Ilogic to Change size on Content Center Components

[Anonymous]

Good afternoon all,

I have a bit of a challenge I'm trying to solve.

I have a pipe assembly that has a few Ebows and Tee's in it. I need to change the size of some of the Elbows and Tee's and have been looking for a way to reach into the content center and change specific parts within my assembly.

I have given the parts to be changed a specific name in the browser but am unable to get much further from there.

Has anyone tried this? And better yet, any success?

If anyone could share a little insight with me I'd appreciate it.

Thanks,

Jeff

IV2014 SP2

[mwighton]

Do you want to replace the part or update it to a new size?

[Anonymous]

I wish to change it's size but would like to be able to replace it. Right now my parts are CPVC but there are variations that require it to all be PVC.

If I have to have 2 different master assemblies for the different materials, I'll do that.

[mwighton]

You can use iLogic to change the size and material of the part, at the part level.

Then in your assembly call the part rule and that will allow you to update it from the assembly file.

If need be you can also replace the parts.

The only problem with this approach is that if you have multiple instances of the same part, as you update 1 they will all change unless you save it as a different part, which may in turn mess up the automation.

[Anonymous]

I have been down that route, I am trying to access the content center " Change Size" thru ilogic.
I have to change the size of the middle "Tee" for different applications. It's easy to do manually so it must be a real pain to do with code.



[cid:image001.png@01D0D4DC.4D913540]

[Vladimir.Ananyev]

Here is the iLogic demo rule that replaces the 1^st component with another family member with the known row number.  Here the new member row is 4.

'This iLogic demo replaces the given standard component
'with another member from same family.

' row number of the new family member .
Dim NewRow As Integer = 4

'active assembly s
Dim oMainAsm As AssemblyDocument = ThisDoc.Document
Dim oAsmDef As AssemblyComponentDefinition = oMainAsm.ComponentDefinition

' get the occurrence by its position in the occurrences collection
Dim oOcc As ComponentOccurrence = oAsmDef.Occurrences.Item(1)
Dim oDef As PartComponentDefinition = oOcc.Definition
Dim oDoc As PartDocument = oDef.Document

'reference to the CC properties - oProps
Dim oPropSets As PropertySets = oDoc.PropertySets
Dim oProps As PropertySet = oPropSets.Item("Content Library Component Properties")

' family id
Dim oProp As Inventor.Property = oProps.Item("FamilyId")
Dim FamilyId As String = oProp.Value
'MsgBox("FamilyId: " + FamilyId)

'reference to the ContentFamily
Dim oContentCenter As ContentCenter = ThisApplication.ContentCenter
Dim oFamily As ContentFamily = oContentCenter.GetContentObject("v3#" + FamilyId + "#")  
'MsgBox("Content Family DisplayName:  " + oFamily.DisplayName & vbNewLine & _
'	    "Rows in Family:  " & oFamily.TableRows.Count )

'create new member file
Dim ErrorType As MemberManagerErrorsEnum
Dim strContentPartFileName As String
Dim strErrorMessage As String
strContentPartFileName = oFamily.CreateMember(NewRow, ErrorType, strErrorMessage)

'replace the existing component with the new one
oOcc.Replace(strContentPartFileName, False)

Beep
'---------------------------------------

[Anonymous]

Vladimir,

This looks like what I am trying to do.

I will be back in the office next week to try it.

Thank You for taking the time to look into this for me.

Jeff

[Jef_E]

Hi,

I find this a wonderful topic. But for me personal the essential part has not been addressed from the OP's question.

For me a important point is that he needs to change the size in the original question. I would also like to do this but in the API there is only a example for replacing the content-center part.

---

@Anonymous wrote:
I need to change the size of some of the Elbows and Tee's

---

---

@Anonymous wrote:
but would like to be able to replace it

---

So I think the main question here is, can you place a standard or custom content center component. And then change it's size via the API?

What is answered, is the part how to replace it. But this is a different operation with different consequences.

In example you place a custom content center in the assembly. This obligates you to save it somewhere.

• You want to change it's size, the components choice is correct but not the size. No new part is required (when done manually) because the part will get it's new parameters from the content center. This will also mean that all extra modifications are retained so no work is lost.

• When you replace this file with the same part from the content center to change it's size, a new part is required so you will have to save it (Now you have 2 files that are the same but with diffrent sizes). Plus all the extra modifications you have made on the part are now gone because they are made in the replaced file.

So we know how to replace it from the content center as shown by @Vladimir.Ananyev, but can we change it's size too? If not, I will be obligated to look towards iParts to do the job, but my favor goes to the content center.

[adam.nagy]

Hi,

I played around with things a bit.

If I inserted the Content Center part as Standard, then when changing the size through the UI the same thing will happen: the new size will be created and the component will be replaced with it, i.e. the component will reference a different part file.

If I inserted the Content Center part as Custom, then it's only created once, and when changing the size through the UI then a new member will be created and it will overwrite the originally created part file - so no "replace" happens as the referenced part file is simply overwritten with the newly created one. Should be possible through the API as well.

Cheers,

[Jef_E]

---

@adam.nagy wrote:

Hi,

I played around with things a bit.

If I inserted the Content Center part as Standard, then when changing the size through the UI the same thing will happen: the new size will be created and the component will be replaced with it, i.e. the component will reference a different part file.

If I inserted the Content Center part as Custom, then it's only created once, and when changing the size through the UI then a new member will be created and it will overwrite the originally created part file - so no "replace" happens as the referenced part file is simply overwritten with the newly created one. Should be possible through the API as well.

Cheers,

---

Could you provide a sample for doing this via the API? This would be very helpfull. All I could find in the Programming help is this sample but it's not quite the same? It does not changes the size but replaces the component?

Spoiler

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

    ' Prompt user to pick an occurrence
    Dim oOcc As ComponentOccurrence
    Set oOcc = ThisApplication.CommandManager.Pick(kAssemblyOccurrenceFilter, "Pick occurrence to replace")

    If oOcc.DefinitionDocumentType <> kPartDocumentObject Then
        MsgBox "Occurrence does not reference a content part."
        Exit Sub
    End If

    Dim oOccDef As PartComponentDefinition
    Set oOccDef = oOcc.Definition

    If Not oOccDef.IsContentMember Then
        MsgBox "The occurrence does not reference a content part."
        Exit Sub
    End If

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

    ' Get the content node (category) "Fasteners:Bolts:Hex Head"
    Dim oContentNode As ContentTreeViewNode
    Set oContentNode = oContentCenter.TreeViewTopNode.ChildNodes.Item("Fasteners").ChildNodes.Item("Bolts").ChildNodes.Item("Hex Head")

    ' Get the "ISO 4015" Family object.
    Dim oFamily As ContentFamily
    For Each oFamily In oContentNode.Families
        If oFamily.DisplayName = "ISO 4015" Then
            Exit For
        End If
    Next

    ' Create a member based on the second row of the family.
    Dim error As MemberManagerErrorsEnum
    Dim strContentPartFileName As String
    Dim strErrorMessage As String
    strContentPartFileName = oFamily.CreateMember(2, error, strErrorMessage)

    Call oOcc.Replace(strContentPartFileName, False)
End Sub

[Vladimir.Ananyev]

You should change the appropriate value in the members' active iPartTableRow as shown in the following vba code sample:

Sub test3()
    
    Dim oAssyDoc As Inventor.Document
    Set oAssyDoc = ThisApplication.ActiveDocument
    Dim oOccs As ComponentOccurrences
    Set oOccs = oAssyDoc.ComponentDefinition.Occurrences
    'custom iPart member - here it's the first occurrence
    Dim oOcc As ComponentOccurrence
    Set oOcc = oOccs.Item(1)
    
    'reference to the iPart member
    Dim oDef As PartComponentDefinition
    Set oDef = oOcc.Definition
    Dim oMember As iPartMember
    Set oMember = oDef.iPartMember
    
    'reference to the iPart factory
    Dim oFactory As iPartFactory
    Set oFactory = oMember.ParentFactory
    
    'table columns list
    Dim oColumns As iPartTableColumns
    Set oColumns = oFactory.TableColumns
    
    'table rows list
    Dim oRows As iPartTableRows
    Set oRows = oFactory.TableRows
    
    Dim oRow As iPartTableRow
    Dim oColumn As iPartTableColumn
    Dim i As Integer, j As Integer
    
    'print the  current table content
    'headers
    Debug.Print "i",
    For j = 1 To oColumns.Count
        Set oColumn = oColumns.Item(j)
        Debug.Print oColumn.DisplayHeading,
    Next j
    Debug.Print
    'table cells' values
    For i = 1 To oRows.Count
        Set oRow = oRows.Item(i)
        Debug.Print i,
        For j = 1 To oColumns.Count
            Debug.Print oRow.Item(j).value,
        Next j
        Debug.Print
    Next
    
    'change angle value in row 4
    Set oRow = oMember.row
    oRow.Item(4).value = "38 deg"  '<--- change to the required value
    'reset active row
    Call oMember.ChangeRow(oRow)
    
    oAssyDoc.Update
    
    
    'print the updated table content
    Debug.Print " --- Updated table ---"
    'headers
    Debug.Print "i",
    For j = 1 To oColumns.Count
        Set oColumn = oColumns.Item(j)
        Debug.Print oColumn.DisplayHeading,
    Next j
    Debug.Print
    'table cells' values
    For i = 1 To oRows.Count
        Set oRow = oRows.Item(i)
        Debug.Print i,
        For j = 1 To oColumns.Count
            Debug.Print oRow.Item(j).value,
        Next j
        Debug.Print
    Next
    
    Beep
End Sub

I tested this code with the custom iPart file attached.

i             Member        Part Number   d0            d1            
 1            Part1-01      Part1-01      3             0 deg         
 2            Part1-03      Part1-03      2 in          30            
 3            Part1-04      AAA           3 in          45            
 4            Part1-02      Part1-02      2 in          18 deg        
 --- Updated table ---
i             Member        Part Number   d0            d1            
 1            Part1-01      Part1-01      3             0 deg         
 2            Part1-03      Part1-03      2 in          30            
 3            Part1-04      AAA           3 in          45            
 4            Part1-02      Part1-02      2 in          38 deg  

Here is equivalent iLogic code (with debug printing removed). Place it in the assemble document.

Dim oAssyDoc As Inventor.AssemblyDocument = ThisDoc.Document
Dim oOccs As ComponentOccurrences = oAssyDoc.ComponentDefinition.Occurrences
 
'custom iPart member - here it's the first occurrence
Dim oOcc As ComponentOccurrence = oOccs.Item(1)
 
'reference to the iPart member
Dim oDef As PartComponentDefinition = oOcc.Definition
Dim oMember As iPartMember = oDef.iPartMember
 
'reference to the iPart factory
Dim oFactory As iPartFactory = oMember.ParentFactory
 
'change angle value in row 4
Dim oRow As iPartTableRow = oMember.row
oRow.Item(4).Value = "28 deg"  '<--- change to the required value
 
'reset active row
Call oMember.ChangeRow(oRow)
 
oAssyDoc.Update
Beep
MsgBox("DONE")

[Jef_E]

Hi, thanks for that sample code. But i'm not sure that i'm getting it 100% Where is the link to this thread: "Ilogic to Change size on Content Center Components"?

[Vladimir.Ananyev]

Could you try the following code.  It changes the size of the custom member via changing active row (plus prints some debugging information):

Sub TestObject()
    Dim oApp As Inventor.Application
    Set oApp = ThisApplication
    Dim oMainAsm As AssemblyDocument
    Set oMainAsm = oApp.ActiveDocument
    
    Dim oAsmDef As AssemblyComponentDefinition
    Set oAsmDef = oMainAsm.ComponentDefinition
    
    ' get the 1st occurrence
    Dim oOcc As ComponentOccurrence
    Set oOcc = oAsmDef.Occurrences.Item(1)
    Dim oDef As PartComponentDefinition
    Set oDef = oOcc.Definition
    Dim oDoc As PartDocument
    Set oDoc = oDef.Document
    
    'reference to the CC properties - oProps
    Dim oPropSets As PropertySets
    Set oPropSets = oDoc.PropertySets
    Dim oProps As PropertySet
    Set oProps = oPropSets.Item("Content Library Component Properties")
    
    ' family id
    Dim oProp As Inventor.Property
    Set oProp = oProps.Item("FamilyId")
    Dim FamilyId As String
    FamilyId = oProp.value
    Debug.Print "FamilyId: " + FamilyId
    
    'reference to the ContentFamily
    Dim oContentCenter As ContentCenter
    Set oContentCenter = oApp.ContentCenter
    Dim oFamily As ContentFamily
    Set oFamily = oContentCenter.GetContentObject("v3#" + FamilyId + "#")
    Debug.Print "Content Family DisplayName:  " + oFamily.DisplayName
    
    Debug.Print "Rows in Family:  " & oFamily.TableRows.Count
    
    
    ' get the current MemberId
    Set oProp = oProps.Item("MemberId")
    Dim MemberId As Integer
    MemberId = CInt(oProp.value)
    Debug.Print "Current MemberId (row): " + CStr(MemberId)

    
    'find nCol - table column for PARTNUMBER
    Dim nCol As Integer
    nCol = -1
    Dim i As Integer
    For i = 1 To oFamily.TableColumns.Count
      If oFamily.TableColumns.Item(i).InternalName = "PARTNUMBER" Then
        nCol = i
        Exit For
      End If
    Next
    If nCol < 0 Then
      'column not found - error message
      Exit Sub
    End If

    
    'table row for the member
    Dim oRow As ContentTableRow
    Set oRow = oFamily.TableRows.Item(MemberId)
    'get PartNumber
    Dim partNumber As String
    partNumber = oRow.Item(nCol).value
    Debug.Print "Member PartNumber: " & partNumber & vbCr

    
    ' Create a member based on the NewRow row in the family.
    Dim NewRow As Integer
    NewRow = 3  ' <--------------------- new member row
    
    Dim error As MemberManagerErrorsEnum
    Dim strContentPartFileName As String
    Dim strErrorMessage As String
    strContentPartFileName = oFamily.CreateMember(NewRow, error, strErrorMessage)

    Call oOcc.Replace(strContentPartFileName, False)
    
    Beep
End Sub

cheers,

[Jef_E]

Yes! This is some good stuff. But unfortunally i'm getting this error, I don't see how you could run this code past this error? Or am I doing something wrong?

Debug data before the error, seems to be all correct.

FamilyId: d560d377-52f5-4751-b731-d8716562d772
Content Family DisplayName:  EM - WN-flanges - ASME B16.5
Rows in Family:  109

Error produced on CInt(oProp.Value)

' get the current MemberId
oProp = oProps.Item("MemberId")
Dim MemberId As Integer
MemberId = CInt(oProp.Value)
Debug.Print("Current MemberId (row): " + CStr(MemberId))

Error message:

An unhandled exception of type 'System.InvalidCastException' occurred in Microsoft.VisualBasic.dll
Additional information: Conversion from string "12d3857b-0da9-4bfd-ae39-ae80745c" to type 'Integer' is not valid.

Please don't tell me that this is a version issue, i'm using Autodesk Inventor 2014 SP2

[Jef_E]

I did some research on this error and it's quite logic that it's produced. In the programming help is stated:

kMemberIdContentLibrary
20
MemberId: String (VT_BSTR), Read Only, No UI, Row Id of the Member in the Family Table. Used to uniquely identify this Member in the Family Table. 

So the MemberID should be a string as shown in the error message and therefor could not be convented to Integer.

Thus I made a little adjustment in the piece that produces the error. Now it works for me.

' get the current MemberId
oProp = oProps.Item("MemberId")
Dim MemberId As String
MemberId = oProp.Value
Debug.Print("Current MemberId (row): " + MemberId)

Now to illustrated what happend using this code:

I placed a standard content center part as custom into my assembly, let the code do it's magic and voila, another size of flange appeared on the spot.

The problem, this now is a standard content center part. So it did not change it's size but it replaced it. (obvious because at the end is stated oOcc.Replace)

The question still remains: can you change the size for content center parts via API without replacing it? ( Or should I use this technique to find the row values and adjust them into the part directly if it's a custom part, would be alot more coding.. Not my favorite solution because it's diffrent for each part.)

This piece of code is extremely usefull for me, but I would like to go a little bit further and change the size. Because we do like to work with custom content center parts where I work.

[Vladimir.Ananyev]

You cannot change the Inventor Content Center workflow.  It treats standard and custom CC components a little bit differently.  You may copy all the required standard components into the custom library or develop some alternatuive solution for CC to work around but this would require a lot of coding.

[Jef_E]

Correct me if i'm wrong, but how is this adjusting the content center workflow. The way I see it, it has 2 flows, but only 1 is accessible via the API?

For now, we are using the replace from content center technique? And we can't use the change size technique?

[Vladimir.Ananyev]

Let’s clarify – “Change Size” is a CC’s command. It will firstly generate a new file (they are based on the same family template file), and then replace.

You may customize your Custom CC member providing custom parameters’ values to the CreateMember method via the NameValueMap argument (see the code sample in the attachment):

' add length
Dim nvm As NameValueMap
Set nvm = ThisApplication.TransientObjects.CreateNameValueMap
Call nvm.Add("B_L", length) 'B_L - length parameter name

'set the full filename for the member file
Dim folder As String
folder = Left(oAsmDoc.FullFileName, InStrRev(oAsmDoc.FullFileName, "\"))
Dim fname As String
fname = folder & "DIN 1026 - " & memberName & " - " & CStr(length) & ".ipt"

'create member file (gives an error if file was already created)
Dim failureReason As MemberManagerErrorsEnum
Dim failureMessage As String
Dim memberFilename As String
memberFilename = family.CreateMember( _
        row, failureReason, failureMessage, _
        ContentMemberRefreshEnum.kRefreshOutOfDateParts, _
        True, fname, nvm)

If custom parts saved in the project workspace they are treated as regular Inventor files. In this case it is also possible to change their parameters (e.g., channel length is controlled by the user parameter B_L).

cheers,

[Jef_E]

Thank you @Vladimir.Ananyev for all your reply's. It's really helpfull. But just one more thing (for using content center parts as custom).. You say "It will firstly generate a new file (they are based on the same family template file), and then replace"

How does Inventor then do this? I have a flange placed as Custom and I added a chamfer on it. Now if I change size, it still is the same fle on the same location as I saved it + it still has the chamfer. Does it still generate a new file and then replace it?

Question: is it possible to get the Template Parameters for the content center family that is beeing used? If yes this would be a easy way to have a code that can change all the sizes for all the content center parts that are saved as custom.

[Vladimir.Ananyev]

Sorry for the long delay but this topic is interesting enough and we discussed it internally for some time.

If we talk about “Change Size as custom”, there is no existed API to support currently.

There is a series of internal logic that are implemented in CC.

For example,

• Get all parameters need to change
• Get the new values
• Batch Edit the parameters

…

• Update Part

In this case Inventor changes existing part document via Parameters API + iProperties APIs directly.  No new part, no replacement.  Of course, it is always better to have an appropriate API function, but in this particular case you are able to implement this workflow yourself.

You start with your CC custom component saved locally.  You know its row in the CC family table and you know the new target row. 

As user parameter names are the same as corresponding ContentTableColumn’s InternalNames you may update the user parameters’ values with the values read from the corresponding cells in the target row.   The following function could be used to find the required column number by user parameter name:

Function GetColumnByName(ByRef family As ContentFamily, _
                         ByVal ColumnName As String) As Integer
    'find CC family table column by its name ColumnName
    Dim i As Integer
    For i = 1 To family.TableColumns.Count
        If family.TableColumns.Item(i).InternalName = ColumnName Then
            Debug.Print "f-n GetColumnByName: " & i & "  " & family.TableColumns.Item(i).InternalName
            GetColumnByName = i
            Exit Function
        End If
    Next
    GetColumnByName = -1
End Function

You should also update part number, stock number, MemberId, Member Revision and may be other iProperties as well.  Finally you should rename component in the browser (name is usually based on part number) and update both part and assembly documents.

It is not easy to implement a general utility that could work with any CC family, but fortunately in most cases you work with several particular families (e.g., structural shapes – angles, channels, I-beams, etc.).  This could simplify this implementation.