iLogic place Structural Shapes:Channels, how to change length?

[cean_au]

Hi,

I got this code below to place a channel in an assembly, but don't know how to change the length of the steel.

thanks for help

Cean

' Set a reference to the active assembly document.
    Dim oDoc As AssemblyDocument
    oDoc = ThisApplication.ActiveDocument

    ' Set a reference to the ContentCenter object.
    Dim oContentCenter As ContentCenter
    oContentCenter = ThisApplication.ContentCenter

    ' Get the content node (category) "Structural Shapes:Channels"
    Dim oContentNode As ContentTreeViewNode
    oContentNode = oContentCenter.TreeViewTopNode.ChildNodes.Item("Structural Shapes").ChildNodes.Item("Channels")

    ' Get the "DIN 1026 U" Family object.
    Dim oFamily As ContentFamily
    For Each oFamily In oContentNode.Families
        If oFamily.DisplayName = "DIN 1026 U" Then
            Exit For
        End If
    Next

    ' Create a member based on the first row of the family.
    Dim myError As MemberManagerErrorsEnum
    Dim strContentPartFileName As String
    Dim strErrorMessage As String
    strContentPartFileName = oFamily.CreateMember(1, myError, strErrorMessage)
    MessageBox.Show(strContentPartFileName)

    Dim oMat As Matrix
    oMat = ThisApplication.TransientGeometry.CreateMatrix

    ' Insert an instance of the content center member in the assembly.
    call oDoc.ComponentDefinition.Occurrences.Add(strContentPartFileName, oMat)

[Mario-Villada]

Try changing the parameter called "G_L"

[xiaodong_liang]

Hi,

I believe Mario-Villada is correct. One of the parameters of the CC part should control the length of the steel. You could find it and modify it.

[Carthik_Babu]

hi, can you please ping the code to modify the parameter by ilogic. I have same issue in selecting bolt type and length of a content center file.
http://forums.autodesk.com/t5/Autodesk-Inventor-Customization/ilogic-to-trigger-and-insert-custom-co...

[Mario-Villada]

Have a look at a sample code in the programming help called " Model Parameters API Sample". you should find out which parameter controls the length and change it by code. here is some code from the help file.

' Obtain the Model Parameters collection
    Dim oModelParams As ModelParameters
    Set oModelParams = oParams.ModelParameters
    
    ' Iterate through the Model Parameters collection
    Dim iNumModelParams As Long
    Debug.Print "MODEL PARAMETER VALUES"
    For iNumModelParams = 1 To oModelParams.Count
        ' Display the Name
        Debug.Print " Name:" & oModelParams.Item(iNumModelParams).Name
        
        ' Display the Value
        Debug.Print "  Value: " & oModelParams.Item(iNumModelParams).Value
        
        ' Display the units
        Debug.Print "  Units: " & oModelParams.Item(iNumModelParams).Units
       
        ' Change the Model Parameter values
        oModelParams.Item(iNumModelParams).Value = oModelParams.Item(iNumModelParams).Value * 2
    Next iNumModelParams
    
    ' Accessing a particular parameter if you know its name, the user and reference parameters can also be accessed in a similar way
    oModelParams.Item("d0").Name = "NewParam"
    
    ' Change the value of the newly named parameter "param1"
    oModelParams.Item("NewParam").Value = 25
    
    ' Update the model.
    oPartDoc.Update

 Please select this as solved if it helped you.

[Carthik_Babu]

Hi,

Got message: "ModelParameter is not defined". I am using autodesk inventor 2011. Kindly help

[Mario-Villada · Accepted solution]

The code is for VBA

But I guess ilogic can be as simple as getting the parameter like the in picture below.

[Carthik_Babu]

Hi,

I tried the way, you have told by just handling part parameter by ilogic as shown in the below code.

Sub Main()
PlaceContentCenterPart_GND()
iLogicVb.UpdateWhenDone = True
ThisApplication.ActiveView.Fit
End Sub

Sub PlaceContentCenterPart_GND()

    ' Set a reference to the active assembly document.
    Dim oDoc As AssemblyDocument
    oDoc = ThisApplication.ActiveDocument

    ' Set a reference to the ContentCenter object.
    Dim oContentCenter As ContentCenter
    oContentCenter = ThisApplication.ContentCenter

    ' Get the content node (category) 
    Dim oContentNode As ContentTreeViewNode
    oContentNode = oContentCenter.TreeViewTopNode.ChildNodes.Item("Tube & Pipe").ChildNodes.Item("Conduits").ChildNodes.Item("Pipes")
    
    ' Get the Family object.
    Dim oFamily As ContentFamily
    For Each oFamily In oContentNode.Families
        If oFamily.DisplayName = "ANSI/ASME B36.19M Pipe" Then
            Exit For
        End If
    Next

    ' Create a member based on the first row of the family.
    Dim Error1 As MemberManagerErrorsEnum
    Dim strContentPartFileName As String
    Dim strErrorMessage As String
    strContentPartFileName = oFamily.CreateMember(1, Error1, strErrorMessage)
    
        

Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition
Dim oTG As TransientGeometry
oTG = ThisApplication.TransientGeometry
    
' Create a matrix.  
Dim oMatrix As Matrix
oMatrix = oTG.CreateMatrix

'Iterate through all of the occurrences
Dim oOccurrence As ComponentOccurrence

'place an instance of the component 
'in this case at 0,0,0
'positioned at the co-ordinates
oMatrix.SetTranslation(oTG.CreateVector(0, 0, 0)) 

oOccurrence = oAsmCompDef.Occurrences.Add(strContentPartFileName, oMatrix) 
oOccurrence.Grounded = True
Pipe_Length = InputBox("Enter Pipe length (Unit:inches)", "Pipe length", "10")
Parameter(oOccurrence.Name, "L") = Pipe_Length 
Component.Color(oOccurrence.Name) = "Red"
End Sub

It works. But the name of the inserted component (ANSI/ASME B36.19M Pipe 1/8 - Schedule 10S - 10:1), remains same. Is there is any way to assign Pipe Length in the code

 oAsmCompDef.Occurrences.Add

which inserts the part into assembly.

Thanks in advance

[Carthik_Babu]

Any help to handle

Sub CreateMember(Row As VARIANT, ByRef FailureReason As MemberManagerErrorsEnum, ByRef FailureMessage As String, ByRef Refresh As [defaultvalue(kUseDefaultRefreshSetting)] ContentMemberRefreshEnum, ByRef Custom As [defaultvalue(0)] Boolean, ByRef FileName As [defaultvalue("")] String, ByRef CustomInput As [optional] VARIANT, ByRef Options As [optional] VARIANT, Result As [out, retval] BSTR)

[adam.nagy]

Hi Carthik,

You just need to provide custom parameter values for the member you are creating. Simply modify this part of the code:

    Dim values As NameValueMap
    values = ThisApplication.TransientObjects.CreateNameValueMap
    Call values.Add("B_L", "0.5 in")
    Dim strErrorMessage As String
    strContentPartFileName = oFamily.CreateMember(1, myError, strErrorMessage, , , , values)

Cheers,

[Carthik_Babu]

Hi Adam Nagy,

Thanks al lot for the solution.....

I have modified the code as below, it worked......

Sub Main()
PlaceContentCenterPart_GND()
iLogicVb.UpdateWhenDone = True
ThisApplication.ActiveView.Fit
End Sub

Sub PlaceContentCenterPart_GND()

    ' Set a reference to the active assembly document.
    Dim oDoc As AssemblyDocument
    oDoc = ThisApplication.ActiveDocument

    ' Set a reference to the ContentCenter object.
    Dim oContentCenter As ContentCenter
    oContentCenter = ThisApplication.ContentCenter

    ' Get the content node (category) 
    Dim oContentNode As ContentTreeViewNode
    oContentNode = oContentCenter.TreeViewTopNode.ChildNodes.Item("Tube & Pipe").ChildNodes.Item("Conduits").ChildNodes.Item("Pipes")
    
    ' Get the Family object.
    Dim oFamily As ContentFamily
    For Each oFamily In oContentNode.Families
        If oFamily.DisplayName = "ANSI/ASME B36.19M Pipe" Then
            Exit For
        End If
    Next

    ' Create a member based on the first row of the family.
    Dim Error1 As MemberManagerErrorsEnum
    Dim strContentPartFileName As String
    Dim values As NameValueMap
    values = ThisApplication.TransientObjects.CreateNameValueMap
    Dim strErrorMessage As String
    Pipe_Length = InputBox("Enter Pipe length (Unit:inches)", "Pipe length", "1")
    Call values.Add("PL", Pipe_Length)
    strContentPartFileName = oFamily.CreateMember(1, Error1, strErrorMessage, , , ,values)
    
        

Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition
Dim oTG As TransientGeometry
oTG = ThisApplication.TransientGeometry
    
' Create a matrix.  
Dim oMatrix As Matrix
oMatrix = oTG.CreateMatrix

'Iterate through all of the occurrences
Dim oOccurrence As ComponentOccurrence

'place an instance of the component 
'in this case at 0,0,0
'positioned at the co-ordinates
oMatrix.SetTranslation(oTG.CreateVector(0, 0, 0)) 

oOccurrence = oAsmCompDef.Occurrences.Add(strContentPartFileName, oMatrix) 
oOccurrence.Grounded = True

Component.Color(oOccurrence.Name) = "Red"
End Sub

[Carthik_Babu]

Hi,

To insert Content Center Part as Custom, Kindly find the code below. Hope it will be useful.

Sub Main()
PlaceContentCenterPart_GND()
iLogicVb.UpdateWhenDone = True
ThisApplication.ActiveView.Fit
End Sub

Sub PlaceContentCenterPart_GND()

Top_Node = "Tube & Pipe"
ChildNodes1 = "Conduits"
ChildNodes2 = "Pipes"
Family_Name = "ANSI/ASME B36.19M Pipe"

    ' Set a reference to the active assembly document.
    Dim oDoc As AssemblyDocument
    oDoc = ThisApplication.ActiveDocument
    
    Dim fileName As String = String.Empty
    Dim CustomPartDirectory= ThisDoc.Path & "\"
    Dim isCustom As Boolean = m_customInfo IsNot Nothing
    Dim refresh As Inventor.ContentMemberRefreshEnum = ContentMemberRefreshEnum.kUseDefaultRefreshSetting
    
    ' Set a reference to the ContentCenter object.
    Dim oContentCenter As ContentCenter
    oContentCenter = ThisApplication.ContentCenter

    ' Get the content node (category) 
    Dim oContentNode As ContentTreeViewNode
    oContentNode = oContentCenter.TreeViewTopNode.ChildNodes.Item(Top_Node).ChildNodes.Item(ChildNodes1).ChildNodes.Item(ChildNodes2)
    
    ' Get the Family object.
    Dim oFamily As ContentFamily
    For Each oFamily In oContentNode.Families
        If oFamily.DisplayName = Family_Name Then
            Exit For
        End If
    Next

    ' Create a member based on the first row of the family.
    Dim Error1 As MemberManagerErrorsEnum
    Dim strContentPartFileName As String
    Dim values As NameValueMap
    values = ThisApplication.TransientObjects.CreateNameValueMap
    Dim strErrorMessage As String
    Pipe_Length = InputBox("Enter Pipe length (Unit:inches)", "Pipe length", "1")
    fileName = IO.Path.Combine(CustomPartDirectory + "Output\" , MakeValidFileName(Family_Name + "" + "1/8 - Schedule 10S" + " - " +CStr(Pipe_Length)+ ".ipt"))
    Call values.Add("PL", Pipe_Length)
    MsgBox(fileName)
    strContentPartFileName = oFamily.CreateMember(1, Error1, strErrorMessage,refresh,isCustom,fileName ,values)
    
        

Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition
Dim oTG As TransientGeometry
oTG = ThisApplication.TransientGeometry
    
' Create a matrix.  
Dim oMatrix As Matrix
oMatrix = oTG.CreateMatrix

'Iterate through all of the occurrences
Dim oOccurrence As ComponentOccurrence

'place an instance of the component 
'in this case at 0,0,0
'positioned at the co-ordinates
oMatrix.SetTranslation(oTG.CreateVector(0, 0, 0)) 

oOccurrence = oAsmCompDef.Occurrences.Add(strContentPartFileName, oMatrix) 
oOccurrence.Grounded = True

Component.Color(oOccurrence.Name) = "Red"
End Sub


Public Shared Function MakeValidFileName(ByVal fileName As String) As String
        Dim invalidChars As Char() = New Char() {"/"c, "\"c, ":"c, "<"c, ">"c, """"c}
        If (fileName.IndexOfAny(invalidChars) < 0) Then
            Return fileName
        End If
        For Each ch As Char In invalidChars
            fileName = fileName.Replace(ch, "_"c)
        Next
        Return fileName
 End Function

Example File:http://grabcad.com/library/ilogic-content-center-1