New Drawing Macro Help

I've got a macro question, I'm trying to make a macro that creates a
new drawing file from an assembly file, I am then wanting it to
generate various views placed in the same place. The last couple of
lines are the problem, this macro places views of a certain file but if
I open up a different assembly and make a drawing it places the views
from the first assembly. Any help would be greatly appreciated. I
know very little about Visual Basic, I'm currently taking a class in it
but I haven't learned much yet. I'm looking for the command to use
that selects the currently opened file name and puts it as a variable
to use in the drawing view creation. Also is there any way to make a
macro to do the selected dimension. For example a macro to change a
dimension that is selected to mm from inches?

'
******************************************************************************
' D:\DOCUME~1\LUCASL~1\LOCALS~1\Temp\swx4356\Macro1.swb - macro
recorded on 05/28/06 by *********************
'
******************************************************************************
Dim swApp As Object
Dim Part As Object
Dim SelMgr As Object
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long
Dim Feature As Object

Sub main()

Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
Set SelMgr = Part.SelectionManager
swApp.ActiveDoc.ActiveView.FrameLeft = 0
swApp.ActiveDoc.ActiveView.FrameTop = 0
swApp.ActiveDoc.ActiveView.FrameState = 1
Set Part = swApp.NewDocument("Drawing Template File Path", 12, 0.2794,
0.4318)
Set Part = swApp.ActiveDoc
Set SelMgr = Part.SelectionManager
Part.ViewZoomtofit2
boolstatus = Part.ActivateView("Drawing View1")
boolstatus = Part.Extension.SelectByID2("Drawing View1", "DRAWINGVIEW",
0.1173527476636, 0.1787637757009, 0, False, 0, Nothing, 0)
Part.EditDelete
Dim DrawView As Object
Set DrawView = Part.CreateDrawViewFromModelView2("Assembly File Path",
"*Isometric", 0.1297821308411, 0.1627831401869, 0)
boolstatus = Part.ActivateView("Drawing View4")
Set DrawView = Part.CreateDrawViewFromModelView2("Assebly File Path",
"*Front", 0.294915364486, 0.1610075140187, 0)
Part.ClearSelection2 True
End Sub

Lucas Laverman
Senior, Mechanical Engineering

 

Well it sounds like what you are trying to do is already covered by
existing SolidWorks functionality. It is called "predefined views" and
you can save a drawing of this type as a template. Take the drawing
you want and do insert -> drawing view -> predefined. Place it on
drawing sheet and then fill out the property manager information. Now
to populate all your drawing views just drag a part/assembly/whatever
into the drawing and all the views will populate. Or you can rmb a
predefined view and choose "insert model."

In regards to your code: What I imagine you want to happen is that user
opens an assembly then runs the macro and the drawing gets created. To
do this define your assembly and part variables separately. I didn't
test this, but the below code should pretty much do what you want.
Essentially the currently open document is assumed to be your assembly.
I store it in an Assembly variable. Then I create a drawing and store
its information in the Drawing variable. By separating them I don't
mix up information.


Dim swApp As Object
Dim Assembly As Object
Dim Drawing As Object
Dim SelMgr As Object
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long
Dim Feature As Object
Dim DrawView As Object

Sub main()

Set swApp = Application.SldWorks
Set Assembly = swApp.ActiveDoc
Set SelMgr = Assembly.SelectionManager
Set Drawing = swApp.NewDocument("Drawing Template File Path", 12,
0.2794,
0.4318)

boolstatus = Drawing .Extension.SelectByID2("Drawing View1",
"DRAWINGVIEW",
0.1173527476636, 0.1787637757009, 0, False, 0, Nothing, 0)
Drawing.EditDelete

Set DrawView = Drawing
..CreateDrawViewFromModelView2(Assembly.GetPathName,
"*Isometric", 0.1297821308411, 0.1627831401869, 0)

Set DrawView =
Drawing.CreateDrawViewFromModelView2(Assembly.GetPathName,
"*Front", 0.294915364486, 0.1610075140187, 0)
Drawing.ClearSelection2 True
End Sub

 

Dimensions are tricky. You would use:

DisplayDimension::SetUnits

I would recommend looking at some examples in API help to figure it out.