Need Help with Auto Dimension Macro 2

[joshF]

Looking for help on a auto-Dimension Macro. I have the Auto-Dimension Code, But I'd like to add a feature where I pick the corner (vertex) to be a zero.

Right now it defaults to the bottom/left hand corner. (which is not always ideal)

Can anyone help me with selecting a Vertex in the a drawing view and making this the Zero point for ordinate dimensions?

[indent]Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
'Dim swmodel As SldWorks.ModelDoc2

Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long

Sub main()

Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
Part.ClearSelection2 True
boolstatus = Part.ActivateSheet("Sheet1")
boolstatus = Part.ActivateView("Drawing View1")

'vertical
boolstatus = Part.Extension.SelectByID2("Drawing View1", "DRAWINGVIEW", 0, 0, 0, False, 0, Nothing, 0)
boolstatus = Part.Extension.SelectByRay(0.109400029853413, 0.130434382958623, 6.34999999999764E-03, 0, 0, -1, 1.28866875828181E-03, 1, True, 4, 0)
longstatus = Part.AutoDimension(1, 2, 1, 2, -1)

'Horizontal
boolstatus = Part.Extension.SelectByID2("Drawing View1", "DRAWINGVIEW", 0, 0, 0, False, 0, Nothing, 0)
boolstatus = Part.Extension.SelectByRay(8.28686142417286E-02, 0.106556108908108, 6.34999999988395E-03, 0, 0, -1, 1.28866875828181E-03, 1, False, 0, 0)
longstatus = Part.AutoDimension(1, 2, 1, 2, -1)

End Sub[/indent]

 

[ctopher]

I'm not sure. But, try under "View, annotations, Model items".

Chris, CSWP
SolidWorks '20
ctophers home
SolidWorks Legion

 

[sanganaksakha]

Hello,

See if this works for you.

Insert a sketch point in 'Drawing View3' at the desired point. Select the sketch point. (Make sure that no other object is selected.)

Then run the following code.

Option Explicit

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
'Dim swmodel As SldWorks.ModelDoc2

Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long

Sub main()

    Set swApp = Application.SldWorks
    Set Part = swApp.ActiveDoc
        
    'Horizontal

    Dim thePT As Object
    Set thePT = Part.SelectionManager.GetSelectedObject6(1, -1)
    ''''' Select the sketchpoint
    
    '''''''''''''''''
    Dim sData As SelectData
    
    Set sData = Part.SelectionManager.CreateSelectData
    
    sData.Mark = swAutodimMark_e.swAutodimMarkOriginDatum
    '''' See help for details.
    
    Call thePT.Select4(False, sData)
    '''''''''''''''''
    
    ''''''''''''''''''''''
    ''''' This code must be after Sketchpoint is processed. Otherwise sketchpoint gets unselected.
    
    boolstatus = Part.ActivateSheet("Sheet1")
    boolstatus = Part.ActivateView("Drawing View3")
    boolstatus = Part.Extension.SelectByID2("Drawing View3", "DRAWINGVIEW", 0, 0, 0, False, 0, Nothing, 0)
    
    ''''''''''''''''
    
    longstatus = Part.AutoDimension(1, 2, 1, 2, -1)

End Sub

 

[TheTick]

I have a much faster process for making auto-dimensioned prints. The quality is the same and the paper is much cheaper.