count numbers of holes in the iam

[TatianaR]

Hello!
Please tell me how to use the iLogic cod, count the number of holes in the assembly
Thank you
Tatiana

[Vladimir.Ananyev]

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,

[TatianaR]

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

[Vladimir.Ananyev · Accepted solution]

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,

[TatianaR]

Dear Vladimir
Thank you for your help
I really appreciate it
But  I have another question
In the assembly file I want not only the number of holes bur also the diameter of the holes.

for example:

12 holes - diameter 5 mm
5 hole - diameter 7 mm
Which functions is necessary for this purpose?

Best regards

Tatiana

[Vladimir.Ananyev · Accepted solution]

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,

[belash007]

Hi Vladimir.
Is there any way to count punch features in assembly as similar to hole you shown above?

Thanks
Belash