This VBA macro demonstrates how to find the specific named edge from the underlying 3D document and select it in the drawing view.
This technique can be used when developing drawing automation macros and applications.
Note in your macro you might not use named entities, instead some different logic can be applied (e.g. finding by coordinates, color, attributes etc.). However the process of conversion the pointer to drawing view space will be the same.
This macro will work with the drawing view of the assembly where named edge is contained in the top level component as shown below:
Refer Get Component By Name example for the code to get component on any level if needed.
Name of the edge needs to be assigned from the corresponding part document.
Dim swApp As SldWorks.SldWorks Sub main() Set swApp = Application.SldWorks Dim swDraw As SldWorks.DrawingDoc Set swDraw = swApp.ActiveDoc Dim swView As SldWorks.view Set swView = swDraw.FeatureByName("Drawing View1").GetSpecificFeature() Dim swEdge As SldWorks.edge Set swEdge = FindEdge(swDraw, swView, "Part1-1", "MyEdge") Debug.Print swView.SelectEntity(swEdge, False) End Sub Function FindEdge(draw As SldWorks.DrawingDoc, view As SldWorks.view, compName As String, edgeName As String) As SldWorks.edge Dim swAssy As SldWorks.AssemblyDoc Set swAssy = view.ReferencedDocument Dim swComp As SldWorks.Component2 Set swComp = swAssy.GetComponentByName(compName) Dim swRefPart As SldWorks.PartDoc Set swRefPart = swComp.GetModelDoc2 Dim swEdge As SldWorks.edge Set swEdge = swRefPart.GetEntityByName(edgeName, swSelectType_e.swSelEDGES) Set swEdge = swComp.GetCorresponding(swEdge) Set FindEdge = swEdge End Function