Autodesk Inventor has an Excellent Bill of Materials (BoM) interface which allows user to create and Export BoM’s from the assembly environment.
However, if you have an Assembly model that has a mix of normal and sheet metal components, there is no way to distinguish between the 2 part types in the BoM environment.
I’ve written a little iLogic Utility that exports a sheet metal parts list or BoM, this version is pretty simplistic, in that it just lists off each part, it does not specify a quantity, so if there are 3 of the same part required, they will be listed 3 times, and will be listed in the order in which they appear in the assembly.
The iLogic utility works it’s way through an Assembly file (including sub assemblies) exporting the name as well as some iProperties of every sheet metal part to a text file.
The Animated GIF below shows it in action:
Here’s the iLogic code:
'iLogic code by Clint Brown @ClintBrown3D
'originally posted at https://clintbrown.co.uk/ilogic:-export-sheet-metal-bom
Dim doc = ThisDoc.Document : If doc.DocumentType = kAssemblyDocumentObject Then
Else : Return : End If
'Create Txt BoM
oWrite = IO.File.CreateText(ThisDoc.PathAndFileName(False) & ".txt")
oWrite.WriteLine("-----------------------------------Unofficial Inventor----------------------------------------")
oWrite.WriteLine("Sheet Metal BoM: " & ThisDoc.FileName(True))
oWrite.WriteLine("")
oWrite.Close()
SheetMetalCheckGUID = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" ' This is the Sheet Metal unique identifier
'Iterate through the Assembly to find Sheet Metal parts
Dim oAssyDoc As AssemblyDocument
Dim oCompOccEnum As ComponentOccurrencesEnumerator
Dim oCompOcc As ComponentOccurrence
oAssyDoc = ThisApplication.ActiveDocument
oCompOccEnum = oAssyDoc.ComponentDefinition.Occurrences.AllReferencedOccurrences(oAssyDoc.ComponentDefinition)
For Each oCompOcc In oCompOccEnum
If oCompOcc.Definition.Document.SubType = SheetMetalCheckGUID Then 'Check for Sheet Metal parts
Try
'Set up properties to write to the BoM
o1 = oCompOcc.Name & " : " & iProperties.MaterialOfComponent(oCompOcc.Name)
o2 = " -- Part Number: " & iProperties.Value(oCompOcc.Name, "Project", "Part Number")
o3 = " -- Mass: " & iProperties.MassOfComponent(oCompOcc.Name)
o4 = " -- Material: " & iProperties.MaterialOfComponent(oCompOcc.Name)
o5 = " -- Thickness: " & Parameter(oCompOcc.Name, "Thickness")
oInfo = o1 & o2 & o3 & o4 & o5
Dim oAppend As System.IO.StreamWriter 'Update Txt BoM
oAppend = IO.File.AppendText(ThisDoc.PathAndFileName(False) & ".txt")
oAppend.WriteLine(oInfo)
oAppend.Flush()
oAppend.Close()
Catch
MessageBox.Show("Oh Snap!", "@ClintBrown3D")
End Try
End If
Next
ThisApplication.StatusBarText = "Unoffical Inventor - Sheet Metal BoM Export Successful"
i = MessageBox.Show("Would you like to see the Parts List?", "Unofficial Inventor", MessageBoxButtons.YesNo)
If i = vbYes Then : GoTo ClintBrown1 : Else : GoTo ClintBrown2 : End If
ClintBrown1 : ThisDoc.Launch(ThisDoc.PathAndFileName(False) & ".txt")
ClintBrown2 : Return
