Automate ipart flat pattern export to dxf

[dan_goodrich89]

I'm trying to modify Clint Browns Automate DXF Flat Patterns iLogic code to run through all ipart members and export dxfs https://clintbrown.co.uk/2018/12/09/dxf/

It works on the active iPart, adjusting the code to name the dxf using the ipart number, but I'm struggling with looping it though all iPart members.

[JelteDeJong · Accepted solution]

does this work for you?

Dim doc As PartDocument = ThisDoc.Document

If (doc.ComponentDefinition.IsiPartFactory = False) Then
    MsgBox("This is not an iPart factory")
End If

Dim fact As iPartFactory = doc.ComponentDefinition.iPartFactory
For Each row As iPartTableRow In fact.TableRows
    fact.DefaultRow = Row
    doc.Update()
    doc.Update2(False)

    Dim oCompDef As SheetMetalComponentDefinition = doc.ComponentDefinition
    If oCompDef.HasFlatPattern = False Then
        oCompDef.Unfold()
    Else
        oCompDef.FlatPattern.Edit
    End If

    'DXF Settings
    Dim sOut As String
    sOut = "FLAT PATTERN DXF?AcadVersion=2000&OuterProfileLayer=IV_INTERIOR_PROFILES"
    Dim sFname As String = "c:\temp\" & ThisDoc.FileName(False) & "_" & Row.MemberName & ".dxf"

    'Export the DXF and fold the model back up
    oCompDef.DataIO.WriteDataToFile(sOut, sFname)
    oCompDef.FlatPattern.ExitEdit()
Next

[dan_goodrich89]

Works perfectly, thank you!

[Anonymous]

First and foremost thank you for the great piece of code you have provided here.

I am trying to do something similar, I made a recent forum post about it, for reference:

https://forums.autodesk.com/t5/inventor-customization/ilogic-code-to-export-all-iparts-as-dxf-or-dwg...

But I tried your code on a flat pattern drawing. It went through all the iParts and seemed like it was saving it or doing something since it went through each and every single drawing, however I cannot find where these files ended up... Code ran flawlessly no errors.

[aurel_e]

Have you looked at   "c:\temp\" ?

[KrishR330]

Dim sFname As String = "c:\temp\" & ThisDoc.FileName(False) & "_" & Row.MemberName & ".dxf"

I am trying to name the DXF file with values of few custom parameters of my iPart file instead of Row.MemberName.  Can you help change the code accordingly?

 Thanks and Regards,

Krish

[floccipier]

@JelteDeJong brilliant as always. thanks for this simple and effective code.