API : sketching in a drawing view ?

I can't reach to sketch in a drawing view. Below is a macro that creates a
view and draws 10 random lines, but they appear on the background, not in
the desired view.
Any idea ? (Macro recording & playback doesn't work...) Thanks!

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)
Dim view As SldWorks.view
Set view = doc.GetFirstView
Call doc.SelectByID(viewname, "DRAWINGVIEW", 0, 0, 0)
Dim sketch As SldWorks.sketch
Set sketch = view.GetSketch
sketch.Select (False)
Call doc.EditSketch
Set sketch = doc.GetActiveSketch
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

 

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(),
0)
Next i

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

 

I can't reach to sketch in a drawing view. Below is a macro that creates a

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,
0, 0)
'''''' NOT NEEDED '''''Dim sketch As SldWorks.sketch
'''''' NOT NEEDED '''''Set sketch = view.GetSketch
'''''' NOT NEEDED '''''sketch.Select (False)
'''''' NOT NEEDED '''''Call doc.EditSketch
'''''' NOT NEEDED '''''Set sketch = doc.GetActiveSketch

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