Add dimensions to bend lines using SOLIDWORKS API
This example demonstrates how to add dimensions to bend lines in the drawing view of sheet metal flat pattern using SOLIDWORKS API.
It is required to select the sketch lines using the select data object with the view assigned, otherwise the dimensions creating will fail.
IModelDoc2::AddDimension2 SOLIDWORKS API is used to add the dimension. Dimension is positioned at (0, 0, 0) coordinate. Refer the Dimension Visible Entities example for code snippet for calculating the optimal dimension position.
Dim swApp As SldWorks.SldWorks Dim swModel As SldWorks.ModelDoc2 Dim swSelMgr As SldWorks.SelectionMgr Dim swView As SldWorks.View Sub main() Set swApp = Application.SldWorks Set swModel = swApp.ActiveDoc If Not swModel Is Nothing Then Set swSelMgr = swModel.SelectionManager Set swView = swSelMgr.GetSelectedObject6(1, -1) If Not swView Is Nothing Then Dim vBendLines As Variant vBendLines = swView.GetBendLines If UBound(vBendLines) >= 1 Then Dim swSelData As SldWorks.SelectData Set swSelData = swSelMgr.CreateSelectData swSelData.View = swView 'must be set swModel.ClearSelection2 True Dim i As Integer For i = 0 To 1 Dim swSkSeg As SldWorks.SketchSegment Set swSkSeg = vBendLines(i) swSkSeg.Select4 True, swSelData Next swModel.AddDimension2 0, 0, 0 Else MsgBox "There should be at least 2 bend lines in the drawing view" End If Else MsgBox "Please select drawing view with flat pattern" End If Else MsgBox "Please open drawing" End If End Sub