check if hole has thread

[Charlies_3D_T]

Hello,

Do one of you know how i can check with ilogic if the hole feature has thread? 

I want a code that checks if the hole is a normal hole or a threaded hole. 

Thanks for the help!

[JelteDeJong]

hi, does this work for you?

[iLogic]

Dim feature As PartFeature = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFeatureFilter, "Select a hole")

If (feature.Type <> ObjectTypeEnum.kHoleFeatureObject) Then
    MsgBox("This is not an hole feature")
End If

Dim hole As HoleFeature = feature
Dim info As HoleTapInfo = hole.TapInfo

If (info Is Nothing) Then
    MsgBox("This hole is not threaded")
Else
    MsgBox("This hole is thread: " + info.ThreadDesignation)
End If

[Charlies_3D_T]

@JelteDeJong 

Hello,

Not working like i want. 

I explained myself bad i think. 

I want the rule to be automaticaly so it goes true all the PartFeatures. And i detect if its a hole and a cut or extrude and does something then. 

With your rule i need to select a hole. I need for example the rule below when the hole is thread then i = i + 1. But when i try to adapt your code it's not working. 

For Each oFeature In oFeatures
	'check if its a hole
	If TypeOf oFeature Is ExtrudeFeature And oFeature.Suppressed = False And oFeature.Name.Contains("Hole") Then
		'increment one
		i = i + 1
	End If	
Next

[JhoelForshav]

Hi @Charlies_3D_T 

Do you just want to count how many faces in the part has threads?

Like this?

Dim pDoc As PartDocument = ThisDoc.Document
Dim i As Integer
For Each oBod As SurfaceBody In pDoc.ComponentDefinition.SurfaceBodies
	For Each oFace As Face In oBod.Faces
		If oFace.ThreadInfos IsNot Nothing Then i += 1
	Next
Next

Messagebox.Show("Threaded faces in part: " & i, "Number of threads")

[JelteDeJong · Accepted solution]

If you need to find the features to changed them. then you could also use this code:

Dim doc As PartDocument = ThisDoc.Document
Dim features = doc.ComponentDefinition.Features

Dim numberOfThreadedHoleFeatures As Integer = 0
For Each hole As HoleFeature In features.HoleFeatures
    Dim info As HoleTapInfo = hole.TapInfo
    If (info IsNot Nothing) Then
        numberOfThreadedHoleFeatures = numberOfThreadedHoleFeatures + 1
        ' Your hole changing code go's here
    End If
Next
MsgBox("Number of holes with thread: " & numberOfThreadedHoleFeatures)

' you can skip this loop if you just want to count the number of tread features
For Each thread As ThreadFeature In features.ThreadFeatures
    ' Your thread changing code go's here
Next
MsgBox("Number of threadfeatures (on a extrude or cut feature): " _
		& features.ThreadFeatures.Count)

[Charlies_3D_T]

@JelteDeJong 

Can i ask you if you want to take a look at an other problem? In this problem i want to have for example a assembly painted and then i need the color placed in a custom property inside this assembly so that when i make a drawing i can get the color on the drawing. 

I don't want to paint the parts because in real life you first assembly the welding assembly and after it goes to the painting stage. I hope you can help me. 

I have this rule for placing the color inside a property inside a part: 

Dim oDoc As Document
oDoc = ThisDoc.Document
 
If ThisDoc.Document.ActiveAppearance.DisplayName.Contains("RAL") then
 
iProperties.Value("Custom", "Color") = Left(ThisDoc.Document.ActiveAppearance.DisplayName, 8)

End If

Here is the link with my question: 

https://forums.autodesk.com/t5/inventor-customization/how-to-add-appearance-from-an-assembly-to-the-...