Align line along axis using SOLIDWORKS API

Example demonstrates how to align all sketch lines in the active sketch (add the sketch relation) with one of the selected options using SOLIDWORKS API:

Along X (horizontal)
Along Y (vertical)
Along Z

This example will work with both 2D and 3D sketch.

ISketchRelationManager SOLIDWORKS API interface is used to manage the relations of the sketch entities.

Enum AlignmentDir_e
    AlongX = 1
    AlongY = 2
    AlongZ = 3
End Enum

Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swSketch As SldWorks.Sketch
Dim swSketchRelMgr As SldWorks.SketchRelationManager

Sub main()

    On Error Resume Next
    
    Set swApp = Application.SldWorks
    
    Set swModel = swApp.ActiveDoc
    
    If Not swModel Is Nothing Then
        
        Set swSketch = swModel.SketchManager.ActiveSketch
        
        If Not swSketch Is Nothing Then
            
            Dim dir As AlignmentDir_e
            dir = InputBox("Specify the type of alignment for sketch lines: 1 - Along X, 2 - Along Y, 3 - Along Z")
            
            Set swSketchRelMgr = swSketch.RelationManager
            
            Dim vSegs As Variant
                        
            vSegs = swSketch.GetSketchSegments
         
            Dim swSkLines() As SldWorks.SketchSegment
            Dim isSkLinesArrInit As Boolean
            isSkLinesArrInit = False
            
            For i = 0 To UBound(vSegs)
                
                Dim swSkSeg As SldWorks.SketchSegment
                Set swSkSeg = vSegs(i)
                
                If swSkSeg.GetType() = swSketchSegments_e.swSketchLINE Then
                    
                    If Not isSkLinesArrInit Then
                        isSkLinesArrInit = True
                        ReDim swSkLines(0)
                    Else
                        ReDim Preserve swSkLines(UBound(swSkLines) + 1)
                    End If
                    
                    Set swSkLines(UBound(swSkLines)) = swSkSeg
                    
                End If
                
            Next
            
            Dim constType As swConstraintType_e
                
            Select Case dir
                Case AlignmentDir_e.AlongX
                    If swSketch.Is3D() Then
                        constType = swConstraintType_e.swConstraintType_ALONGX3D
                    Else
                        constType = swConstraintType_e.swConstraintType_HORIZONTAL
                    End If
                Case AlignmentDir_e.AlongY
                    If swSketch.Is3D Then
                        constType = swConstraintType_e.swConstraintType_ALONGY3D
                    Else
                        constType = swConstraintType_e.swConstraintType_VERTICAL
                    End If
                Case AlignmentDir_e.AlongZ
                    If swSketch.Is3D Then
                        constType = swConstraintType_e.swConstraintType_ALONGZ
                    Else
                        MsgBox "Invalid. Z is not a valid orientation for 2D Sketch"
                        End
                    End If
            End Select
            
            swSketchRelMgr.AddRelation swSkLines, constType
        
        Else
            MsgBox "Please open the sketch"
        End If
    
    Else
        MsgBox "Please open document"
    End If
    
End Sub