topic Re: iFeature in Inventor Programming Forum

iFeature

martinhoos — Thu, 08 Feb 2018 14:26:50 GMT

Hello,

i have a iFeature named LongPilot. If i insert this one time the name changed to "LongPilot:1" and the next time to "LongPilot:2". Is it possible to count the quantity of the "LongPilots"? Possible quantitys are only: 0 or 1 or 2 of them. The amount stored in an userparameter named "amount".

One Probleme: If i insert and insert and delete and delete the Longpilots, i can have names like "LongPilot:8" or stuff like this....

Hopefully you can help me...

Regards from Germany.

Martin

Re: iFeature

bradeneuropeArthur — Thu, 08 Feb 2018 14:48:54 GMT

Hi,

Again and modified a little!!

Public Sub features()

Dim a As Application
Set a = ThisApplication
Dim b As PartDocument
Set b = a.ActiveDocument
Dim f As Object ' ExtrudeFeature
'Set c = b.ComponentDefinition.Features

Dim i As Integer
i = 0
For Each f In b.ComponentDefinition.features
If InStr(f.Name, "LongPilot") > 0 Then
i = i + 1
End If

Next

MsgBox i
End Sub

Re: iFeature

martinhoos — Fri, 09 Feb 2018 09:33:24 GMT

Hi Brandeneurope,

thank you for your reply... your makro runs! Is it possible for you to change the script into ilogic-code? I tried .... without result 😞

Regards Martin

Re: iFeature

chandra.shekar.g — Fri, 09 Feb 2018 09:58:37 GMT

@martinhoos,

Try the following iLogic code to count LongPilot iFeature.

Dim b As PartDocument
b = ThisApplication.ActiveDocument

Dim i As Integer 

For Each f In b.ComponentDefinition.Features
	If f.Name.StartsWith("LongPilot")Then
		i = i + 1 
	End If
Next

MessageBox.Show("Count of LongPilot is : " & i.ToString, "iLogic")

Please feel free to contact if there is any queries,

If solves problem, click on "Accept as solution" / give a "Kudo".

Thanks and regards,

Re: iFeature

bradeneuropeArthur — Fri, 09 Feb 2018 10:00:08 GMT

Yes,

Public Sub Main()

Dim a As Application
a = ThisApplication
Dim b As PartDocument
b = a.ActiveDocument
Dim f As Object ' ExtrudeFeature
'Set c = b.ComponentDefinition.Features

Dim i As Integer
i = 0
For Each f In b.ComponentDefinition.Features
If InStr(f.Name, "LongPilot") > 0 Then
i = i + 1
End If

Next

MsgBox (i)
End Sub

Re: iFeature

bradeneuropeArthur — Fri, 09 Feb 2018 10:18:58 GMT

@martinhoos

Please let me know if you need further assistance....

Re: iFeature

martinhoos — Fri, 09 Feb 2018 11:27:50 GMT

Hi Brandeneurope,

yes i need further help.... i thought i couldt handle this by myselfe - but ..... (its to hard to understand)

the idea is: i have a tube which i changed which ilogic (diameter, radius, material ....)

sometimes i need the "LongPilot", which has also a diameter. If the Name of the LongPilot is "LongPilot:1" or "LongPilot:2" i can change the diameter with:

iFeature.ChangeRow("LongPilot:1", "16 mm")

or 

iFeature.ChangeRow("LongPilot:1", "18 mm")

But sometimes the name is, for example like, "LongPilot:5" (delete and stored again) - so i can not identify the Name 😞

I used this code to place the LongPilot in:

Public Sub Main() 

	Dim oPartDoc As PartDocument 
	oPartDoc = ThisApplication.ActiveDocument 

	Dim oPartDef As PartComponentDefinition 
	oPartDef = oPartDoc.ComponentDefinition 

	Dim oWorkPoint As WorkPoint 
	oWorkPoint = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kWorkPointFilter, "Select a point to place iFeature")  
	' Get the selected face to use as input for the iFeature. 
	Dim oFacePlane As WorkPlane 
	oFacePlane = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kWorkPlaneFilter, "Select a Plane to place iFeature") 

	Dim oFeatures As PartFeatures 
	oFeatures = oPartDef.Features 

	' Create an iFeatureDefinition object. 
	Dim oiFeatureDef As iFeatureDefinition 
	oiFeatureDef = oFeatures.iFeatures.CreateiFeatureDefinition("V:\Inventor-2015\1-Inventor\Catalog\KKI\LongPilot.ide")

	' Set the input. 
	Dim oInput As iFeatureInput 
	For Each oInput In oiFeatureDef.iFeatureInputs 
		Dim oParamInput As iFeatureParameterInput 
		
		Select Case oInput.Name 
		Case "Durchmesser" 
		Dim oTubeDia As iFeatureParameterInput 
		oTubeDia = oInput 
		oTubeDia.Expression = durchmesser


		Case "Skizzierebene1" 
		Dim oPlaneInput As iFeatureSketchPlaneInput 
		oPlaneInput = oInput 
		oPlaneInput.PlaneInput = oFacePlane 

		Case "Referenzpunkt1" 

		Dim oRefPoint As iFeatureEntityInput 
		oRefPoint = oInput 
		oRefPoint.Entity = oWorkPoint 

		End Select 
	Next 

	' Create the iFeature. 
	Dim oiFeature As iFeature 
	oiFeature = oFeatures.iFeatures.Add(oiFeatureDef) 

End Sub

Long Story short: If i changed the diameter from the tube all longpilots (max. 2) shouldt change also.... AND i need the amount of the Longpilots (you gave me the code above)

Hopefully you can give me support to handle the problem.... Thank you very much!

Regards

Martin

Re: iFeature

bradeneuropeArthur — Fri, 09 Feb 2018 11:37:14 GMT

So if Diameter pipe change from 12 mm to 16 mm, the Pilot must also change from 12 to 16 mm. am I right?

Re: iFeature

chandra.shekar.g — Fri, 09 Feb 2018 11:51:23 GMT

@martinhoos,

Do you need number of 16 dia tube and 12 dia tube? Also, wants to change name of LongPilot to respective diameter name?

Thanks and regards,

Re: iFeature

martinhoos — Fri, 09 Feb 2018 12:13:25 GMT

yes you are right....

Re: iFeature

martinhoos — Fri, 09 Feb 2018 12:21:15 GMT

The Diameters are Ø10, Ø12, Ø16 and Ø18

If i changed the Diameter from Ø12 to Ø18 of the tube, the Longpilot shouldt also changes to Ø18.

The second is, i need the number of inserted LongPilots (0 or 1 or 2)

Regards Martin

Re: iFeature

bradeneuropeArthur — Fri, 09 Feb 2018 14:21:35 GMT

Could you please upload the feature PilotHole

Re: iFeature

martinhoos — Mon, 12 Feb 2018 06:54:12 GMT

Hello Brandeneurope,

thanks for your reply... here is the iFeature...

Regards Martin

Re: iFeature

bradeneuropeArthur — Mon, 12 Feb 2018 06:59:46 GMT

How is your pipe diameter parameter called?

Re: iFeature

martinhoos — Mon, 12 Feb 2018 07:06:50 GMT

the Diameter of the pipe is called: durchmesser

Re: iFeature

bradeneuropeArthur — Mon, 12 Feb 2018 07:33:28 GMT

Public Sub Main()
MsgBox 	 (Parameter.Param("durchmesser").expression)
If Parameter.Param("durchmesser").Expression = "10 mm
Call features("LongPilot", 10 mm)
End If

If Parameter.Param("durchmesser").Expression = "16 mm" Then 
Call features("LongPilot", 16 mm) 
End If

'etc 
	

End Sub

Public Sub features(Str As String , Dia as string)

Dim a As Application
a = ThisApplication
Dim b As PartDocument
b = a.ActiveDocument
Dim f As Object ' ExtrudeFeature
'Set c = b.ComponentDefinition.Features

Dim i As Integer
i = 0
For Each f In b.ComponentDefinition.Features
If InStr(f.Name, Str) > 0 Then

iFeature.ChangeRow(f.name, Dia)

i = i + 1
End If

Next
MsgBox (f.name)
MsgBox (i)
End Sub

EDIT .....................

Re: iFeature

chandra.shekar.g — Mon, 12 Feb 2018 09:11:42 GMT

@martinhoos,

Try the following iLogic code to rename the "LongPilot" iFeature with respect to Diameter.

Public Sub Main()

    Dim oPartDoc As PartDocument
    oPartDoc = ThisApplication.ActiveDocument
          
    Dim oPartDef As PartComponentDefinition
    oPartDef = oPartDoc.ComponentDefinition
    
    Dim oFeatures As PartFeatures
    oFeatures = oPartDef.Features
    
    Dim i10Cnt As Integer
    Dim i12Cnt As Integer
    Dim i16Cnt As Integer
    Dim i18Cnt As Integer
    
    Dim oiFeature As iFeature
    For Each oiFeature In oFeatures.iFeatures
        If InStr(oiFeature.Name, "LongPilot") > 0 Then
            If oiFeature.Parameters.Item(8).Expression = "10 mm" Then
                i10Cnt = i10Cnt + 1
            ElseIf oiFeature.Parameters.Item(8).Expression = "12 mm" Then
                i12Cnt = i12Cnt + 1
            ElseIf oiFeature.Parameters.Item(8).Expression = "16 mm" Then
                i16Cnt = i16Cnt + 1
            ElseIf oiFeature.Parameters.Item(8).Expression = "18 mm" Then
                i18Cnt = i18Cnt + 1
            End If
        End If
    Next
    
    Dim i As Integer
    If i10Cnt > 0 Then
        For i = 1 To i10Cnt
            For Each oiFeature In oFeatures.iFeatures
                If InStr(oiFeature.Name, "LongPilot") > 0 Then
                    If oiFeature.Parameters.Item(8).Expression = "10 mm" Then
                        If oiFeature.Name = "LongPilot Dia 10 mm :" & i - 1 Then
                             GoTo NextIteration10
                        End If
                        If Not InStr(oiFeature.Name, "LongPilot Dia 10 mm :") > 0 Then
                            oiFeature.Name = "LongPilot Dia 10 mm :" & i-1
                            GoTo NextIteration10
                        End If
                    End If
                End If
            Next
NextIteration10:
        Next
    End If
    If i12Cnt > 0 Then
        For i = 1 To i12Cnt
            For Each oiFeature In oFeatures.iFeatures
                If InStr(oiFeature.Name, "LongPilot") > 0 Then
                    If oiFeature.Parameters.Item(8).Expression = "12 mm" Then
                        If oiFeature.Name = "LongPilot Dia 12 mm :" & i -1 Then
                             GoTo NextIteration12
                        End If
                        If Not InStr(oiFeature.Name, "LongPilot Dia 12 mm :") > 0 Then
                            oiFeature.Name = "LongPilot Dia 12 mm :" & i -1
                            GoTo NextIteration12
                        End If
                    End If
                End If
            Next
NextIteration12:
        Next
    End If
    If i16Cnt > 0 Then
        For i = 1 To i16Cnt
            For Each oiFeature In oFeatures.iFeatures
                If InStr(oiFeature.Name, "LongPilot") > 0 Then
                    If oiFeature.Parameters.Item(8).Expression = "16 mm" Then
                        If oiFeature.Name = "LongPilot Dia 16 mm :" & i -1Then
                             GoTo NextIteration16
                        End If
                        If Not InStr(oiFeature.Name, "LongPilot Dia 16 mm :") > 0 Then
                            oiFeature.Name = "LongPilot Dia 16 mm :" & i -1
                            GoTo NextIteration16
                        End If
                    End If
                End If
            Next
NextIteration16:
        Next
    End If
    If i18Cnt > 0 Then
        For i = 1 To i18Cnt
            For Each oiFeature In oFeatures.iFeatures
                If InStr(oiFeature.Name, "LongPilot") > 0 Then
                    If oiFeature.Parameters.Item(8).Expression = "18 mm" Then
                        If oiFeature.Name = "LongPilot Dia 18 mm :" & i - 1 Then
                             GoTo NextIteration18
                        End If
                        If Not InStr(oiFeature.Name, "LongPilot Dia 18 mm :") > 0 Then
                            oiFeature.Name = "LongPilot Dia 18 mm :" & i - 1
                            GoTo NextIteration18
                        End If
                    End If
                End If
            Next
NextIteration18:
        Next
    End If

End Sub

Please feel free to contact if there is any queries.

If solves problem, click on "Accept as solution" / give a "Kudo".

Thanks and regards,

Re: iFeature

bradeneuropeArthur — Mon, 12 Feb 2018 09:15:16 GMT

Please let me know if you need assistance.

Re: iFeature

martinhoos — Mon, 12 Feb 2018 12:23:58 GMT

Hello Brandeneurope,

Thank you very much ... this is what i needed! Great work.

Regards Martin

Re: iFeature

martinhoos — Mon, 12 Feb 2018 12:25:35 GMT

Hello Chandra,

thank you very much for your help - also your code helps me to solve my Problem.

Regards Martin