multiple iso views
multiple iso views
(OP)
I once found in a tip/trick for making multiple isoviews in the view orientation box. Does anyone have this proceedure? It's setes up the box so you can quickly get the right front, right rear, left front, and left rear isometric views while your working on a part or assembly.






RE: multiple iso views
Bradley
RE: multiple iso views
http://www.shounco.com/sw/TipsnTricks.htm
RE: multiple iso views
I have a view defined in my drwaing template called "TitleBlockOnly" I have a macro button assigned to this. Guess what it does?
Crashj 'doh' Johnson
RE: multiple iso views
1) Choose the face you want to be at the lower left
of your new ISO view
2) Set your screen view normal to that face
3) Bring up your 'view orientation' dialogue
4) Update your Front view to be the current view.
5) Switch to the ISO view.
6) Create a new view with an appropriate name.
7) You can now reset the standard views and Solidworks
will still remember how to display the new ISO
I know it sounds complicated, but it goes quickly once you know what you are going for.
RE: multiple iso views
A Related Side Note: There is a standard views toolbar that both changes view and magnifies to extents from a single button click. Check it out <View><toolbars>
RE: multiple iso views
Set model to standard *isometric view then hold down the shift key and press one of the arrow keys. This will rotate your view of the part 90 degrees.
-Caper-
RE: multiple iso views
' *********************************************************
' ISOViews - macro recorded on 12/20/01 by Mike J. Wilson
' *********************************************************
' Special thanks to Dennis Kelley and Dan Hanger for tips
' Modified to include all 8 Iso Views by Lee Bell
Dim swApp As Object
Dim Part As Object
Dim boolstatus As Boolean
Dim longstatus As Long
Dim Annotation As Object
Dim Gtol As Object
Dim DatumTag As Object
Dim FeatureData As Object
Dim Feature As Object
Dim Component As Object
Sub main()
Set swApp = CreateObject("SldWorks.Application")
Set Part = swApp.ActiveDoc
pi = 4 * Atn(1)
Z = Tan(30 * pi / 180)
X = Atn(Z / Sqr(-Z * Z + 1))
Y = -45 * pi / 180
Part.DeleteNamedView ("TRF-ISO")
Part.DeleteNamedView ("TRR-ISO")
Part.DeleteNamedView ("TLF-ISO")
Part.DeleteNamedView ("TLR-ISO")
Part.DeleteNamedView ("BRF-ISO")
Part.DeleteNamedView ("BRR-ISO")
Part.DeleteNamedView ("BLF-ISO")
Part.DeleteNamedView ("BLR-ISO")
Part.ShowNamedView2 "*Front", -1
Part.ActiveView().RotateAboutCenter X, Y
Part.ViewZoomtofit
Part.NameView ("TRF-ISO")
Part.ShowNamedView2 "*Right", -1
Part.ActiveView().RotateAboutCenter X, Y
Part.ViewZoomtofit
Part.NameView ("TRR-ISO")
Part.ShowNamedView2 "*Back", -1
Part.ActiveView().RotateAboutCenter X, Y
Part.ViewZoomtofit
Part.NameView ("TLR-ISO")
Part.ShowNamedView2 "*Left", -1
Part.ActiveView().RotateAboutCenter X, Y
Part.ViewZoomtofit
Part.NameView ("TLF-ISO")
Part.ShowNamedView2 "*Front", -1
Part.ActiveView().RotateAboutCenter -X, Y
Part.ViewZoomtofit
Part.NameView ("BRF-ISO")
Part.ShowNamedView2 "*Right", -1
Part.ActiveView().RotateAboutCenter -X, Y
Part.ViewZoomtofit
Part.NameView ("BRR-ISO")
Part.ShowNamedView2 "*Back", -1
Part.ActiveView().RotateAboutCenter -X, Y
Part.ViewZoomtofit
Part.NameView ("BLR-ISO")
Part.ShowNamedView2 "*Left", -1
Part.ActiveView().RotateAboutCenter -X, Y
Part.ViewZoomtofit
Part.NameView ("BLF-ISO")
Set Part = Nothing
Set swApp = Nothing
End Sub
Lee
RE: multiple iso views
RE: multiple iso views
The answer is yes; “SolidWorks help” explains it very well.
Go to the SolidWorks help, search for orientation. Read that. Once you have a named view you can insert it in a drawing.
Bradley
RE: multiple iso views
How are you creating your views in the drawing? You will only be able to change the View’s Orientation if you Do Not accept the current view when the view is created.
WRINKLED was NOT one of the things I wanted to be when I grew up!
RE: multiple iso views