Hello together,
is there a way to calculate the axial alignment of holes to see if they fit?
Thank you very much
Georg
Axial alignment of holes
Hi @GeorgK,
You mean, need to delete WorkAxis?
Thanks and regards,
CHANDRA SHEKAR G
Developer Advocate
Autodesk Developer Network
your code for checking all holes is really a time saver. The axis are very good to see the alignment. If the holes are in red or green and with a number with the clientgraphis this would improve the process to find it.
Public Sub SetFaceColor()
Dim partDoc As PartDocument
Set partDoc = ThisApplication.ActiveDocument
' Check to see if the client graphics already exist and delete them if they do.
On Error Resume Next
Dim graphics As ClientGraphics
Set graphics = partDoc.ComponentDefinition.ClientGraphicsCollection.Item("ColorTest")
If Err.Number = 0 Then
graphics.Delete
ThisApplication.ActiveView.Update
Exit Sub
End If
On Error GoTo 0
Dim selectedFace As face
Set selectedFace = ThisApplication.CommandManager.Pick(kPartFaceFilter, "Select a face")
' They don't exist so create them.
Set graphics = partDoc.ComponentDefinition.ClientGraphicsCollection.Add("ColorTest")
Dim node As GraphicsNode
Set node = graphics.AddNode(1)
' Create surface graphics using the selected face.
Dim surfGraphics As SurfaceGraphics
Set surfGraphics = node.AddSurfaceGraphics(selectedFace)
' Set the priority so that it will display on top of the real face.
surfGraphics.DepthPriority = 3
' Define the color using rgb values.
surfGraphics.Color = ThisApplication.TransientObjects.CreateColor(255, 10, 10, 1)
' Refresh the view.
ThisApplication.ActiveView.Update
End Sub
http://modthemachine.typepad.com/my_weblog/2012/03/clientgraphics-text-on-each-planar-face.html
http://modthemachine.typepad.com/my_weblog/2012/03/surfacegraphics-select-primitives.html
At the end there should be a table with all aligned holes. Is it possible to find holes which are not alignet in a radius from 1mm to other holes?
The table could be a text-file or ClientGraphicsText.
Public Sub ClientGraphicsText()
' Set a reference to the document. This will work with
' either a part or assembly document.
Dim oDoc As Document
Set oDoc = ThisApplication.ActiveDocument
' Set a reference to the component definition.
Dim oCompDef As ComponentDefinition
Set oCompDef = oDoc.ComponentDefinition
' Attempt to get the existing client graphics object. If it exists
' delete it so the rest of the code can continue as if it never existed.
Dim oClientGraphics As ClientGraphics
On Error Resume Next
Set oClientGraphics = oCompDef.ClientGraphicsCollection.Item("Text Test")
If Err.Number = 0 Then
oClientGraphics.Delete
End If
On Error GoTo 0
ThisApplication.ActiveView.Update
' Create a new ClientGraphics object.
Set oClientGraphics = oCompDef.ClientGraphicsCollection.Add("Text Test")
' Create a graphics node.
Dim oNode As GraphicsNode
Set oNode = oClientGraphics.AddNode(1)
' Create text graphics.
Dim oTextGraphics As TextGraphics
Set oTextGraphics = oNode.AddTextGraphics
' Set the properties of the text.
oTextGraphics.Text = "This is the sample text. 123"
oTextGraphics.Anchor = ThisApplication.TransientGeometry.CreatePoint(0, 0, 0)
oTextGraphics.Bold = True
oTextGraphics.Font = "Arial"
oTextGraphics.FontSize = 40
oTextGraphics.HorizontalAlignment = kAlignTextLeft
oTextGraphics.Italic = True
Call oTextGraphics.PutTextColor(0, 255, 0)
oTextGraphics.VerticalAlignment = kAlignTextMiddle
' Update the view to see the text.
ThisApplication.ActiveView.Update
End Sub
If System.IO.File.Exists("c:\Temp\Bohrungen.txt") Then
System.IO.File.Delete("c:\Temp\Bohrungen.txt")
End If
Dim file As System.IO.StreamWriter
file = My.Computer.FileSystem.OpenTextFileWriter("c:\Temp\Bohrungen.txt", True)
..........................
..........................
If Math.Round(dia1, 4) = Math.Round(dia2, 4) Then
Debug.Print("Hole diameter of plate 1 = " & dia1 & " compared with Hole diameter of plate 2 = " & dia2 & " => OK - Default")
file.WriteLine("Hole diameter of plate 1 = " & "Ø" & dia1 & " - " & oHoleFeature1.ExtendedName & " compared with Hole diameter of plate 2 = " & "Ø" & dia2 & " - " & oHoleFeature2.ExtendedName & " => OK - Default")
ElseIf Math.Round(dia1, 4) >= Math.Round(dia2, 4) And Math.Round(dia1, 4) <= Math.Round(dia2, 4) + 0.5 Then
Debug.Print("Hole diameter of plate 1 = " & dia1 & " compared with Hole diameter of plate 2 = " & dia2 & " => OK - Special Type")
file.WriteLine("Hole diameter of plate 1 = " & "Ø" & dia1 & " - " & oHoleFeature1.ExtendedName & " compared with Hole diameter of plate 2 = " & "Ø" & dia2 & " - " & oHoleFeature2.ExtendedName & " => OK - Special Type")
Else
Debug.Print("Hole diameter of plate 1 = " & dia1 & " compared with Hole diameter of plate 2 = " & dia2 & " => Not OK")
file.WriteLine("Hole diameter of plate 1 = " & "Ø" & dia1 & " - " & oHoleFeature1.ExtendedName & " compared with Hole diameter of plate 2 = " & "Ø" & dia2 & " - " & oHoleFeature2.ExtendedName & " => Not OK")
End If
m_Inventor.StatusBarText = "Ausgabe in c:\Temp\Bohrungen.txt"
file.Close()
Process.Start("c:\Temp\Bohrungen.txt"
To check all the hole variations is very complex. How could I check if there is any srew or pin etc. in the hole and get the name? Do I need to use the AnalyzeInterference or is there any other possibility?
Georg
Hi @GeorgK,
Try the following VB.net code which lists all aligned and misaligned hole. It also writes to text file.
Private Sub Body_Faces()
Dim m_Inventor As Inventor.Application
m_Inventor = System.Runtime.InteropServices.Marshal.GetActiveObject("Inventor.Application")
If System.IO.File.Exists("c:\Temp\Bohrungen.txt") Then
System.IO.File.Delete("c:\Temp\Bohrungen.txt")
End If
Dim file As System.IO.StreamWriter
file = My.Computer.FileSystem.OpenTextFileWriter("c:\Temp\Bohrungen.txt", True)
Dim oDoc As AssemblyDocument
oDoc = m_Inventor.ActiveDocument
Dim oCompdef As AssemblyComponentDefinition
oCompdef = oDoc.ComponentDefinition
Dim oBody1 As SurfaceBody
Dim oBody2 As SurfaceBody
oBody1 = m_Inventor.CommandManager.Pick(SelectionFilterEnum.kPartBodyFilter, "Select first body")
oBody2 = m_Inventor.CommandManager.Pick(SelectionFilterEnum.kPartBodyFilter, "Select a body to compare")
Dim oFace1 As Face
Dim oFace2 As Face
Dim oFaceColl1 As ObjectCollection
oFaceColl1 = m_Inventor.TransientObjects.CreateObjectCollection()
Dim oFaceColl2 As ObjectCollection
oFaceColl2 = m_Inventor.TransientObjects.CreateObjectCollection()
Dim oAxis1 As WorkAxis
Dim oAxisColl1 As ObjectCollection
oAxisColl1 = m_Inventor.TransientObjects.CreateObjectCollection()
Dim oAxis2 As WorkAxis
Dim oAxisColl2 As ObjectCollection
oAxisColl2 = m_Inventor.TransientObjects.CreateObjectCollection()
For Each oFace1 In oBody1.Faces
If oFace1.SurfaceType = SurfaceTypeEnum.kCylinderSurface Then
oAxis1 = oCompdef.WorkAxes.AddFixed(oFace1.Geometry.BasePoint, oFace1.Geometry.AxisVector)
If IsAxisDuplicate(oAxis1, oAxisColl1) = False Then
oAxisColl1.Add(oAxis1)
oFaceColl1.Add(oFace1)
Else
oAxis1.Delete()
End If
End If
Next
For Each oFace2 In oBody2.Faces
If oFace2.SurfaceType = SurfaceTypeEnum.kCylinderSurface Then
oAxis2 = oCompdef.WorkAxes.AddFixed(oFace2.Geometry.BasePoint, oFace2.Geometry.AxisVector)
If IsAxisDuplicate(oAxis2, oAxisColl2) = False Then
oAxisColl2.Add(oAxis2)
oFaceColl2.Add(oFace2)
Else
oAxis2.Delete()
End If
End If
Next
For i As Integer = 1 To oAxisColl1.Count
oAxis1 = oAxisColl1.Item(i)
Dim j As Integer = 0
j = CompareAlignment(oAxis1, oAxisColl2)
If j > 0 Then
oFace1 = oFaceColl1.Item(i)
oFace2 = oFaceColl2.Item(j)
CompareFace(oFace1, oFace2, file)
oFace1.AttributeSets.Add("Aligned")
oFace2.AttributeSets.Add("Aligned")
End If
Next
For Each oFace1 In oFaceColl1
If oFace1.AttributeSets.Count = 0 Then
Dim oHoleFeature As HoleFeature
oHoleFeature = oFace1.CreatedByFeature
Dim dia As Double
dia = oHoleFeature.HoleDiameter.Value * 10 ' Converting cm to mm
file.WriteLine("Hole diameter of plate 1 = " & "Ø" & dia & " - " & oHoleFeature.ExtendedName & " => misaligned")
End If
Next
For Each oFace2 In oFaceColl2
If oFace2.AttributeSets.Count = 0 Then
Dim oHoleFeature As HoleFeature
oHoleFeature = oFace2.CreatedByFeature
Dim dia As Double
dia = oHoleFeature.HoleDiameter.Value * 10 ' Converting cm to mm
file.WriteLine("Hole diameter of plate 2 = " & "Ø" & dia & " - " & oHoleFeature.ExtendedName & " => misaligned")
End If
Next
CleanAxis(oAxisColl1)
CleanAxis(oAxisColl2)
m_Inventor.StatusBarText = "Ausgabe in c:\Temp\Bohrungen.txt"
file.Close()
Process.Start("c:\Temp\Bohrungen.txt")
End Sub
Public Sub CleanAxis(ByVal oAxisColl As ObjectCollection)
For Each oAxis As WorkAxis In oAxisColl
oAxis.Delete()
Next
End Sub
Public Sub CompareFace(ByVal oFace1 As Face, ByVal oFace2 As Face, ByVal file As System.IO.StreamWriter)
Dim oHoleFeature1 As HoleFeature
oHoleFeature1 = oFace1.CreatedByFeature
Dim dia1 As Double
dia1 = oHoleFeature1.HoleDiameter.Value
dia1 = dia1 * 10 'Converting cm to mm
Dim oHoleFeature2 As HoleFeature
oHoleFeature2 = oFace2.CreatedByFeature
Dim dia2 As Double
dia2 = oHoleFeature2.HoleDiameter.Value
dia2 = dia2 * 10 'Converting cm to mm
If Math.Round(dia1, 4) = Math.Round(dia2, 4) Then
Debug.Print("Hole diameter of plate 1 = " & dia1 & " compared with Hole diameter of plate 2 = " & dia2 & " => OK - Default")
file.WriteLine("Hole diameter of plate 1 = " & "Ø" & dia1 & " - " & oHoleFeature1.ExtendedName & " compared with Hole diameter of plate 2 = " & "Ø" & dia2 & " - " & oHoleFeature2.ExtendedName & " => OK - Default")
ElseIf Math.Round(dia1, 4) >= Math.Round(dia2, 4) And Math.Round(dia1, 4) <= Math.Round(dia2, 4) + 0.5 Then
Debug.Print("Hole diameter of plate 1 = " & dia1 & " compared with Hole diameter of plate 2 = " & dia2 & " => OK - Special Type")
file.WriteLine("Hole diameter of plate 1 = " & "Ø" & dia1 & " - " & oHoleFeature1.ExtendedName & " compared with Hole diameter of plate 2 = " & "Ø" & dia2 & " - " & oHoleFeature2.ExtendedName & " => OK - Special Type")
Else
Debug.Print("Hole diameter of plate 1 = " & dia1 & " compared with Hole diameter of plate 2 = " & dia2 & " => Not OK")
file.WriteLine("Hole diameter of plate 1 = " & "Ø" & dia1 & " - " & oHoleFeature1.ExtendedName & " compared with Hole diameter of plate 2 = " & "Ø" & dia2 & " - " & oHoleFeature2.ExtendedName & " => Not OK")
End If
End Sub
Public Function CompareAlignment(ByVal oAxis As WorkAxis, ByVal oAxisCollection As ObjectCollection) As Integer
For i As Integer = 1 To oAxisCollection.Count
Dim axis As WorkAxis
axis = oAxisCollection.Item(i)
If oAxis.Line.IsColinearTo(axis.Line) Then
Return i
Exit Function
End If
Next
Return 0
End Function
Public Function IsAxisDuplicate(ByVal oAxis As WorkAxis, ByVal oAxisColl As ObjectCollection) As Boolean
If oAxisColl.Count > 0 Then
For i As Integer = 1 To oAxisColl.Count
Dim Axis As WorkAxis
Axis = oAxisColl.Item(i)
If Axis.Line.IsColinearTo(oAxis.Line) Then
Return True
End If
Next
Return False
Else
Return False
End If
End Function
Please feel free to contact if there is any doubt.
If solves problem, click on "Accept as solution" / give a "Kudo".
Thanks and regards,
CHANDRA SHEKAR G
Developer Advocate
Autodesk Developer Network
Hi @Anonymous,
The attached image is unclear to me. Can you please explain in detail?
"Need to check in all direction" means what?
Thanks and regards,
CHANDRA SHEKAR G
Developer Advocate
Autodesk Developer Network
Hi @Anonymous,
Correct me if I am wrong. You are trying create work axis only for hole feature to check alignment.
Thanks and regards,
CHANDRA SHEKAR G
Developer Advocate
Autodesk Developer Network
Hi @Anonymous,
Try the following VBA code to compare hole feature.
Public Sub Body_Faces()
Dim m_Inventor As Inventor.Application
m_Inventor = System.Runtime.InteropServices.Marshal.GetActiveObject("Inventor.Application")
Dim oDoc As AssemblyDocument
oDoc = m_Inventor.ActiveDocument
Dim oCompdef As AssemblyComponentDefinition
oCompdef = oDoc.ComponentDefinition
Dim oBody1 As SurfaceBody
Dim oBody2 As SurfaceBody
oBody1 = m_Inventor.CommandManager.Pick(SelectionFilterEnum.kPartBodyFilter, "Select first body")
oBody2 = m_Inventor.CommandManager.Pick(SelectionFilterEnum.kPartBodyFilter, "Select a body to compare")
Dim oFace As Face
Dim oAxis As WorkAxis
For Each oFace In oBody1.Faces
If oFace.SurfaceType = SurfaceTypeEnum.kCylinderSurface Then
oAxis = oCompdef.WorkAxes.AddFixed(oFace.Geometry.BasePoint, oFace.Geometry.AxisVector)
Dim comparedFace As Face
comparedFace = CompareFaces(oAxis, oBody2, oCompdef)
If comparedFace Is Nothing Then
oAxis.Name = oAxis.Name & "_misaligned"
Else
Dim oHoleFeature1 As HoleFeature
oHoleFeature1 = oFace.CreatedByFeature
Dim dia1 As Double
dia1 = oHoleFeature1.HoleDiameter.Value
dia1 = dia1 * 10 'Converting cm to mm
Dim oHoleFeature2 As HoleFeature
oHoleFeature2 = comparedFace.CreatedByFeature
Dim dia2 As Double
dia2 = oHoleFeature2.HoleDiameter.Value
dia2 = dia2 * 10 'Converting cm to mm
If Math.Round(dia1, 4) = Math.Round(dia2, 4) Then
Debug.Print("Hole diameter of plate 1 = " & dia1 & " compared with Hole diameter of plate 2 = " & dia2 & " => OK - Default")
ElseIf Math.Round(dia1, 4) >= Math.Round(dia2, 4) And Math.Round(dia1, 4) <= Math.Round(dia2, 4) + 0.5 Then
Debug.Print("Hole diameter of plate 1 = " & dia1 & " compared with Hole diameter of plate 2 = " & dia2 & " => OK - Special Type")
Else
Debug.Print("Hole diameter of plate 1 = " & dia1 & " compared with Hole diameter of plate 2 = " & dia2 & " => Not OK")
End If
End If
End If
Next
Dim oPane As BrowserPane
oPane = oDoc.BrowserPanes.ActivePane
Dim alignedNodes As ObjectCollection
alignedNodes = m_Inventor.TransientObjects.CreateObjectCollection
Dim misAlignedNodes As ObjectCollection
misAlignedNodes = m_Inventor.TransientObjects.CreateObjectCollection
For i = 4 To oCompdef.WorkAxes.Count
oAxis = oCompdef.WorkAxes.Item(i)
Dim misaligned As Boolean
misaligned = EndsWith(oAxis.Name, "misaligned")
Dim oNode As BrowserNode
If misaligned = True Then
oNode = oPane.GetBrowserNodeFromObject(oAxis)
misAlignedNodes.Add(oNode)
Else
oNode = oPane.GetBrowserNodeFromObject(oAxis)
alignedNodes.Add(oNode)
End If
Next
Dim alignedAxes As BrowserFolder
alignedAxes = oPane.AddBrowserFolder("Aligned Axes", alignedNodes)
Dim misAlignedAxes As BrowserFolder
misAlignedAxes = oPane.AddBrowserFolder("MisAligned Axes", misAlignedNodes)
End Sub
Public Function CompareFaces(ByVal oAxis1 As WorkAxis, ByVal oBody As SurfaceBody, ByVal compDef As AssemblyComponentDefinition) As Face
For Each oFace As Face In oBody.Faces
If oFace.SurfaceType = SurfaceTypeEnum.kCylinderSurface Then
Dim oAxis As WorkAxis
oAxis = compDef.WorkAxes.AddFixed(oFace.Geometry.BasePoint, oFace.Geometry.AxisVector)
If oAxis.Line.IsColinearTo(oAxis1.Line) Then
oAxis.Delete()
Return oFace
Exit Function
Else
oAxis.Delete()
End If
End If
Next
Return Nothing
End Function
Public Function EndsWith(str As String, ending As String) As Boolean
Dim endingLen As Integer
endingLen = Len(ending)
EndsWith = (Microsoft.VisualBasic.Right(Trim(UCase(str)), endingLen) = UCase(ending))
End Function
Thanks and regards,
CHANDRA SHEKAR G
Developer Advocate
Autodesk Developer Network
Hi @b_sharanraj,
Sorry for miscommunication,
The code was in VB.net.
Thanks and regards,
CHANDRA SHEKAR G
Developer Advocate
Autodesk Developer Network