count numbers of holes in the iam
Hi Tatiana,
I added iLogic rules to sample part files you provided.
Case 1. Hole feature pattern
Attached file hole_pattern_iLOGIC.ipt contains the demo iLogic rule for hole feature rectangular pattern.
' Calc Holes in HoleFeature Pattern
'assume part document
Dim oDoc As PartDocument = ThisDoc.Document
'Set oDoc = ThisApplication.ActiveDocument
Dim oDef As PartComponentDefinition = oDoc.ComponentDefinition
'assume rectangular pattern
Dim oRectPatterns As RectangularPatternFeatures = oDef.Features.RectangularPatternFeatures
Dim N As Integer = 0 'counter
For Each oRP As RectangularPatternFeature In oRectPatterns
'consider only hole patterns
If Not (TypeOf oRP.ParentFeatures.Item(1) Is HoleFeature) Then Continue For
For Each oFPE As FeaturePatternElement In oRP.PatternElements
If Not oFPE.Suppressed Then N += 1
Next
Next
MsgBox ("The number of holes in the current part is: " & N)
Circular patterns could be processed in the samilar way.
Refer Inventor API Help for CircularPatternFeature object description.
Case 2. Hole features created “from sketch”.
See iLogic rule in the attached file extrude_point_pattern_hole_iLOGIC.ipt
' CalcHolesFromSketch
Dim oDoc As PartDocument = ThisDoc.Document
Dim oDef As PartComponentDefinition = oDoc.ComponentDefinition
Dim oHoles As HoleFeatures = oDef.Features.HoleFeatures
Dim N As Integer = 0 'counter
For Each oH As HoleFeature In oHoles
If oH.Suppressed Then Continue For
If oH.PlacementType = HolePlacementTypeEnum.kSketchPlacementType Then
N += oH.HoleCenterPoints.Count
End If
Next
Beep
MsgBox ("The number of holes in the current part is: " & N)
Hope you could modify these iLogic code samples to suit your needs.
Cheers,
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network
Hi Vladimir
Thank you very much for your help.
But I have another question, hope - the last 
How to count the number of holes in the assembly file?
Files for an example - I added
Whether this is possible in general, counting the holes different ways in a single file?
Best regards
Tatiana
Hi Tatiana,
I've attached assembly with iLogic rules that could help you to start.
The first rule Iterates through all leaf occurrences collection.
The second rule Iterates through all referenced documents collection.
The last should be more efficient if your assembly includes a lot of copies of parts with holes.
(I did not test this idea though).
Both Main methods call the same function GetHolesQty which returns the number of holes in the specified part component definition.
Please note that this function cannot work with nested feature patterns.
Approach 1. Iterates through all leaf occurrences collection.
Sub Main()
Dim oAsmDoc As AssemblyDocument = ThisDoc.Document
Dim oAsmDef As AssemblyComponentDefinition = oAsmDoc.ComponentDefinition
Dim N As Integer = 0 'holes counter
For Each oOcc As ComponentOccurrence In oAsmDef.Occurrences.AllLeafOccurrences
If Not oOcc.Suppressed Then
If oOcc.DefinitionDocumentType = kPartDocumentObject Then
Dim oDef As PartComponentDefinition = oOcc.Definition
N += GetHolesQty(oDef)
End If
End If
Next
Beep
MsgBox ("The number of holes in the current part is: " & N)
End Sub
Approach 2. Iterates through all referenced documents collection.
Sub Main()
Dim oAsmDoc As AssemblyDocument = ThisDoc.Document
Dim oAsmDef As AssemblyComponentDefinition = oAsmDoc.ComponentDefinition
Dim oOccs As ComponentOccurrences = oAsmDef.Occurrences
Dim N As Integer = 0 'holes counter
For Each oDoc As Inventor.Document In oAsmDoc.AllReferencedDocuments
If TypeOf oDoc Is PartDocument Then
Dim m As Integer = GetHolesQty(oDoc.ComponentDefinition)
N = N + m * oOccs.AllReferencedOccurrences(oDoc).Count
End If
Next
Beep
MsgBox ("The number of holes in the current part is: " & N)
End Sub
'''Calculates holes in the part document
'''Be careful: nested patterns are not analyzed!
Function GetHolesQty(ByVal oDef As PartComponentDefinition) As Integer
Dim N As Integer = 0 'counter
Dim oHoles As HoleFeatures = oDef.Features.HoleFeatures
For Each oH As HoleFeature In oHoles
If Not oH.Suppressed Then
N += oH.HoleCenterPoints.Count
End If
Next
'have we any rectangular patterns ?
Dim oRectPatterns As RectangularPatternFeatures
oRectPatterns = oDef.Features.RectangularPatternFeatures
For Each oRPF As RectangularPatternFeature In oRectPatterns
Dim m As Integer = 0
If Not oRPF.Suppressed Then
If (TypeOf oRPF.ParentFeatures.Item(1) Is HoleFeature) Then
Dim oH As HoleFeature = oRPF.ParentFeatures.Item(1)
If Not oH.Suppressed Then
For Each oFPE As FeaturePatternElement In oRPF.PatternElements
If Not oFPE.Suppressed Then m += 1
Next
End If
End If
N += m - 1
Else
N += m
End If
Next
'have we any circular patterns ?
Dim oCircPatterns As CircularPatternFeatures
oCircPatterns = oDef.Features.CircularPatternFeatures
For Each oCPF As CircularPatternFeature In oCircPatterns
Dim m As Integer = 0
If Not oCPF.Suppressed Then
If (TypeOf oCPF.ParentFeatures.Item(1) Is HoleFeature) Then
Dim oH As HoleFeature = oCPF.ParentFeatures.Item(1)
If Not oH.Suppressed Then
For Each oFPE As FeaturePatternElement In oCPF.PatternElements
If Not oFPE.Suppressed Then m += 1
Next
End If
End If
N += m - 1
Else
N += m
End If
Next
Return N
End Function
Cheers,
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network
Hi Tatiana,
look at the HoleFeature ptoperties - HoleDiameter, HoleType, ExtendedName, etc.
HoleFeature.HoleDiameter property returns the model parameter controlling the diameter of the hole.
HoleDiamener.Expression gives diameter in the string format, e.g. "6 mm".
HoleDiamener.Value gives the same diameter in the base length units (cm) - 6.
The following DevBlog post could help you to discover object model
http://adndevblog.typepad.com/manufacturing/2013/10/discover-object-model.html
Cheers,
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network
