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Loft surface using sketch segments

Question asked by Marco Maso on Oct 31, 2018
Latest reply on Nov 4, 2018 by Artem Taturevych

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Hello again, I have a series of sketch with several sketch segments inside. I would like to create a simple macro that, after selecting two sketch segments, let me quickly create a surface loft.

Unfortunately I can't get InsertLoftRefSurface2 to work, no matter what.

At the moment I simply select two sketch segments in the interface, then launch the macro. The macro:

1. Saves the two selected sketch segments in an array

2. Clears the selection

3. Using ModelDoc2 selects the two sketch segments again using SelectByID2 with mark 1 as per InsertLoftRefSurface2 API remarks

4. If both selections are true (and they are) performs a InsertLoftRefSurface2(false, false, false, 1.0, 0, 0)

Solidworks spins for a second then nothing happens. No errors, no clues, nothing.

I registered a macro doing the same within the interface. The main difference is that the macro selects the two sketch segments using SelectByID2("Unknow", "SELOBJGROUP", [etc.]) with mark 1.

I was also trying to create a temporary body by using Modeler.CreateLoftBody2 but I can't get InsertLoftRefSurface2 to work, let alone CreateLoftBody2.

Is there something I'm not aware of?

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Fifi Riri Oct 31, 2018 11:53 AM
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Could you post your macro's code?
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- Marco Maso @ Fifi Riri on Oct 31, 2018 12:24 PM
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  Absolutely, here's the relevant code.
  
  Dim swApp As SldWorks.SldWorks
  Dim swModel As SldWorks.ModelDoc2
  Dim swModelExtension As SldWorks.ModelDocExtension
  Dim swSelectionManager As SldWorks.SelectionMgr
  Dim selStatus As Boolean
  
  ' Precondition: two sketch segments selected in the interface
  
  Sub main()
  
  Set swApp = Application.SldWorks
  Set swModel = swApp.ActiveDoc
  Set swModelExtension = swModel.Extension
  Set swSelectionManager = swModel.SelectionManager
  
  If swSelectionManager.GetSelectedObjectCount2(-1) = 2 Then
  
      Dim sketchSegment1 As SldWorks.SketchSegment
      Dim sketchSegment2 As SldWorks.SketchSegment
  
      Dim sketchFeature1 As SldWorks.Feature
      Dim sketchFeature2 As SldWorks.Feature
  
      Set sketchSegment1 = swSelectionManager.GetSelectedObject6(1, -1)
      Set sketchSegment2 = swSelectionManager.GetSelectedObject6(2, -1)
  
      Set sketchFeature1 = sketchSegment1.GetSketch()
      Set sketchFeature2 = sketchSegment2.GetSketch()
  
      swModel.ClearSelection2 (True)
  
      Debug.Print "ID #1: " & sketchSegment1.GetName() & "@" & sketchFeature1.Name
      Debug.Print "ID #2: " & sketchSegment2.GetName() & "@" & sketchFeature2.Name
  
      selStatus = swModelExtension.SelectByID2(sketchSegment1.GetName() & "@" & sketchFeature1.Name, "EXTSKETCHSEGMENT", 0, 0, 0, False, 1, Nothing, 0)
      Debug.Print "First sketch segment selection status: " & selStatus
  
      selStatus = swModelExtension.SelectByID2(sketchSegment2.GetName() & "@" & sketchFeature2.Name, "EXTSKETCHSEGMENT", 0, 0, 0, True, 1, Nothing, 0)
      Debug.Print "Second sketch segment selection status: " & selStatus
  
      swModel.InsertLoftRefSurface2 False, True, False, 1, 0, 0
  
  End If
  
  End Sub
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  - Fifi Riri @ Marco Maso on Nov 1, 2018 2:54 AM
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    The macro you posted works fine for me.
    And this works just as well:
    
    Option Explicit
    Dim swApp As SldWorks.SldWorks
    Dim swModel As SldWorks.ModelDoc2
    Dim swSelectionManager As SldWorks.SelectionMgr
    Sub main()
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    Set swSelectionManager = swModel.SelectionManager
    If swSelectionManager.GetSelectedObjectCount2(-1) = 2 Then
    swModel.InsertLoftRefSurface2 False, True, False, 1, 0, 0
    End If
    End Sub
    
    It might depends of the sketch segments themselves.
    Could you post your file?
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  - Artem Taturevych @ Marco Maso on Nov 1, 2018 5:08 AM
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    That most likely incorrect selection points on the profile. Like the one below (blue points):
    You need to use ISelectionMgr::SetSelectionPoint2 to set the points.
    
    But better approach is to use ISketchSegment::Select4 method instead of SelectByID2 and set the selection point via ISelectData::X, ISelectData::Y and ISelectData::Z properties for the selection data in the second parameter.
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    - Marco Maso @ Artem Taturevych on Nov 2, 2018 12:51 PM
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      Excuse me, could you point to me how to correctly use ISelectData? Because I tried but I still don't get anything.
      
          swModel.ClearSelection2 True
      
          Set swSelectData = swSelectionManager.CreateSelectData
      
          swSelectData.Mark = 1
          swSelectData.X = skPtMt1.ArrayData(0)
          swSelectData.Y = skPtMt1.ArrayData(1)
          swSelectData.Z = skPtMt1.ArrayData(2)
          sketchSegment1.Select4 True, swSelectData
      
          swSelectData.X = skPtMt2.ArrayData(0)
          swSelectData.Y = skPtMt2.ArrayData(1)
          swSelectData.Z = skPtMt2.ArrayData(2)
          sketchSegment2.Select4 True, swSelectData
      
          swModel.InsertLoftRefSurface2 False, True, False, 1, 0, 0
      
      skPtMt1 and skPtMt2 are the right side points. I also tried making a line between them and I can confirm they are correct and aligned for loft uses.
      
      I also tried:
      
          Set swSelectData = swSelectionManager.CreateSelectData
          swSelectData.Mark = 1
      
          selStatus = sketchSegment1.Select4(True, swSelectData)
          selStatus = swSelectionManager.SetSelectionPoint2(1, -1, skPtMt1.ArrayData(0), skPtMt1.ArrayData(1), skPtMt1.ArrayData(2))
          selStatus = sketchSegment2.Select4(True, swSelectData)
          selStatus = swSelectionManager.SetSelectionPoint2(1, -1, skPtMt2.ArrayData(0), skPtMt2.ArrayData(1), skPtMt2.ArrayData(2))
      
           'selStatus is true / true / true / true
      
          swModel.InsertLoftRefSurface2 False, True, False, 1, 0, 0
      
      Just to clarify here's what I'm trying to achieve:
      
      One small thing that irks me is that I don't get any kind of feedback on what I'm doing. You need to perfectly know how the API works because SW won't give you any error code, am I correct?
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      - Artem Taturevych @ Marco Maso on Nov 2, 2018 5:39 PM
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        Your first snippet looks correct to me. Second one doesn't as you set the second selection point to the first selection object (you have 1 used twice in the SetSelectionPoint2 method).
        
        Could you please attach this part document?
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        Marco Maso @ Artem Taturevych on Nov 2, 2018 7:49 PM
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        Sure, albeit it's nothing special, just a very basic file to test the macro. Please also find attached the whole code. It's a bit verbose because I wanted to be sure everything was setup correctly.
        
        Preconditions: select only one sketch segment per sketch.
        
        Also it's interesting to note that the code works fine in the "works" file, when there are no other sketch segments inside the sketch. I am prone to think it's still a selection problem.
        
        Mentioning Fifi Riri that asked for the file before. Thanks for your help guys.
        Attachments
        SketchSegmentLoft.swp.zip10.2 KB
        LoftAPI - Doesnt work.SLDPRT.zip34.6 KB
        LoftAPI - Works.SLDPRT.zip31.2 KB
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        Artem Taturevych @ Marco Maso on Nov 4, 2018 1:01 AM
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        Hi Marco,
        
        Thank you for the example models. I now understand the issue. Sketch segments are not valid selection objects for the loft feature. Note that you cannot select segment from the UI as well. When you do it you are prompted to select the open loop via selection manager:
        
        In your second example you have one segment per sketch so it automatically using the entire sketch for profile.
        
        If you want to use only some entities from the sketch you need to use sketch contours instead of sketch segments. Take a look at this example which works with your sample models: Create Surface Loft Feature Via Contours
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Loft surface using sketch segments

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