSpace(startSketchPoint.Geometry)
		Dim startSketchPointInModelSpace = parentView.SheetToModelSpace(startSketchPointInSheetSpace).RootPoint
		sectionRootPoint = startSketchPointInModelSpace
		Exit For
	Next

	'Create and setup coordinate system by sectionDrawingView in Model Space
	Dim matrix As Matrix = ThisApplication.TransientGeometry.CreateMatrix()
	Dim origin As Point = sectionRootPoint
	Dim xAxis As Vector = sectionDrawingViewDirection
	Dim yAxis As Vector = upVector
	Dim zAxis As Vector = xAxis.CrossProduct(yAxis)

	matrix.SetCoordinateSystem(origin, xAxis, yAxis, zAxis)

	'Get referenced documents work points
	Dim refDoc As Document = sectionDrawingView.ReferencedDocumentDescriptor.ReferencedDocument
	Dim workPoints As WorkPoints
	If refDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
		workPoints = TryCast(refDoc, PartDocument).ComponentDefinition.WorkPoints
	ElseIf refDoc.DocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
		workPoints = TryCast(refDoc, AssemblyDocument).ComponentDefinition.WorkPoints
	End If

	'Split workpoints by its position in section drawing view 
	'coordinate system in model space.
	'If the X coordinate of the workpoint is greater then 0
	'and less then sectionDepth the wokpoint is in the part of
	'the model which is displayed in section drawing view.

	'This collection contains pairs of all workpoints and information
	'if the workpoint is visible in section view
	Dim workpointsInSectionView = New Dictionary(Of WorkPoint, Boolean)
	For Each workPoint As WorkPoint In workPoints
		Dim point = WorkPoint.Point
		point.TransformBy(matrix)

		Dim isVisible As Boolean = point.X >= 0 And point.X <= sectionDepth
		workpointsInSectionView.Add(WorkPoint, isVisible)
	Next
	Return workpointsInSectionView
End Function

[wfajber]

Thank you very much. I learned a lot just from studying your code.

However it didn't work and I am trying to figure out why.

Question : at line 60 there is this code. I am confused as to WorkPoint vs workPoint.

For Each workPoint As WorkPoint In workPoints
		Dim point = WorkPoint.Point
		point.TransformBy(matrix)

		Dim isVisible As Boolean = point.X >= 0 And point.X <= sectionDepth
		workpointsInSectionView.Add(WorkPoint, isVisible)
	Next

  Isn't workPoint the variable object, instead of the type WorkPoint with a capital W? This is just confusion on my part, because the looping seems to work.

When I added a line to see the status

For Each workPoint As WorkPoint In workPoints
		Dim point = WorkPoint.Point
		point.TransformBy(matrix)

		Dim isVisible As Boolean = point.X >= 0 And point.X <= sectionDepth
		Logger.Info("point called " & WorkPoint.name & " is visible? " & isVisible)
		workpointsInSectionView.Add(workPoint, isVisible)
	Next

Every workpoint said is was not visible. Sample below.

I will study this some more as the answer might be staring me in the face. 

INFO| 24: >>---------------------------
INFO|point called Center Point is visible? False
INFO|point called WPFTG-N-001 is visible? False
INFO|point called WPFTG-N-002 is visible? False
INFO|point called WPFTG-N-003 is visible? False
INFO|point called WPFTG-N-004 is visible? False
INFO|point called WPFTG-N-005 is visible? False
INFO|point called WPFTG-N-006 is visible? False
INFO|point called WPFTG-N-007 is visible? False
INFO|point called WPFTG-N-008 is visible? False

I then edited the line to add some logging and found the log below. The transformed points seem quite different than the original points. The section is parallel to origin the so I would expect similar size quantities for the points.

For Each workPoint As WorkPoint In workPoints
		Dim point = WorkPoint.Point
		Logger.Info("before transform point = " & point.x & " " & point.y & " " & point.z)
		point.TransformBy(matrix)
		Logger.Info("after transform point = " & point.x & " " & point.y & " " & point.z)
		Dim isVisible As Boolean = point.X >= 0 And point.X <= sectionDepth
		Logger.Info("point called " & WorkPoint.Name & " is visible? " & isVisible)
		workpointsInSectionView.Add(WorkPoint, isVisible)

NFO|before transform point = 0 0 0
INFO|after transform point = -84.0668586067791 341.801372342814 11214.2301765166
INFO|point called Center Point is visible? False
INFO|before transform point = 543 -742.5 -70.0000000000145
INFO|after transform point = -326047.653241163 2528887.90716794 10471.7301765165
INFO|point called WPFTG-N-001 is visible? False
INFO|before transform point = 172.242757308213 -435.553216529248 3.80833576709928E-16
INFO|after transform point = -84.0668586067772 802411.328523685 10778.6769599873
INFO|point called WPFTG-N-002 is visible? False
INFO|before transform point = 326.5 -121.5 -50
INFO|after transform point = -232915.199988956 1520729.10071352 11092.7301765165
INFO|point called WPFTG-N-003 is visible? False

[wfajber · Accepted solution]

I did some debugging and fixed my problem. I very much liked the simplicity of Michael's snippet.  But I would like to make some comments to help future readers.

1. matrix transformation needed one more step to translate a point in the global coordinate system to the view coordinate system. That step is to Invert the matrix.

	'Create and setup coordinate system by sectionDrawingView in Model Space
	Dim matrix As Matrix = ThisApplication.TransientGeometry.CreateMatrix()
	Dim origin As Point = sectionRootPoint
	Dim xAxis As Vector = sectionDrawingViewDirection

	Dim yAxis As Vector = upVector
	Dim zAxis As Vector = xAxis.CrossProduct(yAxis)

	matrix.SetCoordinateSystem(origin, xAxis, yAxis, zAxis)
        maxtrix.Invert  ' This line needed to be added to transfrom from the global coord system to the new system.

I also added the check to see if the section view was Full or was a distance. (sorry for the clunky overuse of booleans)

' if the section depth is full then early exit before checking sectionDepth
	If sectionDrawingView.FullSectionDepth Then
		Return True

And I found that the Inventor 2021 iLogic code editor was overly helpful and it sometimes capitalized the names like workpoint into Workpoint. I found it helpful to add an extra letter like oWorkpoint to lower my frustration level.