Batch Assembly Export

Not enough time today for a proper post just a quick one. I have been working on a vb-ilogic code to identify and resolve all references. On the same process I hope to get a code for renaming the files as well.

This will of course be free and available for everybody to download from this blog but you need to stick around and check my progress because I don’t have a time frame of when that will be available.

Replacing references is working but we get into errors and limitations for special files like skeletons in Frame Generator, Tube and Pipe Route and Runs, welded assemblies, documents marked as Reference in BOM, etc. It’s a slow progress and I can’t allocate it as much time as I would like at the moment.

On a side note, there is a NDA (Non Disclosure Agreement) between me and Autodesk so I can’t say much but I was assured that the T&P list is very important for them.

Enough said on that and for today I will share a bit of code that hopefully will get your productivity up and get those manual tasks to minimum. The code needs to be run from inside an assembly and will save all parts in STEP format in a folder right next to the main assembly. I have done this code for a friend and while he is still testing you can have a preview of it (hurry up Karol).

The SaveAs option in the code can be used with any formats listed in the Save Copy As dialog but you might want to investigate the results and use the ApplicationAddIns and HasSaveCopyAsOption which will give you more control over what gets exported and some of the options in the save as dialog.

The Save As dialog can be bypassed and process the assembly as a batch

If, for example, you need to export the current drawing to PDF you can’t (shouldn’t) use the SaveAs code because it will only export the first sheet and you can’t control, colors, resolution, line weights, printing sheet range, etc. There’s more info in my previous post here.

Here’s the code, enjoy:

 'define the active document as an assembly file

Dim oAsmDoc As AssemblyDocument

oAsmDoc = ThisApplication.ActiveDocument

oAsmName = ThisDoc.FileName(False) 'without extension

If ThisApplication.ActiveDocument.DocumentType <> kAssemblyDocumentObject Then

    MessageBox.Show("Please run this rule from the assembly file.", "iLogic")

    Exit Sub

End If

'get user input

RUsure = MessageBox.Show ( _

"This will create a STEP file for all components." _

& vbLf & " " _

& vbLf & "Are you sure you want to create STEP Drawings for all of the assembly components?" _

& vbLf & "This could take a while.", "iLogic - Batch Output STEPs ",MessageBoxButtons.YesNo)

If RUsure = vbNo Then

    Return

Else

End If

'- - - - - - - - - - - - -STEP setup - - - - - - - - - - - -

oPath = ThisDoc.Path

'get STEP target folder path

oFolder = oPath & "\" & oAsmName & " STEP Files"

'Check for the step folder and create it if it does not exist

If Not System.IO.Directory.Exists(oFolder) Then

System.IO.Directory.CreateDirectory(oFolder)

End If

'- - - - - - - - - - - - -Assembly - - - - - - - - - - - -

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".stp") , True)

'- - - - - - - - - - - - -Components - - - - - - - - - - - -

'look at the files referenced by the assembly

Dim oRefDocs As DocumentsEnumerator

oRefDocs = oAsmDoc.AllReferencedDocuments

Dim oRefDoc As Document

'work the referenced models

For Each oRefDoc In oRefDocs

    Dim oCurFile As Document

    oCurFile = ThisApplication.Documents.Open(oRefDoc.FullFileName, True)

    oCurFileName = oCurFile.FullFileName

   

    'defines backslash As the subdirectory separator

    Dim strCharSep As String = System.IO.Path.DirectorySeparatorChar

   

    'find the postion of the last backslash in the path

    FNamePos = InStrRev(oCurFileName, "\", -1)  

    'get the file name with the file extension

    Name = Right(oCurFileName, Len(oCurFileName) - FNamePos)

    'get the file name (without extension)

    ShortName = Left(Name, Len(Name) - 4)

    Try

        oCurFile.SaveAs(oFolder & "\" & ShortName & (".stp") , True)

    Catch

        MessageBox.Show("Error processing " & oCurFileName, "ilogic")

    End Try

    oCurFile.Close

Next

'- - - - - - - - - - - - -

MessageBox.Show("New Files Created in: " & vbLf & oFolder, "iLogic")

'open the folder where the new files are saved

Shell("explorer.exe " & oFolder,vbNormalFocus)

I have tested it and save the assembly in all these other formats, including Inventor iam:

Results of exporting the assembly.

'- - - - - - - - - - - - -Assembly - - - - - - - - - - - - 

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".iam") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".dwg") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".bmp") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".CATProduct") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".dwf") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".dwfx") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".gif") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".igs") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".ige") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".iges") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".jpg") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".jt") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".pdf") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".png") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".x_b") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".x_t") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".g") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".neu") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".sat") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".stp") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".ste") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".step") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".stl") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".tiff") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".xgl") , True)

ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName &(".zgl") , True)

Later,
ADS

Edit 16-04-14

this is the code to append revision number at the end of the files:

Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisApplication.ActiveDocument
oAsmName = ThisDoc.FileName(False) 'without extension

If ThisApplication.ActiveDocument.DocumentType <> kAssemblyDocumentObject Then
    MessageBox.Show("Please run this rule from the assembly file.", "iLogic")
    Exit Sub
End If
'get user input
RUsure = MessageBox.Show ( _
"This will create a STEP file for all components." _
& vbLf & " " _
& vbLf & "Are you sure you want to create STEP Drawings for all of the assembly components?" _
& vbLf & "This could take a while.", "iLogic - Batch Output STEPs ",MessageBoxButtons.YesNo)
If RUsure = vbNo Then
    Return
Else
End If
'- - - - - - - - - - - - -STEP setup - - - - - - - - - - - -
oPath = ThisDoc.Path
'get STEP target folder path
oFolder = oPath & "\" & oAsmName & " STEP Files"

'get the document revision to use in the new filename
oRevNumAsm = iProperties.Value("Project", "Revision Number")

'Check for the step folder and create it if it does not exist
If Not System.IO.Directory.Exists(oFolder) Then
System.IO.Directory.CreateDirectory(oFolder)
End If


'- - - - - - - - - - - - -Assembly - - - - - - - - - - - -
ThisDoc.Document.SaveAs(oFolder & "\" & oAsmName & "_Rev" & oRevNumAsm &(".stp") , True)

'- - - - - - - - - - - - -Components - - - - - - - - - - - -
'look at the files referenced by the assembly
Dim oRefDocs As DocumentsEnumerator
oRefDocs = oAsmDoc.AllReferencedDocuments
Dim oRefDoc As Document
'work the referenced models
For Each oRefDoc In oRefDocs
    Dim oCurFile As Document
    oCurFile = ThisApplication.Documents.Open(oRefDoc.FullFileName, True)
    oCurFileName = oCurFile.FullFileName

   
    'defines backslash As the subdirectory separator
    Dim strCharSep As String = System.IO.Path.DirectorySeparatorChar
   
    'find the postion of the last backslash in the path
    FNamePos = InStrRev(oCurFileName, "\", -1)  
    'get the file name with the file extension
    Name = Right(oCurFileName, Len(oCurFileName) - FNamePos)
    'get the file name (without extension)
    ShortName = Left(Name, Len(Name) - 4)
    oRevDoc = iProperties.Value(Name, "Project", "Revision Number")


    Try
        oCurFile.SaveAs(oFolder & "\" & ShortName & "_Rev" & oRevDoc & (".stp") , True)
    Catch
        MessageBox.Show("Error processing " & oCurFileName, "ilogic")
    End Try
    oCurFile.Close
Next
'- - - - - - - - - - - - -
MessageBox.Show("New Files Created in: " & vbLf & oFolder, "iLogic")
'open the folder where the new files are saved
Shell("explorer.exe " & oFolder,vbNormalFocus)

Custom Table on Drawing

No time for a regular post or a video but I’ve got a small ilogic code to share on how to create and edit custom tables on drawings.

I am doing half a dozen tanks a week and each need to have a couple of tables with nozzle connection and tank specifications.

The tank is done as ilogic component that I clone along with the drawing each time a new one is needed.

The nozzle connection table looks like this:

And the Operating Conditions table:

                All the info comes from the model and if they are not present then we prompt the user for the values to fill in.

                It is better if you place and position the table before running the code otherwise it will show up somewhere in the lower left corner, (you can always move it of course). If you do place the table first even if it doesn't have the correct info the code will find it and will edit it.

                I am using table name as my search criteria when going through all the custom tables on the drawing.  The limitation would be having two custom tables with same name because it stops at the first one so, although obvious, make sure you have different names for each of your table; can’t call them all “table”.

        TableCheck:

'------------------------------------------------------

'---------------start finding the table----------------

'------------------------------------------------------

For i = 1 To oSheet.CustomTables.Count

    TableTitle = oSheet.CustomTables.Item(i).Title                       

    If TableTitle = "Operating Conditions" Then

        'Remember the table number for editing section

        TableNr = i

        'If table found jump to edit section

        Goto EditTable

    End If

Next

'------------------------------------------------------

'---------------end finding the table----------------

'------------------------------------------------------

               

If the table is not found then we are creating it and then we run the TableCheck again in order to find the table number to edit.

'CreateTable:

'------------------------------------------------------

'---------------start creating the table---------------

'------------------------------------------------------

' Set the column titles

oTitles = New String(){"Item", "Description"}

'

'

'

' Create the custom table

oCustomTable = oSheet.CustomTables.Add("Operating Conditions", ThisApplication.TransientGeometry.CreatePoint2d(15, 15), _

                                    2, 11, oTitles,oContents, oColumnWidths)

'------------------------------------------------------

'---------------finish creating the table---------------

'------------------------------------------------------

'edit the table by restarting the check routine

Goto TableCheck

       

This is where we edit the table, and we check if the model has the info we need and if not then we prompt the user for that. When we prompt we show the user the current value but allow him to change it if he wants:

EditTable:

'------------------------------------------------------

'---------------start editing the table---------------

'------------------------------------------------------

'Get the name Of the first model in the drawing

modelName = IO.Path.GetFileName(ThisDrawing.ModelDocument.FullFileName)

'MessageBox.Show(modelName, "ilogic")

'

'

'

'

'------------------------------------------------------

'---------------finish editing the table---------------

'------------------------------------------------------

It’s pretty much the same for the Tank Connection Details so I won’t post that but the code for this one is down bellow for all those search engines and linked here for you to download.

Later,

ADS.

' Set a reference to the drawing document.

' This assumes a drawing document is active.

Dim oDrawDoc As DrawingDocument

oDrawDoc = ThisApplication.ActiveDocument

' Set a reference to the active sheet.

Dim oSheet As Sheet

oSheet = oDrawDoc.ActiveSheet

'Declare my custom table

Dim oCustomTable As CustomTable

TableCheck:

'------------------------------------------------------

'---------------start finding the table----------------

'------------------------------------------------------

For i = 1 To oSheet.CustomTables.Count

    TableTitle = oSheet.CustomTables.Item(i).Title                       

    If TableTitle = "Operating Conditions" Then

        TableNr = i

        'If table found jumpt to edit section

        Goto EditTable

    End If

Next

'if not found go create it

Goto CreateTable

'------------------------------------------------------

'---------------end finding the table----------------

'------------------------------------------------------

CreateTable:

'------------------------------------------------------

'---------------start creating the table---------------

'------------------------------------------------------

' Set the column titles

oTitles = New String(){"Item", "Description"}

' You can ask user for the name of the columns if you want

'Dim oTitles(1 To 2) As String

'oTitles(1) = "Item"

'oTitles(2) = InputBox("What to prompt", "iLogic", "Default value")

' Set the contents of the custom table (contents are set row-wise)

'more than one way to skin a cat

'Dim oContents(1 To 22) As String

oContents = New String(0 To 21){}

oContents(0) = "Contents"

oContents(1) = "" 'oMedia

oContents(2) = "Working Capacity (EST)"

oContents(3) = "" 'oCapEST

oContents(4) = "Dry Weight"

oContents(5) = "" 'oDryWgt

oContents(6) = "Maximum Working Weight"

oContents(7) = "" 'oMaxWgt

oContents(8) = "Specific Gravity"

oContents(9) = "" 'oSpecGrav

oContents(10) = "Max. Working Temperature"

oContents(11) = "5 Degrees C"

oContents(12) = "Max.Working Pressure"

oContents(13) = "Atmospheric"

oContents(14) = "Materials of Construction"

oContents(15) = "" 'oMaterial

oContents(16) = "Location"

oContents(17) = "Plantroom"

oContents(18) = "Tolerances"

oContents(19) = ""

oContents(20) = "Angular"

oContents(21) = "+/- 0.5 Degrees"

' Set the column widths (defaults to the column title width if not specified)

Dim oColumnWidths(0 To 1) As Double

oColumnWidths(0) = 7.5

oColumnWidths(1) = 6

 

' Create the custom table

oCustomTable = oSheet.CustomTables.Add("Operating Conditions ADS", ThisApplication.TransientGeometry.CreatePoint2d(15, 15), _

                                    2, 11, oTitles,oContents, oColumnWidths)

'------------------------------------------------------

'---------------finish creating the table---------------

'------------------------------------------------------

'edit the table by restarting the check routine

Goto TableCheck

EditTable:

'------------------------------------------------------

'---------------start editing the table---------------

'------------------------------------------------------

'Get the name Of the first model in the drawing

modelName = IO.Path.GetFileName(ThisDrawing.ModelDocument.FullFileName)

'MessageBox.Show(modelName, "ilogic")

   

'declare the table to edit by the number found in check

oCustomTable = oSheet.CustomTables.Item(TableNr)

'Type of Media

Dim oMedia As String

'set the cell to edit, you can add numbers or name

'first cell to edit

oCell1= oCustomTable.Rows.Item(1).Item("Description")

'try and get it from the model

Try

    oMedia = Parameter(modelName, "MediaType")

'if not found, prompt user for it

Catch

    oMedia = InputBox("Contents", "iLogic", oCell1.Value)

End Try

'add media to table

oCell1.Value = oMedia

'Capacity

Dim oCapEst As String

'second cell we're editing

oCell2= oCustomTable.Rows.Item(2).Item("Description")

'try and get it from the model

Try

    oCapEst = Parameter(modelName, "CapEst") & " Litres"

'if not found, prompt user for it

Catch

    oCapEST = InputBox("Working Capcity (EST)", "iLogic", oCell2.Value)

End Try

'add Capacity to table

oCell2.Value = oCapEST

'Dry Weight

Dim oDryWgt As String

'3rd cell we're editing

oCell3 = oCustomTable.Rows.Item(3).Item("Description")

'try and get it from the model

Try

    oDryWgt = Parameter(modelName, "DryWgt") & " Kg"

'if not found, prompt user for it

Catch

    oDryWgt = InputBox("Dry Weight", "iLogic", oCell3.Value)

End Try

'add Weight to table

oCell3.Value = oDryWgt

'Total Weight

Dim oMaxWgt As String

'4th cell we're editing

oCell4= oCustomTable.Rows.Item(4).Item("Description")

'try and get it from the model

Try

    oMaxWgt = Parameter(modelName, "MaxWgt") & " Kg"

'if not found, prompt user for it

Catch

    oMaxWgt = InputBox("Max Working Weight", "iLogic", oCell4.Value)

End Try

'add total weight to table

oCell4.Value = oMaxWgt

'Specific Gravity of Media

Dim oSpecGrav As String

'5th cell to edit

oCell5= oCustomTable.Rows.Item(5).Item("Description")

'try and get it from the model

Try

    oSpecGrav = Parameter(modelName, "SpecGrav")

'if not found, prompt user for it

Catch

    oSpecGrav = InputBox("Specific Gravity", "iLogic", oCell5.Value)

End Try

'add Specific Gravity to table

oCell5.Value = oSpecGrav

'Material

Dim oMaterial As String

'6th cell to edit

oCell6= oCustomTable.Rows.Item(8).Item("Description")

'try and get it from the model

Try

    oMaterial = Parameter(modelName, "MaterialType")

'if not found, prompt user for it

Catch

    oMaterial = InputBox("Material", "iLogic", oCell6.Value)

End Try

'add material to table

oCell6.Value = oMaterial

'------------------------------------------------------

'---------------finish editing the table---------------

'------------------------------------------------------

EndRule: