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How to select Cutlist Item and create a 3D Bounding Box

Question asked by Raymond Yau on Mar 6, 2017
Latest reply on Mar 9, 2017 by Deepak Gupta

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Hi All,

I've been programming a macro that would select the first feature in my Cut-list folder and then create a 3D Bounding Box for the selected item.

From what I've gathered from online resources, here is my (maybe 100th) attempt at the macro.

I'm struggling with the cut-list-item selection part. Some sources I viewed online demonstrates how to select Solid Bodies, but not cut-list item IDs. Perhaps I'm over complicating things?

Help much appreciated.

Sources used:

2016 SOLIDWORKS API Help - Create 3D Bounding Box for Cut List Item Example (VBA)

2015 SOLIDWORKS API Help - Get Names of Bodies in Multibody Part Example (VBA)

2016 SOLIDWORKS API Help - Get Weldment Cut List Feature and Annotations Example (VB.NET)

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim modDocExt As SldWorks.ModelDocExtension
Dim boolstatus As Boolean
Dim swfeat As Feature
Dim CutItem As String

Option Explicit

Sub main()
    Set swApp = Application.SldWorks
    Set Part = swApp.ActiveDoc
    Set modDocExt = Part.Extension


    ' Traverse FeatureManager design tree
    ' Get first feature in FeatureManager design tree
    swfeat = Part.FirstFeature


    'Get ID of first feature
    CutItem = swfeat.GetID

    ' Once body selected, create a bounding box
    boolstatus = modDocExt.SelectByID2(CutItem, "SUBWELDFOLDER", 0, 0, 0, False, 0, Nothing, 0)
    modDocExt.Create3DBoundingBox
End Sub

Dariusz Karcz Mar 6, 2017 12:26 PM

Correct Answer

Hi Raymond,

try this one:

Sub main()

Dim swApp As Object

Dim swmodel As ModelDoc2

Dim swPart As PartDoc

Dim boolstatus As Boolean

Dim swSelMgr As ISelectionMgr

Dim swBody As Body2

Dim vBodies As Variant

Dim j As Integer

Dim BodyFolder As SldWorks.BodyFolder

Dim CutListBdy As Body2

Set swApp = Application.SldWorks

Set swmodel = swApp.ActiveDoc

Set swPart = swmodel

Set swSelMgr = swmodel.SelectionManager

Set swBody = swSelMgr.GetSelectedObject6(0, -1)

Dim Feat As Feature

Set Feat = swmodel.FirstFeature

While Not Feat Is Nothing

If Feat.GetTypeName2 = "CutListFolder" Then

Dim swFeatName As String

swFeatName = Feat.Name

Feat.Select2 True, 0

Debug.Print swFeatName

Set BodyFolder = Feat.GetSpecificFeature2

vBodies = BodyFolder.GetBodies

For j = 0 To UBound(vBodies)

Set CutListBdy = vBodies(j)

Debug.Print CutListBdy.Name

swmodel.Extension.Create3DBoundingBox

Next j

End If

Set Feat = Feat.GetNextFeature()

Wend

End Sub

It is little bit messy, but it works.

It traverse thru all features, then select cutlist folders, then creates a bounding box for every body in cutlist folders.

Loop j is responsible for it, if you want to select only first item, then change this loop.

Preconditions:

Part need to have weldment feature and updated cutlist.

You can achive it, by using IbodyFolder --> UpdateCutList, and InsertWeldmentFeature Method (IFeatureManager)

I hope it will help you.

See the reply in context

No one else had this question

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Amen Allah Jlili Mar 6, 2017 11:42 AM

How about feature.Name?
CutItem = swfeat.Name

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Raymond Yau @ Amen Allah Jlili on Mar 7, 2017 5:04 AM

Hi Amen,

I tried this solution, but it didn't generate a 3D Bounding Box. It didn't even give me a debug option as no errors came up.

Actions

Dariusz Karcz Mar 6, 2017 12:26 PM

Hi Raymond,

try this one:

Sub main()

Dim swApp As Object

Dim swmodel As ModelDoc2

Dim swPart As PartDoc

Dim boolstatus As Boolean

Dim swSelMgr As ISelectionMgr

Dim swBody As Body2

Dim vBodies As Variant

Dim j As Integer

Dim BodyFolder As SldWorks.BodyFolder

Dim CutListBdy As Body2

Set swApp = Application.SldWorks

Set swmodel = swApp.ActiveDoc

Set swPart = swmodel

Set swSelMgr = swmodel.SelectionManager

Set swBody = swSelMgr.GetSelectedObject6(0, -1)

Dim Feat As Feature

Set Feat = swmodel.FirstFeature

While Not Feat Is Nothing

If Feat.GetTypeName2 = "CutListFolder" Then

Dim swFeatName As String

swFeatName = Feat.Name

Feat.Select2 True, 0

Debug.Print swFeatName

Set BodyFolder = Feat.GetSpecificFeature2

vBodies = BodyFolder.GetBodies

For j = 0 To UBound(vBodies)

Set CutListBdy = vBodies(j)

Debug.Print CutListBdy.Name

swmodel.Extension.Create3DBoundingBox

Next j

End If

Set Feat = Feat.GetNextFeature()

Wend

End Sub

It is little bit messy, but it works.

It traverse thru all features, then select cutlist folders, then creates a bounding box for every body in cutlist folders.

Loop j is responsible for it, if you want to select only first item, then change this loop.

Preconditions:

Part need to have weldment feature and updated cutlist.

You can achive it, by using IbodyFolder --> UpdateCutList, and InsertWeldmentFeature Method (IFeatureManager)

I hope it will help you.

Actions

Raymond Yau @ Dariusz Karcz on Mar 8, 2017 3:43 AM

Thanks Dariusz, your solution works very well.

I added some extra lines of code as I just realised that a weldment-cut-list table would have to first exist in the FeatureManagerTree before running your macro, so I added a line of code to create a weldment table before the While Not statement.

Here is the line of code added (in BOLD) to you your solution:

.....
Set swPart = swmodel
Set swSelMgr = swmodel.SelectionManager
Set swBody = swSelMgr.GetSelectedObject6(0, -1)

Dim Feat As Feature

Set Feat = swmodel.FeatureManager.InsertWeldmentFeature() 'Insert weldment feature

Set Feat = swmodel.FirstFeature
While Not Feat Is Nothing
If Feat.GetTypeName2 = "CutListFolder" Then
.....

This successfully creates a weldment cutlist table, but it doesn't continue to process the rest of the code and create a 3D Bounding Box. When I re-run the same macro, it unusually generates multiple weldment cutlists. Any ideas why this might happen?

Actions

Dariusz Karcz @ Raymond Yau on Mar 7, 2017 5:38 AM

Raymond,

currently I have do access to my PC with Sw installed, but try this:

Delete "Set Feat =" and leave only

swmodel.FeatureManager.InsertWeldmentFeature()

try assign a boolean for example:

dim bool as boolean

bool = swmodel.FeatureManager.InsertWeldmentFeature()

Please check it, it it fails, i will look into it later.

Actions

Raymond Yau @ Dariusz Karcz on Mar 8, 2017 3:42 AM

I've tried assigning a boolean, but it still creates multiple weldment tables (as shown in the image) and it doesn't execute the latter part of the code. Since I've removed the 'Set Feat', I also get an object error:

Actions

Dariusz Karcz @ Raymond Yau on Mar 8, 2017 3:13 PM

Raymond, here you go (still messy, but with little bit of comments inside of code), now its working, and does not insert multiple instances of weldment feature, if part is already a weldment:

Sub main()

Dim swApp As Object

Dim swmodel As ModelDoc2

Dim swPart As PartDoc

Dim boolstatus As Boolean

Dim swSelMgr As ISelectionMgr

Dim swBody As Body2

Dim vBodies As Variant

Dim j As Integer

Dim BodyFolder As SldWorks.BodyFolder

Dim CutListBdy As Body2

Dim Feat As Feature

Dim swIsWeldment As Boolean

Set swApp = Application.SldWorks

Set swmodel = swApp.ActiveDoc

Dim bool As Boolean

Set swPart = swmodel

Set swSelMgr = swmodel.SelectionManager

Set swBody = swSelMgr.GetSelectedObject6(0, -1)

swIsWeldment = swPart.IsWeldment

If swIsWeldment = False Then 'Check if part is weldment, if not, create weldment feature

swmodel.FeatureManager.InsertWeldmentFeature

swmodel.EditRebuild3

Else

End If

Set Feat = swmodel.FirstFeature 'get first feature

While Not Feat Is Nothing

If Feat.GetTypeName2 = "CutListFolder" Then 'check that first feature is cutlistfolder

Dim swFeatName As String

Set BodyFolder = Feat.GetSpecificFeature2 'get body folder interface

BodyFolder.GetAutomaticCutList

BodyFolder.UpdateCutList

swmodel.EditRebuild3

swFeatName = Feat.Name

Feat.Select2 True, 0

Debug.Print swFeatName

vBodies = BodyFolder.GetBodies

For j = 0 To UBound(vBodies)

Set CutListBdy = vBodies(j)

Debug.Print CutListBdy.Name

swmodel.Extension.Create3DBoundingBox

Next j

End If

Set Feat = Feat.GetNextFeature()

Wend

End Sub

Actions

Deepak Gupta @ Dariusz Karcz on Mar 8, 2017 3:15 PM

IsWeldment would only work if there is a weldment feature (like feature created using weldment profile).

Actions

Raymond Yau @ Deepak Gupta on Mar 9, 2017 3:20 AM

Hi Deepark,

It appears to work very well with both extruded solids and weldment profiles.

Actions

Deepak Gupta @ Raymond Yau on Mar 9, 2017 3:25 AM

Not sure but it was not working for me on extruded components and was adding multiple weldment feature (like you were facing earlier).

Glad to know it is working for you.

Actions

Raymond Yau @ Dariusz Karcz on Mar 9, 2017 3:17 AM

Thanks Dariusz, this is amazing. It works like a charm. I'm still learning the API as I go and this is a great learning exercise for me. I hope others might find this useful as well. Cheers.

Actions

11 Replies

Amen Allah Jlili Mar 6, 2017 11:42 AM
Mark Correct
Correct Answer
How about feature.Name?
CutItem = swfeat.Name
Like • Show 0 Likes0
Actions
- Raymond Yau @ Amen Allah Jlili on Mar 7, 2017 5:04 AM
  Mark Correct
  Correct Answer
  Hi Amen,
  
  I tried this solution, but it didn't generate a 3D Bounding Box. It didn't even give me a debug option as no errors came up.
  Like • Show 0 Likes0
  Actions
Dariusz Karcz Mar 6, 2017 12:26 PM
Unmark Correct
Correct Answer
Hi Raymond,
try this one:

Sub main()
    Dim swApp As Object
    Dim swmodel As ModelDoc2
    Dim swPart As PartDoc
    Dim boolstatus As Boolean
    Dim swSelMgr As ISelectionMgr
    Dim swBody As Body2
    Dim vBodies As Variant
    Dim j As Integer
    Dim BodyFolder As SldWorks.BodyFolder
    Dim CutListBdy As Body2

    Set swApp = Application.SldWorks
    Set swmodel = swApp.ActiveDoc

    Set swPart = swmodel
    Set swSelMgr = swmodel.SelectionManager
    Set swBody = swSelMgr.GetSelectedObject6(0, -1)

    Dim Feat As Feature
    Set Feat = swmodel.FirstFeature
    While Not Feat Is Nothing
        If Feat.GetTypeName2 = "CutListFolder" Then
        Dim swFeatName As String

        swFeatName = Feat.Name
        Feat.Select2 True, 0

        Debug.Print swFeatName

            Set BodyFolder = Feat.GetSpecificFeature2
            vBodies = BodyFolder.GetBodies
            For j = 0 To UBound(vBodies)
                Set CutListBdy = vBodies(j)
                Debug.Print CutListBdy.Name

                swmodel.Extension.Create3DBoundingBox


            Next j
        End If
        Set Feat = Feat.GetNextFeature()
    Wend
End Sub

It is little bit messy, but it works.
It traverse thru all features, then select cutlist folders, then creates a bounding box for every body in cutlist folders.
Loop j is responsible for it, if you want to select only first item, then change this loop.

Preconditions:
Part need to have weldment feature and updated cutlist.
You can achive it, by using IbodyFolder --> UpdateCutList, and InsertWeldmentFeature Method (IFeatureManager)

I hope it will help you.
Like • Show 1 Like1
Actions
- Raymond Yau @ Dariusz Karcz on Mar 8, 2017 3:43 AM
  Mark Correct
  Correct Answer
  Thanks Dariusz, your solution works very well.
  
  I added some extra lines of code as I just realised that a weldment-cut-list table would have to first exist in the FeatureManagerTree before running your macro, so I added a line of code to create a weldment table before the While Not statement.
  
  Here is the line of code added (in BOLD) to you your solution:
  .....
  Set swPart = swmodel
  Set swSelMgr = swmodel.SelectionManager
  Set swBody = swSelMgr.GetSelectedObject6(0, -1)
  
  Dim Feat As Feature
  
  Set Feat = swmodel.FeatureManager.InsertWeldmentFeature() 'Insert weldment feature
  
  Set Feat = swmodel.FirstFeature
  While Not Feat Is Nothing
  If Feat.GetTypeName2 = "CutListFolder" Then
  .....
  
  This successfully creates a weldment cutlist table, but it doesn't continue to process the rest of the code and create a 3D Bounding Box. When I re-run the same macro, it unusually generates multiple weldment cutlists. Any ideas why this might happen?
  Like • Show 0 Likes0
  Actions
  - Dariusz Karcz @ Raymond Yau on Mar 7, 2017 5:38 AM
    Mark Correct
    Correct Answer
    Raymond,
    
    currently I have do access to my PC with Sw installed, but try this:
    
    Delete "Set Feat =" and leave only
    
    swmodel.FeatureManager.InsertWeldmentFeature()
    
    or
    
    try assign a boolean for example:
    
    dim bool as boolean
    bool = swmodel.FeatureManager.InsertWeldmentFeature()
    
    Please check it, it it fails, i will look into it later.
    Like • Show 0 Likes0
    Actions
    - Raymond Yau @ Dariusz Karcz on Mar 8, 2017 3:42 AM
      Mark Correct
      Correct Answer
      I've tried assigning a boolean, but it still creates multiple weldment tables (as shown in the image) and it doesn't execute the latter part of the code. Since I've removed the 'Set Feat', I also get an object error:
      
      Like • Show 0 Likes0
      Actions
      - Dariusz Karcz @ Raymond Yau on Mar 8, 2017 3:13 PM
        Mark Correct
        Correct Answer
        Raymond, here you go (still messy, but with little bit of comments inside of code), now its working, and does not insert multiple instances of weldment feature, if part is already a weldment:
        
        Sub main()
            Dim swApp As Object
            Dim swmodel As ModelDoc2
            Dim swPart As PartDoc
            Dim boolstatus As Boolean
            Dim swSelMgr As ISelectionMgr
            Dim swBody As Body2
            Dim vBodies As Variant
            Dim j As Integer
            Dim BodyFolder As SldWorks.BodyFolder
            Dim CutListBdy As Body2
            Dim Feat As Feature
            Dim swIsWeldment As Boolean
        
        
            Set swApp = Application.SldWorks
            Set swmodel = swApp.ActiveDoc
            Dim bool As Boolean
        
            Set swPart = swmodel
            Set swSelMgr = swmodel.SelectionManager
            Set swBody = swSelMgr.GetSelectedObject6(0, -1)
        
               swIsWeldment = swPart.IsWeldment
        
                If swIsWeldment = False Then 'Check if part is weldment, if not, create weldment feature
        
                swmodel.FeatureManager.InsertWeldmentFeature
            swmodel.EditRebuild3
                Else
        
                End If
        
        
            Set Feat = swmodel.FirstFeature 'get first feature
            While Not Feat Is Nothing
                If Feat.GetTypeName2 = "CutListFolder" Then 'check that first feature is cutlistfolder
                Dim swFeatName As String
        
                    Set BodyFolder = Feat.GetSpecificFeature2 'get body folder interface
                    BodyFolder.GetAutomaticCutList
                    BodyFolder.UpdateCutList
                    swmodel.EditRebuild3
        
                    swFeatName = Feat.Name
                Feat.Select2 True, 0
        
                Debug.Print swFeatName
                    vBodies = BodyFolder.GetBodies
                    For j = 0 To UBound(vBodies)
                        Set CutListBdy = vBodies(j)
                        Debug.Print CutListBdy.Name
        
                        swmodel.Extension.Create3DBoundingBox
        
        
                    Next j
                End If
                Set Feat = Feat.GetNextFeature()
            Wend
        End Sub
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        Deepak Gupta @ Dariusz Karcz on Mar 8, 2017 3:15 PM
        Mark Correct
        Correct Answer
        IsWeldment would only work if there is a weldment feature (like feature created using weldment profile).
        Like • Show 0 Likes0
        Actions
        Raymond Yau @ Deepak Gupta on Mar 9, 2017 3:20 AM
        Mark Correct
        Correct Answer
        Hi Deepark,
        
        It appears to work very well with both extruded solids and weldment profiles.
        
        Like • Show 0 Likes0
        Actions
        Deepak Gupta @ Raymond Yau on Mar 9, 2017 3:25 AM
        Mark Correct
        Correct Answer
        Not sure but it was not working for me on extruded components and was adding multiple weldment feature (like you were facing earlier).
        
        Glad to know it is working for you.
        Like • Show 0 Likes0
        Actions
        Raymond Yau @ Dariusz Karcz on Mar 9, 2017 3:17 AM
        Mark Correct
        Correct Answer
        Thanks Dariusz, this is amazing. It works like a charm. I'm still learning the API as I go and this is a great learning exercise for me. I hope others might find this useful as well. Cheers.
        Like • Show 0 Likes0
        Actions

How to select Cutlist Item and create a 3D Bounding Box

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