Ilogic to Change size on Content Center Components
Here is the iLogic demo rule that replaces the 1st 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
'---------------------------------------
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network
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,
Adam Nagy
Autodesk Platform Services
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")
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network
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,
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network
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.
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network
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?
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,
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network
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.
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network