Mod the Machine

Migrating your SolidWorks Applications to Inventor

I asked a question in a recent post to see if any of you were interested in a series of posts discussing how to migrate your SolidWorks programs to work with Inventor.  Well, there was some interest in the topic.  Rather than break the information up into a series of posts, here’s a document produced by the Autodesk Developer Network (ADN) team that describes some of the differences in the programming interfaces and some hints and tips to help you with the migration.

Migrating SolidWorks Applications to Autodesk Inventor

This is the initial release of the document so it will likely go through some updates.  Any comments that will help to improve it are welcome.

Totaling the Length of Parts in an Assembly

There’s a question on the Inventor Customization newsgroup that I thought might be of general interest so I’m posting my response here.  The specific question is that they have a cabinet assembly and some of the parts in the assembly represent pieces of molding.  They want to get a total length of all of the molding used in the assembly.  I’ve written a small sample below that illustrates one approach to this.

The first thing before writing any program is to fully understand the conditions the program can expect.  You might need to impose certain requirements on the model in order for the program to function correctly.  A computer program isn’t very smart and only does exactly what you’ve programmed it to do.  Each variation in the conditions of the model requires more code to check for and handle each case.  Here are the assumptions that this program makes about the assembly. 

1. The program is executed when the cabinet assembly is active.
2. Any parts that represent molding will have the word “molding” in the category iProperty.  This is how the program determines which parts are molding parts.
3. Each molding part has a parameter called “Length” that is the actual length of the molding part.

The program demonstrates several basic things that should be interesting for many of you.  First, it traverses the entire assembly looking for molding parts.  It uses the iProperty portion of the API and rule number 2 above to determine which parts in the assembly are molding parts.  Once it finds a molding part it uses the parameters portion of the API to get the length of the molding.  It again uses iProperties to create or update a custom iProperty in the assembly with the total length of the molding (plus 30% for waste).

Not everyone needs a program that totals the length of molding parts but hopefully you can see how this sample could be easily edited to perform other similar tasks.

Something to be aware of is that this is not automatic.  It’s essentially a “snapshot” of the length of molding at the time you run the program.  If you edit, add, or remove parts the iProperty will not automatically update but you’ll need to manually run the program again.

If you’re new to Inventor’s VBA, here’s a post that lists the steps of how to use a VBA macro within Inventor.

' Main program that computes the total length of all molding
' parts in the active assembly.
Public Sub ComputeMoldingLength() 
   Dim asmDoc As AssemblyDocument 
   Set asmDoc = ThisApplication.ActiveDocument 
   Dim asmDef As AssemblyComponentDefinition 
   Set asmDef = asmDoc.ComponentDefinition
 
   ' Call the recursive function to traverse the assembly. 
   Dim MoldingLength As Double 
   MoldingLength = 0 
   Call GetMoldingLength(asmDef.Occurrences, MoldingLength) 

   ' Get the iProperties for this document. 
   Dim propSets As PropertySets 
   Set propSets = asmDoc.PropertySets 

   ' Get the user defined property set. 
   Dim userProps As PropertySet 
   Set userProps = propSets.Item("Inventor User Defined Properties") 

   ' Create a string that represents the length value, 
   ' including an extra 30% for waste. 
   Dim totalLength As String 
   totalLength = asmDoc.UnitsOfMeasure.GetStringFromValue( _
                 MoldingLength * 1.3, kDefaultDisplayLengthUnits) 

   ' Update or create the iProperty containing the length. 
   On Error Resume Next 
   Dim lengthProp As Inventor.Property 
   Set lengthProp = userProps.Item("MoldingLength") 
   If Err.Number <> 0 Then 
      ' The property doesn't exist so create it. 
      Set lengthProp = userProps.Add(totalLength, "MoldingLength") 
   Else 
      lengthProp.value = totalLength 
   End If 

   MsgBox "Total molding length (including 30% waste): " _
          & totalLength
End Sub

' Sub that is called recursively to iterate through the entire
' assembly structure to find and total the lengths of all
' molding parts.
Private Sub GetMoldingLength( _
                      ByVal Occurrences As ComponentOccurrences, _
                      ByRef MoldingLength As Double) 
   ' Iterate through the occurrences in the current assembly. 
   Dim occ As ComponentOccurrence 
   For Each occ In Occurrences 
      ' Check if this is a part or assembly. 
      If occ.DefinitionDocumentType = kPartDocumentObject Then 
         ' Get the iProperties for this document. 
         Dim propSets As PropertySets 
         Set propSets = occ.Definition.Document.PropertySets 

         ' Get the Document Summary Info property set. 
         Dim docSummaryInfo As PropertySet 
         Set docSummaryInfo = propSets.Item( _
                            "Inventor Document Summary Information") 

         ' Check to see if the term "molding" is part of 
         ' the category property. 
         If InStr("MOLDING", _
           UCase(docSummaryInfo.Item("Category").value)) > 0 Then 
             ' Get the user defined property set. 
             Dim userDefinedProps As PropertySet 
             Set userDefinedProps = propSets.Item( _
                                 "Inventor User Defined Properties")
 
             ' Get the component definition of the part. 
             Dim partCompDef As PartComponentDefinition 
             Set partCompDef = occ.Definition 

             ' Get the parameter for the length.  
             ' It will be in centimeters. 
             On Error Resume Next 
             Dim length As Double 
             length = partCompDef.Parameters.Item("Length").value 
             If Err.Number = 0 Then 
                MoldingLength = MoldingLength + length 
             Else 
                MsgBox "Error getting the Length property from " & _
                        occ.Definition.Document.DisplayName 
             End If 
             On Error GoTo 0 
         End If 
      Else 
         ' It's an assembly so call this sub again. 
         Call GetMoldingLength(occ.SubOccurrences, MoldingLength) 
      End If 
   Next
End Sub

Balloon Reporting Macro

There was a question on the Autodesk Inventor Customization newsgroup this morning that caught my interest.  The question was about creating a report, (in their case editing a column in the BOM), that lists all of the balloons in a drawing along with what sheet they’re on and the zone on the sheet they’re located within,

The macro below does this.  The output is simple since it just writes out the result as a file, but you’ll likely want to edit the program to do something else with the result like incorporate it into the BOM, create a custom table, or some other thing I would never have thought of.  The macro assumes that the border was created as a default border.  With a default border it’s a simple matter to get the number of zones on a sheet and determine whether to use numbers or characters for the zone labels.  If you’re using a border you’ve created then you’ll need to edit the program and specify this information.

I tested the macro using the Engine MKII sample assembly shown below.  The drawing that comes with that sample has three sheets and balloons on two of the sheets.

Here are the contents of the report created by the macro.

==== Balloon Report ====
  Sheet: Sheet:1
    Balloon: 8, (7, B)
    Balloon: 7, (1, A)
    Balloon: 11, (7, B)
    Balloon: 12, (7, B)
    Balloon: 23, (7, A)
    Balloon: 19, (7, A)
    Balloon: 28, (7, A)
    Balloon: 26, (7, A)
    Balloon: 18, (8, A)
    Balloon: 20, (8, A)
    Balloon: 110, (3, B)
    Balloon: 81, (3, A)
    Balloon: 112, (4, A)
  Sheet: Sheet:2
    Balloon: 18, (2, B)
    Balloon: 19, (3, A)
    Balloon: 9, (5, C)
    Balloon: 1, (5, D)
    Balloon: 3, (5, D)
    Balloon: 8, (5, C)
    Balloon: 5, (5, D)
    Balloon: 7, (5, C)
    Balloon: 6, (5, C)
    Balloon: 4, (5, D)
    Balloon: 31, (5, B)
    Balloon: 29, (2, B)
    Balloon: 30, (2, B)
    Balloon: 28, (2, B)
    Balloon: 24, (2, B)
    Balloon: 27, (2, B)
    Balloon: 25, (2, B)
    Balloon: 26, (2, B)
    Balloon: 12, (5, B)
    Balloon: 11, (5, B)
    Balloon: 10, (5, B)
    Balloon: 16, (2, C)
    Balloon: 18, (3, D)
    Balloon: 17, (3, D)
    Balloon: 14, (2, C)
    Balloon: 13, (2, C)
    Balloon: 9, (2, C)
    Balloon: 15, (3, D)
    Balloon: 20, (3, A)
    Balloon: 23, (2, A)
    Balloon: 22, (3, A)
    Balloon: 21, (3, A)
  Sheet: Sheet:3

Here’s the VBA macro.  To use it, just copy and paste the code below into a VBA code module, have a drawing open, and run it.  If you’re not familiar with VBA, instructions to do this are available here.

Public Sub BalloonReport() 
  ' Get the active drawing document. 
  Dim drawDoc As DrawingDocument 
  Set drawDoc = ThisApplication.ActiveDocument 

  ' Open a file to write the results into. 
  Dim filename As String 
  filename = "C:\Temp\BalloonReport.txt" 
  Open filename For Output As #1 

  ' Print out the header for the report, both to the 
  ' output file and the immediate window in VBA. 
  Debug.Print "" 
  Debug.Print "==== Balloon Report ====" 
  Print #1, "==== Balloon Report ====" 

  ' Iterate through the sheets. 
  Dim drawSheet As sheet 
  For Each drawSheet In drawDoc.Sheets 
    ' Print out the sheet name. 
    Debug.Print "  Sheet: " & drawSheet.Name 
    Print #1, "  Sheet: " & drawSheet.Name 

    ' Determine the zones within this sheet.  This assumes that
    ' the border was created as a standard border where the
    ' zones are explicitly defined.  If this is a custom border
    ' then some other mechanism will need to be created to 
    ' define the zones. 
    Dim border As DefaultBorder 
    Set border = drawSheet.border 
    Dim XZoneWidth As Double 
    Dim YZoneWidth As Double 
    XZoneWidth = drawSheet.Width / border.HorizontalZoneCount 
    YZoneWidth = drawSheet.Height / border.VerticalZoneCount 
    Dim XZoneIsNumber As Boolean 
    If border.HorizontalZoneLabelMode = kBorderLabelModeNumeric Then 
        XZoneIsNumber = True 
    Else 
        XZoneIsNumber = False 
    End If 

    Dim YZoneIsNumber As Boolean 
    If border.VerticalZoneLabelMode = kBorderLabelModeNumeric Then 
      YZoneIsNumber = True 
    Else 
      YZoneIsNumber = False 
    End If 

    ' Iterate through the balloons on this sheet. 
    Dim drawBalloon As Balloon 
    For Each drawBalloon In drawSheet.Balloons 
      ' Because the border is numbered in the X direction from 
      ' right to left and the sheet coordinate system is from 
      ' left to right, this reverses the X coordinate so the 
      ' zone computation will be correct. 
      Dim newXPosition As Double 
      newXPosition = drawSheet.Width - drawBalloon.position.X 

      ' Determine the X zone. 
      Dim XZone As Integer 
      XZone = Int(newXPosition / XZoneWidth) 

      ' Get the X zone as a string. 
      Dim XZoneValue As String 

      If XZoneIsNumber Then 
        XZoneValue = XZone + 1 
      Else 
        XZoneValue = Chr(XZone + 65) 
      End If 

      ' Determine Y zone. 
      Dim YZone As Integer 
      YZone = Int(drawBalloon.position.Y / YZoneWidth) 

      ' Get the Y zone as a string. 
      Dim YZoneValue As String 
      If YZoneIsNumber Then 
        YZoneValue = YZone + 1 
      Else 
        YZoneValue = Chr(YZone + 65) 
      End If 

      ' Iterate through each value set associated with this balloon. 
      Dim valueSet As BalloonValueSet 
      For Each valueSet In drawBalloon.BalloonValueSets 
        ' Print out the results for this value set. 
        Debug.Print "    Balloon: " & valueSet.value & _ 
                    ", (" & XZoneValue & ", " & YZoneValue & ")" 
        Print #1, "    Balloon: " & valueSet.value & _ 
                  ", (" & XZoneValue & ", " & YZoneValue & ")" 
      Next 
    Next 
  Next 

  ' Close the output file. 
  Close #1 

  MsgBox "Report written to: """ & filename & """"
End Sub