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Re: Loft surface using sketch segments
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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Re: Loft surface using sketch segments
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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Re: Loft surface using sketch segments
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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Re: Loft surface using sketch segments
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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Re: Loft surface using sketch segments
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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Re: Loft surface using sketch segments
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.
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Re: Loft surface using sketch segments
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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