API : sketching in a drawing view ?

Philippe,

The following macro creates lines in the desired view:

Dim doc As SldWorks.DrawingDoc

Public Sub main() Set app = Application.SldWorks Set doc = app.NewDrawing2(swDwgTemplateA3size, "", 0, 0, 0) Dim l, h As Double l = 0.3 h = 0.2 Dim viewname As String viewname = doc.CreateViewport2(0, 0, l, h, 0, 1) Call doc.SelectByID(viewname, "DRAWINGVIEW", 0, 0, 0) Call doc.EditSheet Dim i As Integer For i = 1 To 10 Call doc.CreateLine2(l * Rnd(), h * Rnd(), 0, l * Rnd(), h * Rnd(),

End Sub

I used EditSheet instead of EditSketch and got rid of a few lines that looked like they they were there for debugging purposes.

EditSheeeeeeeeet ! that's it! thanks a lot, Paul!

you have to get the document that the drawing view was created from. exp. if it was a drawing view of a part file. then retrive that parts modeldoc2. View::ReferencedDocument

hopes this helps Sean Phillips

Yes, I went thru this before, myself. Apparently, while SW usually treats any other freshly-created object as the "current" object, when it comes to views, the 'current' view is the sheet itself. The fix is a "one-liner" .. Option Explicit Dim app As SldWorks.SldWorks Dim doc As SldWorks.DrawingDoc Public Sub main() Set app = Application.SldWorks Set doc = app.NewDrawing2(swDwgTemplateA3size, "", 0, 0, 0) Dim l, h As Double l = 0.3 h = 0.2 Dim viewname As String viewname = doc.CreateViewport2(0, 0, l, h, 0, 1)

'''''' NOT NEEDED ''''' Dim view As SldWorks.view '''''' NOT NEEDED ''''' Set view = doc.GetFirstView '''''' NOT NEEDED '''''Call doc.SelectByID(viewname, "DRAWINGVIEW", 0,

success = doc.ActivateView(viewname) ''''''' THE ONE "MAGIC" LINE

Dim i As Integer For i = 1 To 10 Call doc.CreateLine2(l * Rnd(), h * Rnd(), 0, l * Rnd(), h * Rnd(), 0) Next i End Sub

also, the RND function doesnt really generate random numbers unless you 'seed' it, normally with the timer function:

Randomize Timer ' uses milliseconds past misnight as a seed