Single laser line in save as... *.dxf

[Anonymous]

Hello all,

I'm working on auto generate pdf/dxf for inventor files with iLogic. For so far it's creating pdf and dxf as I wanted it to create, the difficulty was in the creation of dxf with the *.ini file and layers visible and invisible. But it works fine now. The thing is that the sometimes I want to have a single laser line in the *.dxf. I've found a work around of creating this with editing the flat pattern; made a extrusion and over that extrusion a sketch; with creating *.dxf I made the 'IV_UNCONSUMED_SKETCHES:Visibility=ON' so it's visible on the dxf. Problem solved I thought.

Now I get the product in my hand and the single laser line isn't cut 😞 the thing is that it is in a different layer (in the *.dxf file) so the laser program did not used it for its program. So I can asked the laser machine man to pay attention on the different layers or what I thing should be a better solution to let Inventor Merge the unconsumed sketches with Interior_Profile layer. This is possible with AutoCAD Mechanical so I hope Inventor can do this to in its save copy as... *.dxf.

Please let my know if you know how this is possible.

Best Regards,

Bram

[frederic.vandenplas]

Hi, 

This is my code for exporting to dxf, which may help you in the right direction.

This is my code (vb.net) , the only thing that may cause problems is this:

SplineTolerance=0,01 --> possible 0.01 instead of 0,01

 Private Sub SMExport_OnExecute(Context As NameValueMap) Handles SMExport.OnExecute

            Try

            Dim oIamDoc As AssemblyDocument = InvApp.ActiveDocument
            Dim oIamCompDef As AssemblyComponentDefinition = oIamDoc.ComponentDefinition
            Dim oRefDocs As DocumentsEnumerator = oIamDoc.AllReferencedDocuments

            For Each oRefDoc As Document In oRefDocs
                If oRefDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
                    If LCase(Trim(oRefDoc.PropertySets.Item("Inventor Summary Information").Item("Subject").Value)) <> "no" Then
                        Dim oDoc As PartDocument = InvApp.Documents.ItemByName(oRefDoc.FullFileName)
                        Dim oOccs As ComponentOccurrencesEnumerator = oIamCompDef.Occurrences.AllReferencedOccurrences(oDoc)

                        oDoc = InvApp.Documents.Open(oRefDoc.FullFileName, True)
                        If oDoc.ComponentDefinition.HasMultipleSolidBodies = False Then
                            Dim strMaterial As String = oDoc.ActiveMaterial.DisplayName
                            Dim strTotalFileName As String = InvApp.DesignProjectManager.ActiveDesignProject.WorkspacePath & "\2D\Laser\" & oRefDoc.PropertySets.Item("Design Tracking Properties").Item("Part Number").Value & " " & oDoc.ComponentDefinition.Parameters("Thickness").Value * 10 & "mm" & " " & oDoc.ActiveMaterial.DisplayName & " " & oOccs.Count & "st.dxf"

                            Dim oDataIO As DataIO = oDoc.ComponentDefinition.DataIO
                            oDataIO.WriteDataToFile("FLAT PATTERN DXF?AcadVersion=R12&SimplifySplines=True&MergeProfilesIntoPolyline=True&SplineTolerance=0,01&UnconsumedSketchesLayer=UnConsumedSketchesLayer&OuterProfileLayer=OuterProfile&InteriorProfilesLayer=InteriorProfile&AltRepFrontLayer=AltRepFront&AltRepBackLayer=AltRepBack&InteriorProfilesLayer=UnconsumedSketch&TangentRollLinesLayer=TangentRoll&RollLinesLayer=Roll&InvisibleLayers=IV_TANGENT;IV_BEND;IV_BEND_DOWN;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_FEATURE_PROFILES;IV_FEATURE_PROFILES_DOWN", strTotalFileName)
                            'oDataIO.WriteDataToFile("FLAT PATTERN DXF?AcadVersion=2000", strTotalFileName)
                        End If

                        InvApp.ActiveDocument.Close(True)
                    End If
                End If
                Next
            Catch ex As Exception
                MessageBox.Show(ex.ToString)
            End Try
        End Sub

[Anonymous]

Hello Frederic,

Thanks for you reply, I've tried your 'mergeprofilesintopolylines' but I don't think I need that. In the picture below you see 2 lines close to each other, that 2 lines I would like to 'merge'into one line. I don't think thats the function of the mergeprofilesintopolylines...

Best Regards,

Bram

[frederic.vandenplas]

Aha, now i see, did you ever tried the cosmetic welding line? It may be a better solution?

I did not test if there is a seperate layer for that.

Part is attached (Inventor 2015)

[Anonymous · Accepted solution]

Thanks for your reply, I work here with inv2012 😞

But I found a solution for my problem: In the picture below I've made a sketch en made it visible so it would me seen in the dxf. Now in the dxf creation I gave UnconsumedSketchesLayer and InteriorProfilesLayer the same Layer name and now it works. 

sOut = "FLAT PATTERN DXF?AcadVersion=2004&OuterProfileLayer=IV_OUTER_PROFILE&UnconsumedSketchesLayerColor=0;0;0&UnconsumedSketchesLayer=IV_INTERIOR_PROFILES&InteriorProfilesLayer=IV_INTERIOR_PROFILES&InvisibleLayers=IV_TANGENT;IV_BEND;IV_BEND_DOWN;IV_ROLL_TANGENT;IV_ARC_CENTERS"