Delete bolted connections - explode holes

[GeorgK]

Hello together,

is there a way to delete the bolted connections and keep the parts which are inserted with the bolted connection with VB.NET?

How could I explode the holes  (make them independent) in plates?

https://forums.autodesk.com/t5/inventor-forum/make-holes-independent-throug-several-parts/td-p/68825...

https://forums.autodesk.com/t5/inventor-forum/make-hole-through-several-plates/td-p/2973292

Thank you

Georg

[wayne.brill]

Hello Georg,

There is not any API for bolted connections. Also there is not any direct method in the API to do what the explode command does to the ClientFeature using the UI to allow the hole to be converted to a HoleFeature. 

It seems like it should be possible to use the API to get the HoleFeature from the ClientFeatureElements of the ClientFeatureDefinition. Once your code gets the HoleFeature created you could delete the ClientFeature. I do not have code that does this and I am not sure how doing this would interact with the bolted connection.  

You can use Inventor VBA and the watch window to see the properties of the ClientFeature. Here is a snippet that you can use. Put a break point on End Sub and add a watch for oObj. (have the hole selected in the part before running the code). You will also find attributes that are used by the bolted connection.

Public Sub SelectTest()
    Dim oDoc As Document ' DrawingDocument
    Set oDoc = ThisApplication.ActiveDocument
  
    If oDoc.SelectSet.count > 0 Then
        Dim oObj As Object
        Set oObj = oDoc.SelectSet(1)
    End If
      
End Sub

If you want an API to delete the bolted connections and keep the parts which are inserted with the bolted connection and the holes in the parts please post it on the Inventor idea station.

http://forums.autodesk.com/t5/inventor-ideastation/idb-p/v1232/tab/most-recent

Thanks,

Wayne

[GeorgK]

Hello Wayne,

is it possible to ask the developper how to change the hole (explode it)? That would be very helpful.

Georg

[wayne.brill]

Hi Georg,

A colleague has this suggestion:

>> >>

The users want to delete bolt connection and keep the holes through Inventor API. Please correct me if I am wrong.

From my side, we just need delete the bolt connection by API. Actually, Bolt Connection is a ComponentOccurrence object from viewpoint of API. Below is sample code.
 
  Dim oCompOcc As ComponentOccurrence
  Set oCompOcc = oAssyDoc.ComponentDefinition.Occurrences.Item(3)

  Call oCompOcc.Delete

<< <<

I used similar code and I see the bolted connection is deleted and the holes remain in the part. To test this just have the bolted connected selected.

Public Sub SelectTest()
    Dim oDoc As Document 
    Set oDoc = ThisApplication.ActiveDocument
   
    If oDoc.SelectSet.count > 0 Then
        Dim oObj As Object
        Set oObj = oDoc.SelectSet(1)
        
        Dim oCmpOcc As ComponentOccurrence
        Set oCmpOcc = oObj 

        Call oCmpOcc.Delete

    End If
End Sub

I do notice that after the bolted connection ComponentOccurrence is deleted by API the hole in the part has attributes that seem to be related to bolted connection. I believe your code could safely delete these attributes as well.

Thanks,

Wayne

[GeorgK]

Hello Wayne,

this is a workaround but does not solve the problem.

Thank you.

Georg

[wayne.brill · Accepted solution]

Hi Georg,

After the component occurrence for the bolted connection is deleted the holes in the parts are ClientFeatures. The code below will do something similar to exploding the client feature using the UI. (thanks to a colleague for providing it) 

Notice the ClientFeatureDefinition.ClientFeatureElements.Item(index).Delete is used to delete the element to release the native object(Hole feature in the case). Then the ClientFeature is deleted.

Sub ExplodeClientFeature()

    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.ActiveDocument
    
    'get client feature
    Dim oCF As ClientFeature
    Set oCF = oPartDoc.ComponentDefinition.Features.ClientFeatures.Item(1)
    
    'delete elements in client feature
    Dim oCFElements As ClientFeatureElements
    Set oCFElements = oCF.Definition.ClientFeatureElements
    
    Dim nCount As Integer
    nCount = oCFElements.count
    
    Dim i As Integer
    For i = nCount To 1 Step -1
        Call oCFElements.Item(i).Delete
    Next
    
    'delete client feature
    Call oCF.Delete

End Sub

Thanks,

Wayne

[GeorgK]

Hello Wayne,

great! That solves my problem.

Georg