9 Replies Latest reply on Dec 16, 2015 4:38 AM by Amen Allah Jlili

    Traverse multiple drawing sheets and create views of different parts

    A. T
    A. T Dec 14, 2015 7:05 AM

      Hello, I was wondering if anyone could help me with this. I have an assembly that comprises of 12 parts. I am trying to build a macro that would create 12 sheets in one drawing and then create a standard 3 view of each part, in the corresponding sheet. So far I have managed to create the sheets with a simple loop and then traverse each sheet. What I cannot understand is how to get the name of each part in order to create the views. The 12 sheets are named Part1, Part2,..., Part12. The parts though, don't follow the same name pattern.

       

      Dim swapp As SldWorks.SldWorks

      Dim swmodel As SldWorks.ModelDoc2

      Dim swDraw As SldWorks.DrawingDoc

      Dim TemplateName As String

       

      Sub main()

      Set swapp = Application.SldWorks

      Set swmodel = swapp.ActiveDoc

      TemplateName = "C:\Templates\Drawing.DRWDOT"

      Set swDraw = swapp.NewDocument(TemplateName, swDwgPaperA3size, 0, 0)

      Dim retval As Boolean

       

      ' Loop for creating multiple Sheets

      Dim i As Integer

      Dim SheetName As Variant

      'Dim PartName As Variant

      'PartName = "C:\MyParts\Upper_Link.SLDPRT"  ' Example name of a part

       

      For i = 1 To 12

      SheetName = "Part" & i

      swDraw.NewSheet3 SheetName, swDwgPaperA3size, swDwgTemplateA3size, 1, 5, False, "", 0, 0, ""

      Next i

       

      For i = 1 To 12

      swDraw.ActivateSheet ("Part" & i)

      'retval = swDraw.Create3rdAngleViews2(PartName)   ' Creates views of the same part to all 12 sheets

      Next i

       

      End Sub

        • Re: Traverse multiple drawing sheets and create views of different parts
          Amen Allah Jlili
          Amen Allah Jlili Dec 14, 2015 9:33 AM (in response to A. T)

          Wayyyyyyyyyyyyyy before you add the sheets:

           

          - Using SldWorks.OpenDoc method, open the assembly inside a ModelDoc2

          - Define an AssemblyDoc object inside which you cast the ModelDoc2 object
          - Use the method AssemblyDoc.GetComponents to get a variant of component2.
          - Define a collection object and call it (for example) ComponentsFilePaths

          - Traverse the component2 variant and use the collection:add method to add component2.GetPathName (Now you have a collection of file paths!)

          - Close the ModelDoc2 of the assembly using ModelDoc2.Close
          - Remove duplicates
          Back to the drawing doc now:

          - Traverse the ComponentsFilePaths collection, add new sheet then use swDraw.Create3rdAngleViews2(Collection(i))  to insert the views
          Help pointers:

           

          - When you hear traversing, often times, people are refering to for each loops.
          Example: Traversing a component2 variant called Components

           

          Dim Obj 
For Each Obj In Components
Dim Comp As Component2
Set Comp = Obj
'Doc stuff here
Next Obj

           

          - When you're inserting sheets, you might want to use the filename as the sheet's name.
          If the filename is not meaningful, consider creating a class with two fields: name and filepath. You add whatever customproperty from the component2 as the name and the file path as seen before. After that you add the class objects to the collection. If you choose to use the filename. Use the split function to get the filename from the path.

           

          Dim FilePath As String
FilePath = "C:\File.Exension"
Dim FileName As String
FileName = Split(Split(FilePath,"\")[Ubound(Split(FilePath,"\"))],".")[0]

           

           

          Cheers

            • Re: Traverse multiple drawing sheets and create views of different parts
              A. T
              A. T Dec 15, 2015 6:13 AM (in response to Amen Allah Jlili)

              Thank you very much for your reply. I tried out as you suggested and I think I have managed to get what I want, almost. So I would like to ask how to eliminate duplicates, as the macro creates drawing views for each component and finally how do I disable the creation of views for the subassemblies?

                • Re: Traverse multiple drawing sheets and create views of different parts
                  Amen Allah Jlili
                  Amen Allah Jlili Dec 16, 2015 4:41 AM (in response to A. T)

                  You're doing the right way! You're almost there!


                  Instead of removing duplicates, prevent duplicates from being added simply by checking if file path already exist in the collection before adding?

                   

                  Dim Exist as Boolean 
For i = 0 To ComponentsFilePath.Count
If ComponentsFilePath(i) = swComp.GetPathName Then
Exist = True
Exit For
End If
Next i
If Exist = False Then
ComponentsFilePaths.Add(swComp.GetPathName)
End If

                   

                  I've written this off the top of my head. So you can improve it.

                   

                  Instead of traversing the vcomp for the sheet creation, traverse the filepath collection (because vcomp might have duplicates eg: one part figuring in different sub-assemblies)

                    • Re: Traverse multiple drawing sheets and create views of different parts
                      A. T
                      A. T Dec 15, 2015 7:30 AM (in response to Amen Allah Jlili)

                      Great, I'll give it a try. And something else, if you have time, do you have any idea how to prevent sheets memorandum from getting named with the same name? For example one component is named "4_Upper_Link", all the sheets (in the field DWG No) are named like this. Would be better if each sheet's DWG No field is named after the name of the component.

                        • Re: Traverse multiple drawing sheets and create views of different parts
                          Amen Allah Jlili
                          Amen Allah Jlili Dec 15, 2015 8:01 AM (in response to A. T)

                          If I understood correctly. You need to edit the annotation inside the sheet template title block and link it to the model doc built in name property.
                          Hope this illustration is useful (The language is french is that interests you ):
                          preview.png

                           

                          Kindly post your full working code so the community can benefit from it.

                            • Re: Traverse multiple drawing sheets and create views of different parts
                              A. T
                              A. T Dec 15, 2015 1:38 PM (in response to Amen Allah Jlili)

                              You are right, I deleted the code prior to editing my last comment, as it was not fully functional.

                               

                              Dim swApp As SldWorks.SldWorks

                              Dim swModel As SldWorks.ModelDoc2

                              Dim swAssy As SldWorks.AssemblyDoc

                              Dim swDraw As SldWorks.DrawingDoc

                              Dim swComp As SldWorks.Component2

                              Dim PathCollection As collection

                              Dim vComps As Variant

                              Dim SheetName As Variant

                              Dim AssyName As String

                              Dim TemplateName As String

                              Dim i As Integer

                              Dim retval As Boolean

                              Dim errors As Long

                              Dim warnings As Long

                                

                              Sub main()

                                  Set swApp = Application.SldWorks

                                  Set swModel = swApp.ActiveDoc

                                  Set swAssy = swModel

                                  Set PathCollection = New collection

                                

                              AssyName = "C:\MyAssemblies\Test_Assembly.SLDASM"

                              Set swAssy = swApp.OpenDoc6(AssyName, swDocASSEMBLY, 0, "", errors, warnings)

                                   

                              TemplateName = "C:\MyTemplates\Drawing.DRWDOT"

                              Set swDraw = swApp.NewDocument(TemplateName, swDwgPaperA3size, 0, 0)

                               

                              vComps = swAssy.GetComponents(False)

                               

                                  For i = 1 To UBound(vComps)

                                      Set swComp = vComps(i)

                                      PathCollection.Add swComp.GetPathName

                                  Next i

                               

                                   For i = 1 To PathCollection.Count

                                   SheetName = "Part" & i

                              retval = swDraw.NewSheet3(SheetName, swDwgPaperA3size, swDwgTemplateA3size, 1, 2, False, "", 0, 0, "")

                              retval = swDraw.Create3rdAngleViews2(PathCollection(i))

                                  Next i

                               

                              End Sub

                          • Re: Traverse multiple drawing sheets and create views of different parts
                            A. T
                            A. T Dec 16, 2015 4:18 AM (in response to Amen Allah Jlili)

                            I have read that when using a collection it will store only unique values. If this is true then there is no need for extra code to prevent the duplicates from adding to the collection, but I am not sure how to properly use the collection for this purpose. I would appreciate any idea. Also I haven't figured out how to prevent the duplicates with if statements as you proposed.

                              • Re: Traverse multiple drawing sheets and create views of different parts
                                Amen Allah Jlili
                                Amen Allah Jlili Dec 16, 2015 4:38 AM (in response to A. T)

                                That's not precisely true. Collections store a (key,value) pair where the value can be the same across the collections, the key need to be unique. When you don't specify the key, VBA will take care of it. This screenshot of this test sub will illustrate my point.

                                preview.png

                                 

                                1. Dim Exist as Boolean  'Default value is false
                                2. ' Look if swComp.GetPathName exist in the collection
                                3. For i = 0 To ComponentsFilePath.Count - 1
                                4. If ComponentsFilePath(i) = swComp.GetPathName Then 
                                5. ' Set Exist to true since the file path exists and break off the for loop
                                  Exist = True
                                6. Exit For 
                                7. End If 
                                8. Next i 
                                10. If Exist = False Then 'This mean that the swComp.GetPathName does not exist in the collection 
                                11. ComponentsFilePaths.Add(swComp.GetPathName) 
                                12. End If
                            • Re: Traverse multiple drawing sheets and create views of different parts
                              Amen Allah Jlili
                              Amen Allah Jlili Dec 15, 2015 7:40 AM (in response to A. T)

                              To prevent the creation of subassemblies sheets, simply check if the extension in the filepathname is not that of an assembly before adding it to the collection. Use the split function to split the pathname into an array with "." being the separator. The utmost element of the array is the extension which should not be ASM or SLDASM.


                              Another cooler option (but consumes memory and time) is to use Component2.GetModelDoc and cast into a ModelDoc2 and use GetType to get the type of the model.


                              GetType returns an integer represents the type of the model doc with 1 representing part documents.