turn off certain layers when exporting as dxf

[mindaV3J2J]

Hello,

I'm trying to export as dxf from parts; however, my script includes the tangent lines when exported, which means there are 3 bend lines instead of one. I want to turn off the IV_TANGENT and IV_ROLL_TANGENT layers.

My code is below.

```

Sub ExportFlatPatternToDXF2()

Dim SETFilePath As String
SETFilePath = "path"

If ThisApplication.ActiveDocument.DocumentType <> kAssemblyDocumentObject Then
MsgBox "Please open an assembly document.", vbExclamation, "iLogic"
Exit Sub
End If

Dim oAsmDoc As AssemblyDocument
Set oAsmDoc = ThisApplication.ActiveDocument

Dim oRefDocs As DocumentsEnumerator
Set oRefDocs = oAsmDoc.AllReferencedDocuments

Dim oRefDoc As Document
For Each oRefDoc In oRefDocs

If oRefDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
Dim oSheetMetDoc As PartDocument
Set oSheetMetDoc = ThisApplication.Documents.Open(oRefDoc.FullFileName, True)

Dim oCompDef As SheetMetalComponentDefinition
Set oCompDef = oSheetMetDoc.ComponentDefinition

Dim oDef As FlatPattern

' If oCompDef.HasFlatPattern = False Then
' oCompDef.Unfold
' End If
Set oDef = oCompDef.FlatPattern
If oDef Is Nothing Then GoTo NextOcc

Dim sOut As String
sOut = "FLAT PATTERN DXF?AcadVersion=2018&OuterProfileLayer=IV_INTERIOR_PROFILES"

Dim sFname As String
sFname = SETFilePath & "\" & oSheetMetDoc.DisplayName & ".dxf"

Dim oDataIO As DataIO
Set oDataIO = oCompDef.DataIO

oDataIO.WriteDataToFile sOut, sFname

oCompDef.FlatPattern.ExitEdit
End If
NextOcc:
Next oRefDoc

MsgBox "Flat patterns exported to " & SETFilePath, vbInformation, "iLogic"
End Sub

```

[johnsonshiue]

Hi! Another way to do it without using an iLogic rule is to save the seeing as a configuration. Turn off the layers and save the configuration (at the top of the dialog). Keep using the same cfg file and those layers will be turned off.

Many thanks!

[mindaV3J2J]

Hi!

Can you go into more detail? I'm a little lost with this response.

[Curtis_Waguespack]

Hi @mindaV3J2J 

I think you just need to update your sOut line to something like this:

Dim sOut As String
sOut = "FLAT PATTERN DXF?AcadVersion=2007" & _
"&OuterProfileLayer=IV_INTERIOR_PROFILES" &  _
"&InvisibleLayers = IV_TANGENT;IV_ROLL_TANGENT" 

Reference link:

https://help.autodesk.com/view/INVNTOR/2022/ENU/?guid=WriteFlatPatternAsDXF_Sample

related link:

https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/export-into-quot-dxf-quot-the-flat-p...

And here is an example of all options, just for reference:

Dim sOut As String
sOut="FLAT PATTERN DXF?AcadVersion=2007" &  _
"&TangentLayer=IV_TANGENT " &  _
"&BendLayer=IV_BEND" &  _
"&BendDownLayer=IV_BEND_DOWN" &  _
"&ToolCenterLayer=IV_TOOL_CENTER" &  _
"&ToolCenterDownLayer=IV_TOOL_CENTER_DOWN" &  _
"&ArcCentersLayer=IV_ARC_CENTERS" &  _
"&OuterProfileLayer=IV_OUTER_PROFILE" &  _
"&InteriorProfilesLayer=IV_INTERIOR_PROFILES" &  _
"&FeatureProfilesLayer=IV_FEATURE_PROFILES" &  _
"&FeatureProfilesDownLayer=IV_FEATURE_PROFILES_DOWN" &  _
"&AltRepFrontLayer=IV_ALTREP_FRONT" &  _
"&AltRepBackLayer=IV_ALTREP_BACK" &  _
"&UnconsumedSketchesLayer=IV_UNCONSUMED_SKETCHES" &  _
"&TangentRollLinesLayer=IV_ROLL_TANGENT" &  _
"&RollLinesLayer=IV_ROLL" &  _
"&InvisibleLayers=IV_TANGENT;IV_ROLL_TANGENT" &  _
"&TangentLayerColor=0;0;0 " &  _
"&endLayerColor=255;0;0" &  _
"&BendDownLayerColor=0;255;0" &  _
"&ToolCenterLayerColor=0;0;0" &  _
"&ToolCenterDownLayerColor=0;0;0" &  _
"&ArcCentersLayerColor=0;0;0" &  _
"&OuterProfileLayerColor=0;0;0" &  _
"&InteriorProfilesLayerColor=0;0;0" &  _ 
"&FeatureProfilesLayerColor=0;0;0" &  _
"&FeatureProfilesDownLayerColor=0;0;0" &  _
"&AltRepFrontLayerColor=0;0;0" &  _
"&AltRepBackLayerColor=0;0;0" &  _
"&UnconsumedSketchesLayerColor=-255;-255;-255" &  _
"&TangentRollLinesLayerColor=0;0;0" &  _
"&RollLinesLayerColor=0;0;0" &  _
"&MergeProfilesIntoPolyline=True"

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[mindaV3J2J]

Hi!

Thanks so much. However, when i run this, im getting an invalid procedure call or argument error, runtime error 5. Do you know why this is? 

Thanks so much

[mindaV3J2J]

Actually, it outputted correctly i just changed the acad version to match mine; however, the tangent lines are still there. Any other ideas?

[Curtis_Waguespack]

Hi @mindaV3J2J 

Ahh, I was just trying to match what you had in the original example as far as ACAD version, but goofed that up. You are correct there is no 2008 version ( I updated my examples).

I just did a quick test and see the same results as you. I'll see if I can figure out what the issue is. It's likely a syntax issue with the sOut line.

[mindaV3J2J]

Awesome i appreciate it. No rush whatsoever.

[Curtis_Waguespack · Accepted solution]

@mindaV3J2J , I had extra spaces in the sOut line that was causing the issue. I'll update my previous posts so it doesn't trip someone else up in the future.

Try this:

Dim sOut As String
sOut = "FLAT PATTERN DXF?AcadVersion=2007" & _
"&OuterProfileLayer=IV_INTERIOR_PROFILES" & _
"&InvisibleLayers=IV_TANGENT;IV_ROLL_TANGENT"

[mindaV3J2J]

worked!!! thanks so much

[mindaV3J2J]

Sorry last question and this is unrelated, is there a way i can get this to loop through multiple inventor assembly files and pirnt the dxfs of each assembly rather than just the one using VBA. I assume we will have to use visual basic for this.

[Curtis_Waguespack]

---

@mindaV3J2J wrote:

Sorry last question and this is unrelated, is there a way i can get this to loop through multiple inventor assembly files and pirnt the dxfs of each assembly rather than just the one using VBA. I assume we will have to use visual basic for this.

---

yeah, you can probably do this.

How are you identifying the assemblies?

Are they all in the same folder? All open in Inventor? Something else?

[mindaV3J2J]

yes they're all in the same folder. My coworker would like to be able to drop multiple assemblies in the same folder and output the respective flat parts in individual folders corresponding to the assembly it came from. thanks so much for your help as well

[Curtis_Waguespack]

@mindaV3J2J , 

This VBA example will open all the assemblies in a folder, and then close them. Add your DXF code where indicated.

Sub FindFilesWithComment()

    sName = ThisApplication.ActiveDocument.FullFileName
    Dim filesystem As Object
    Set filesystem = CreateObject("Scripting.FilesystemObject")
    
    Dim ActiveDoc As Document
    Set ActiveDoc = ThisApplication.ActiveDocument
   
    Dim FolderPath As String
    FolderPath = BrowseForFolder()
    
    If FolderPath = "" Then Exit Sub
    
    Dim oFSO As Object
    Dim oFolder As Object
    Dim oFile As Object
    Dim oFiles As Object

     
    Dim oFileNames As String
    oFileNames = "Files with comments: " & oComment
    Set oFSO = CreateObject("Scripting.FileSystemObject")
     
    Set oFolder = oFSO.GetFolder(FolderPath)
    
    For Each oFile In oFolder.Files
        If LCase(oFSO.GetExtensionName(oFile.Name)) = "iam" Then
        
            sFilename = FolderPath & "\" & oFile.Name
            Dim oAsmDoc As AssemblyDocument
            
            'set option to false to open invisible and run faster
            Set oAsmDoc = ThisApplication.Documents.Open(sFilename, True)
            
            MsgBox (oAsmDoc.FullFileName)
        
            Dim oRefDocs As DocumentsEnumerator
            Set oRefDocs = oAsmDoc.AllReferencedDocuments
        
            Dim oRefDoc As Document
            For Each oRefDoc In oRefDocs
                
                'put your DXF code here
                
            Next oRefDoc
            
            If Not ActiveDoc Is oAsmDoc Then oAsmDoc.Close (True) 'true = skip save
        
        End If
     
    Next oFile
    
    
End Sub
Function BrowseForFolder(Optional OpenAt As Variant) As Variant

    Dim ShellApp As Object
    Set ShellApp = CreateObject("Shell.Application"). _
    BrowseForFolder(0, "Please choose a folder", 0, OpenAt)
    On Error Resume Next
    BrowseForFolder = ShellApp.self.Path
    On Error GoTo 0
    Set ShellApp = Nothing
    Select Case Mid(BrowseForFolder, 2, 1)
    Case Is = ":"
        If Left(BrowseForFolder, 1) = ":" Then GoTo Invalid
    Case Is = "\"
        If Not Left(BrowseForFolder, 1) = "\" Then GoTo Invalid
    Case Else
        GoTo Invalid
    End Select

    Exit Function

Invalid:
    BrowseForFolder = ""
End Function

[Apollo_Tamworth]

Hi Mate,
What about these 2 layers:
IV_MARK_SURFACE
And 
IV_MARK_SURFACE_BACK.
I need  to change the layer's name, but I can not.