Assy File face to dxf

[lkirit2000]

Hi 

How to create an inventor assy file surface to dxf file for laser cutting.

I am using Inventor 2020.

Rgds

[Xun.Zhang · Accepted solution]

Hello @lkirit2000,

Create a new part, derived the assembly in and select the face, export surface to dxf from the context menu.

Hope it helps!

[lkirit2000]

Hi 

I am still haven't solve the problem.

Please let me know how to make a derive part?

Rgds

[lkirit2000]

Hi Xun,

Please see the attached image below, when select all faces, I couldn't get any option " Export Face As ".

Is there any other way to do this ?

Rgds

[lkirit2000]

Hi 

I have attached image.

Rgds

[Xun.Zhang]

Hello @lkirit2000,

Create a new part, find the command Derive (3D Model\Create) and invoke it, select the assembly and complete the derive workflow. Now you have a part with all geometries from that assembly. Then, select a face, right click the mouse to bring up context menu, select Export face as...

Hope it helps!

[lkirit2000]

Hi Xun,

Thanks for your prompt response.

I my derived part has grrove, so I could not select all file in one right click.

When I select the multiple clicks with Ctrl, then right click the " Export Face As " option is not available ?

Rgds

[Xun.Zhang]

Hello @lkirit2000,

Only 1 piece of planar face is supported.

Please use Unwrap command to make bunch of faces into a single planar face. 

Hope it helps!

[S_May]

@lkirit2000 

[Xun.Zhang]

Hello @S_May,

This is really cool! 👏

[S_May]

'define the active document as an assembly file
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisApplication.ActiveDocument
oAsmName = Left(oAsmDoc.DisplayName, Len(oAsmDoc.DisplayName) -4)
'check that the active document is an assembly file
If ThisApplication.ActiveDocument.DocumentType <> kAssemblyDocumentObject Then
MessageBox.Show("Please run this rule from the assembly file.", "iLogic")
Exit Sub
End If
'get user input
RUsure = MessageBox.Show ( _
"This will create a DXF file for all of the asembly components that are sheet metal." _
& vbLf & "This rule expects that the part file is saved." _
& vbLf & " " _
& vbLf & "Are you sure you want to create DXF for all of the assembly components?" _
& vbLf & "This could take a while.", "iLogic - Batch Output DXFs ",MessageBoxButtons.YesNo)
If RUsure = vbNo Then
Return
Else
End If
oPath = ThisDoc.Path
oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
oContext = ThisApplication.TransientObjects.CreateTranslationContext
oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
oOptions = ThisApplication.TransientObjects.CreateNameValueMap
'get DXF target folder path
oFolder = oPath & "\" & oAsmName & " DXF Files"
'Check for the DXF folder and create it if it does not exist
If Not System.IO.Directory.Exists(oFolder) Then
System.IO.Directory.CreateDirectory(oFolder)
End If
'- - - - - - - - - - - - -
'- - - - - - - - - - - - -Component - - - - - - - - - - - -
'look at the files referenced by the assembly
Dim oRefDocs As DocumentsEnumerator
oRefDocs = oAsmDoc.AllReferencedDocuments
Dim oRefDoc As Document
'work the the drawing files for the referenced models
'this expects that the model has been saved
For Each oRefDoc In oRefDocs
iptPathName = Left(oRefDoc.FullDocumentName, Len(oRefDoc.FullDocumentName) - 3) & "ipt"
'check that model is saved
If(System.IO.File.Exists(iptPathName)) Then
Dim oDrawDoc As PartDocument
oDrawDoc = ThisApplication.Documents.Open(iptPathName, True)
oFileName = Left(oRefDoc.DisplayName, Len(oRefDoc.DisplayName))
Try
'Set the DXF target file name

Try
CustomName =iProperties.Value(oFileName, "Custom", "PF_PRT_ZNR")
Catch
CustomName ="XXX" 'Wert, wenn iPropertie PF_PRT_ZNR nicht existiert
End Try

oDataMedium.FileName = oFolder & "\" & CustomName  & " " & oFileName & ".dxf"

Dim oCompDef As SheetMetalComponentDefinition
oCompDef = oDrawDoc.ComponentDefinition
If oCompDef.HasFlatPattern = False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Dim sOut As String
sOut = "FLAT PATTERN DXF?AcadVersion=2004&OuterProfileLayer=IV_OUTER_PROFILE"
oCompDef.DataIO.WriteDataToFile( sOut, oDataMedium.FileName)
'just for check its works coretcly
'i=MessageBox.Show(oDataMedium.FileName, "Title",MessageBoxButtons.OKCancel)
'MessageBox.Show(i,"title",MessageBoxButtons.OK)
'If i=2 Then
'Exit Sub
'End If
oCompDef.FlatPattern.ExitEdit
Catch
End Try
oDrawDoc.Close
Else
End If
Next

[Xun.Zhang]

Hello @S_May,

How about Non-sheetmetal parts? Any more thoughts? 🙄

[S_May]

Hi @Xun.Zhang , @lkirit2000 

This solution is only for sheet metal parts, not for normal components and not for flattening in 2020....

[thenottakenname]

Would making a drawing and placing the view of the surface to be cut, then going to save as -> save copy as -> and changing the file type to dxf work? That's how I transport model views to AutoCAD.

[S_May]

@thenottakenname 

1. You must create all components as sheet metal
2. for the flat sheet you need no drawing