how to give the good Parts name

[hugo7]

Hi i want that my rules generate the name off the parts automatically

heres my post my problem is at line 30 

[FINET_Laurent]

Hello @hugo7,

How would the name be formated ? We can have any name you can think of. 

Also, please copy paste the code here so we can implement it for you.

Kind regards,

FINET L.

[hugo7]

oDoc = ThisDoc.Document

  'check if the part is a sheet metal part
  If oDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
                   
    oDoc = ThisApplication.ActiveDocument
    Dim oCompDef As SheetMetalComponentDefinition
    oCompDef = oDoc.ComponentDefinition
    
    If oCompDef.HasFlatPattern = False Then
        oCompDef.Unfold
    Else
        oCompDef.FlatPattern.Edit
    End If
                
    Dim sOut As String
    Dim oPath As String
                                
    oPath = ThisDoc.Path & "\DXF Flat & Step" 
	
                
    If Not System.IO.Directory.Exists(oPath) Then
        System.IO.Directory.CreateDirectory(oPath)
    End If
                
    Dim sFname As String
   
    sOut = "FLAT PATTERN DXF?AcadVersion=2004&RebaseGeometry=True&OuterProfileLayer=0&OuterProfileLayerColor=0;0;0&InteriorProfilesLayer=0&InteriorProfilesLayerColor=0;0;0;0;0;IV_OUTER_PROFILE;IV_INTERIOR_PROFILES;IV_FEATURE_PROFILES;IV_FEATURE_PROFILES_DOWN;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_ROLL_TANGENT;IV_ROLL&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_UNCONSUMED_SKETCHES;IV_BEND;IV_BEND_DOWN"
               
    sFname = oPath & "test"& ".dxf"
    oCompDef.DataIO.WriteDataToFile(sOut, sFname)
	
    'MessageBox.Show("Your file was saved in the following dirctory: " + sFname)
  Else
    'MessageBox.Show("Only sheet metal parts can be exported as DXF. Nice Try! :-)")
  End If

[sebastien_forman]

hello, try that

oDoc = ThisDoc.Document

' Check if the part is a sheet metal part
If oDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
    oDoc = ThisApplication.ActiveDocument
    Dim oCompDef As SheetMetalComponentDefinition
    oCompDef = oDoc.ComponentDefinition
    
    ' Check if the part has a flat pattern
    If Not oCompDef.HasFlatPattern Then
        oCompDef.Unfold
    Else
        oCompDef.FlatPattern.Edit
    End If
                
    Dim oPath As String
    oPath = ThisDoc.Path & "\DXF Flat & Step"
                
    ' Check if the output directory exists, if not, create it
    If Not System.IO.Directory.Exists(oPath) Then
        System.IO.Directory.CreateDirectory(oPath)
    End If
                
    Dim sFname As String
    sFname = oPath & "\"&ThisDoc.FileName &"_flat.dxf" ' Correctly formatted DXF file path
    
    ' Define parameters for DXF export
    Dim sOut As String
    sOut = "FLAT PATTERN DXF?AcadVersion=2004&RebaseGeometry=True&OuterProfileLayer=0&OuterProfileLayerColor=0;0;0&InteriorProfilesLayer=0&InteriorProfilesLayerColor=0;0;0;0;0;IV_OUTER_PROFILE;IV_INTERIOR_PROFILES;IV_FEATURE_PROFILES;IV_FEATURE_PROFILES_DOWN;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_ROLL_TANGENT;IV_ROLL&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_UNCONSUMED_SKETCHES;IV_BEND;IV_BEND_DOWN"
               
    ' Export the sheet metal part as a DXF file
    oCompDef.DataIO.WriteDataToFile(sOut, sFname)
Else
    ' Display a message if the part is not a sheet metal part
    MessageBox.Show("Only sheet metal parts can be exported as DXF.")
End If

[hugo7]

Thank that works fine

now can you make this rule to save at the same doc ?

i need to generate a dxf and a .step or combine the 2 rules if its possible ?

' Get the STEP translator Add-In.
Dim oSTEPTranslator As TranslatorAddIn
oSTEPTranslator = ThisApplication.ApplicationAddIns.ItemById("{90AF7F40-0C01-11D5-8E83-0010B541CD80}")
Dim oContext As TranslationContext
oContext = ThisApplication.TransientObjects.CreateTranslationContext
Dim oOptions As NameValueMap
oOptions = ThisApplication.TransientObjects.CreateNameValueMap

If oSTEPTranslator.HasSaveCopyAsOptions(ThisApplication.ActiveDocument, oContext, oOptions) Then
    ' Set application protocol.
    ' 2 = AP 203 - Configuration Controlled Design
    ' 3 = AP 214 - Automotive Design
    oOptions.Value("ApplicationProtocolType") = 3
    ' Other options...
    'oOptions.Value("Author") = ""
    'oOptions.Value("Authorization") = ""
    'oOptions.Value("Description") = ""
    'oOptions.Value("Organization") = ""
    oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
    Dim oData As DataMedium
    oData = ThisApplication.TransientObjects.CreateDataMedium
    oData.FileName = ThisDoc.PathAndFileName(False) & ".stp"
oSTEPTranslator.SaveCopyAs(ThisApplication.ActiveDocument, oContext, oOptions, oData)
End If

[sebastien_forman · Accepted solution]

try that 😉

Sub main()
    ' Get the active document
    oDoc = ThisDoc.Document

    ' Check if the part is a sheet metal part
    If oDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
        ' Set the active document as the current document
        oDoc = ThisApplication.ActiveDocument
        Dim oCompDef As SheetMetalComponentDefinition
        oCompDef = oDoc.ComponentDefinition
        
        ' Check if the part has a flat pattern
        If Not oCompDef.HasFlatPattern Then
            oCompDef.Unfold
        Else
            oCompDef.FlatPattern.Edit
        End If
                    
        ' Define the output directory path
        Dim oPath As String
        oPath = ThisDoc.Path & "\DXF Flat & Step"
                    
        ' Check if the output directory exists, if not, create it
        If Not System.IO.Directory.Exists(oPath) Then
            System.IO.Directory.CreateDirectory(oPath)
        End If
                    
        ' Define the DXF file name and path
        Dim sFname As String
        sFname = oPath & "\"&ThisDoc.FileName &"_flat.dxf" ' Correctly formatted DXF file path
        
        ' Define parameters for DXF export
        Dim sOut As String
        sOut = "FLAT PATTERN DXF?AcadVersion=2004&RebaseGeometry=True&OuterProfileLayer=0&OuterProfileLayerColor=0;0;0&InteriorProfilesLayer=0&InteriorProfilesLayerColor=0;0;0;0;0;IV_OUTER_PROFILE;IV_INTERIOR_PROFILES;IV_FEATURE_PROFILES;IV_FEATURE_PROFILES_DOWN;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_ROLL_TANGENT;IV_ROLL&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_UNCONSUMED_SKETCHES;IV_BEND;IV_BEND_DOWN"
                   
        ' Export the sheet metal part as a DXF file
        oCompDef.DataIO.WriteDataToFile(sOut, sFname)
        
        ' Export STEP
        ExportStep(oPath, ThisDoc.FileName)
        
    Else
        ' Display a message if the part is not a sheet metal part
        MessageBox.Show("Only sheet metal parts can be exported as DXF.")
    End If
End Sub

Function ExportStep(ByVal oPath As String, ByVal fileName As String)
    ' Get the STEP translator Add-In
    Dim oSTEPTranslator As TranslatorAddIn
    oSTEPTranslator = ThisApplication.ApplicationAddIns.ItemById("{90AF7F40-0C01-11D5-8E83-0010B541CD80}")
    Dim oContext As TranslationContext
    oContext = ThisApplication.TransientObjects.CreateTranslationContext
    Dim oOptions As NameValueMap
    oOptions = ThisApplication.TransientObjects.CreateNameValueMap

    ' Set the STEP file folder
    oFolder = oPath

    ' Check for the STEP folder and create it if it does not exist
    If Not System.IO.Directory.Exists(oFolder) Then
        System.IO.Directory.CreateDirectory(oFolder)
    End If

    ' Check if the translator has save copy options
    If oSTEPTranslator.HasSaveCopyAsOptions(ThisDoc.Document, oContext, oOptions) Then
        ' Set application protocol
        oOptions.Value("ApplicationProtocolType") = 3 ' 3 = AP 214 - Automotive Design
        
        ' Set the context type
        oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
        
        ' Create a data medium
        Dim oData As DataMedium
        oData = ThisApplication.TransientObjects.CreateDataMedium
        
        ' Set the STEP file name and path
        oData.FileName = oFolder & "\" & fileName & "-flat.stp"
        
        ' Save the part as a STEP file
        oSTEPTranslator.SaveCopyAs(ThisDoc.Document, oContext, oOptions, oData)
    End If
End Function

[hugo7]

thank you very helpfull

have a good one !