DXF flat pattern using Inventor iLogic - MFG Master Class

by Clint Brown

At the recent CADline MFG Mater Class events, I showed how easy it was to automatically export DXF flat patterns from Inventor using iLogic.

In this blog post, I want to share some of the code I used, and I also wanted to show those users that are new to iLogic, how to get the rule working in their .ipt files.

The rule automatically creates a flat pattern of the part, saved to the same location as the current part. Note that the file MUST be saved before running the rule to avoid errors.

The first thing to do is to create a new sheet metal part. And to then get the iLogic browser up, this is done by clicking on the View Tab, then the User Interface Dropdown, and then by ticking iLogic Browser

In the top of your iLogic browser, right click on the part name, and then select “Add Rule”

Give the rule a name

Then paste the code below into the  rule and close the dialogue box. As soon as you do this, the rule will run.

Copy and paste all of the code between the lines (Sub Main to End Sub)

_{Sub Main}

_{DefaultChoice = True}

_{CadlinePathProperty()}

_Cadline()

_{End Sub}

_{Sub CadlinePathProperty()}

_{Dim FilePATH As String = "FilePATH"}

_{customPropertySet = ThisDoc.Document.PropertySets.Item _}

_{("Inventor User Defined Properties")}

_Try

         _{prop= customPropertySet.Item(FilePATH)}

_Catch

            _{customPropertySet.Add("", FilePATH)}

_{End Try}

_{If iProperties.Value("Custom", "FilePATH") = "" Then}

_{iProperties.Value("Custom", "FilePATH") = "C:\"}

_Else

_{End If}

_{Dim partDoc As PartDocument}

_{If ThisApplication.ActiveDocument.DocumentType <> kPartDocumentObject Then}

_{MessageBox.Show ("Please open a part document", "iLogic")}

_{End If}

_{FilePATH = InputBox("Enter a FilePATH for part file", "iLogic", iProperties.Value("Custom", "FilePATH"))}

_{iProperties.Value("Custom", "FilePATH") = FilePATH}

_{End Sub}

_{Public Sub Cadline()}

    _{Dim oDoc As PartDocument}

    _{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 sPATH As String}

    _{sPATH = iProperties.Value("Custom", "FilePATH")}

    _{sOut = "FLAT PATTERN DXF?AcadVersion=2000&OuterProfileLayer=IV_INTERIOR_PROFILES"}

    _{Dim sFname As String}

    _{sFname = sPATH & "\" & ThisDoc.FileName(False) & ".dxf"}

    _{MessageBox.Show("DXF SAVED TO: " & sFname ,"DXF Saved", MessageBoxButtons.OK)}

    _{oCompDef.DataIO.WriteDataToFile( sOut, sFname)}

  _{oDoc = ThisApplication.ActiveDocument}

_{Dim oSMDef As SheetMetalComponentDefinition}

_{oSMDef = oDoc.ComponentDefinition}

_{oSMDef.FlatPattern.ExitEdit}

_{'This code has been adapted from http://www.cadlinecommunity.co.uk/Blogs/Blog.aspx?ScoId=}

_{'4733ef2d-cd48-4bd9-a280-1d88dbbf3556&returnTo=%2fBlogs%2fclintonbrown%2fDefault.aspx}

_{'&returnTitle=Clinton+Brown%20Blog}

_{End Sub}

Any time you want to run the rule again, right click on it and select Run Rule