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