AnsweredAssumed Answered

Traverse multiple drawing sheets and create views of different parts

Question asked by A. T. on Dec 14, 2015
Latest reply on Dec 16, 2015 by Amen Allah Jlili

Like • Show 0 Likes0
Comment • 9

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

Amen Allah Jlili Dec 14, 2015 9:33 AM

Correct Answer

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

See the reply in context

No one else had this question

Outcomes

Amen Allah Jlili Dec 14, 2015 9:33 AM

Wayyyyyyyyyyyyyy before you add the sheets:

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

- 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

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

Cheers

Actions

A. T. @ Amen Allah Jlili on Dec 15, 2015 6:13 AM

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?

Actions

Amen Allah Jlili @ A. T. on Dec 16, 2015 4:41 AM

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)

Actions

A. T. @ Amen Allah Jlili on Dec 15, 2015 7:30 AM

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.

Actions

Amen Allah Jlili @ A. T. on Dec 15, 2015 8:01 AM

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 ):

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

Actions

A. T. @ Amen Allah Jlili on Dec 15, 2015 1:38 PM

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

Actions

A. T. @ Amen Allah Jlili on Dec 16, 2015 4:18 AM

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.

Actions

Amen Allah Jlili @ A. T. on Dec 16, 2015 4:38 AM

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.

Dim Exist as Boolean 'Default value is false
' Look if swComp.GetPathName exist in the collection
For i = 0 To ComponentsFilePath.Count - 1
If ComponentsFilePath(i) = swComp.GetPathName Then
' Set Exist to true since the file path exists and break off the for loop
Exist = True
Exit For
End If
Next i
If Exist = False Then 'This mean that the swComp.GetPathName does not exist in the collection
ComponentsFilePaths.Add(swComp.GetPathName)
End If

Actions

Amen Allah Jlili @ A. T. on Dec 15, 2015 7:40 AM

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.

Actions

9 Replies

Amen Allah Jlili Dec 14, 2015 9:33 AM
Unmark Correct
Correct Answer
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
Like • Show 1 Like1
Actions
- A. T. @ Amen Allah Jlili on Dec 15, 2015 6:13 AM
  Mark Correct
  Correct Answer
  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?
  Like • Show 0 Likes0
  Actions
  - Amen Allah Jlili @ A. T. on Dec 16, 2015 4:41 AM
    Mark Correct
    Correct Answer
    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)
    Like • Show 0 Likes0
    Actions
    - A. T. @ Amen Allah Jlili on Dec 15, 2015 7:30 AM
      Mark Correct
      Correct Answer
      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.
      Like • Show 0 Likes0
      Actions
      - Amen Allah Jlili @ A. T. on Dec 15, 2015 8:01 AM
        Mark Correct
        Correct Answer
        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 ):
        
        Kindly post your full working code so the community can benefit from it.
        Like • Show 0 Likes0
        Actions
        A. T. @ Amen Allah Jlili on Dec 15, 2015 1:38 PM
        Mark Correct
        Correct Answer
        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
        Like • Show 0 Likes0
        Actions
    - A. T. @ Amen Allah Jlili on Dec 16, 2015 4:18 AM
      Mark Correct
      Correct Answer
      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.
      Like • Show 0 Likes0
      Actions
      - Amen Allah Jlili @ A. T. on Dec 16, 2015 4:38 AM
        Mark Correct
        Correct Answer
        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.
        
        Dim Exist as Boolean 'Default value is false
        ' Look if swComp.GetPathName exist in the collection
        For i = 0 To ComponentsFilePath.Count - 1
        If ComponentsFilePath(i) = swComp.GetPathName Then
        ' Set Exist to true since the file path exists and break off the for loop
        Exist = True
        Exit For
        End If
        Next i
        If Exist = False Then 'This mean that the swComp.GetPathName does not exist in the collection
        ComponentsFilePaths.Add(swComp.GetPathName)
        End If
        Like • Show 0 Likes0
        Actions
  - Amen Allah Jlili @ A. T. on Dec 15, 2015 7:40 AM
    Mark Correct
    Correct Answer
    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.
    Like • Show 0 Likes0
    Actions

Traverse multiple drawing sheets and create views of different parts

Outcomes

Related Content

Recommended Content