Hi,
I often find myself fiddling around to select the origin when dimensioning sketches, does anyone know of a macro that selects the origin while I'm in the smart dimension?
I know that I can select the origin prior to starting smart dimension but that's still a bit awkward.
Br,
I just had the same thought as the OP and found this.
Your macro works great for a dimension of a line. I frequently dimension between a point and the origin (as in the hole wizard) and before I place the dimension as I move the mouse it will change from a straight line between the two points to a dimension in either the x or y axis.
Is it possible to make the macro create the dimension but not place it so I can still choose where to place it and therefore along which axis it is measuring?
When I delete the last section so it doesn't create it automatically it highlights the origin but the smart dimension seems to be ignoring that fact that it is selected and so I still have to manually select it.
I don't think it's possible to not place the dimension.
What you can do is 2 macros for either vertical or horizontal dimension
Option Explicit
Sub main()
Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim swSelMgr As SldWorks.SelectionMgr
Dim myDisplayDim As SldWorks.DisplayDimension
Dim selObj As Object
Dim UserPreference As Boolean
Dim boolstatus As Boolean
Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
Set swSelMgr = Part.SelectionManager
Set selObj = swSelMgr.GetSelectedObject6(1, 0)
boolstatus = Part.Extension.SelectByID2("Point1@Origin", "EXTSKETCHPOINT", 0, 0, 0, True, 0, Nothing, 0)
UserPreference = swApp.GetUserPreferenceToggle(swUserPreferenceToggle_e.swInputDimValOnCreate)
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False
Set myDisplayDim = Part.AddVerticalDimension2(0, 0, 0)' Set myDisplayDim = Part.AddHorizontalDimension2(0, 0, 0)
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, UserPreference
End Sub
An other possibility would be to use the mouse position relative to the 2 points with: 2017 SOLIDWORKS API Help - GetMouse Method (IModelView)
Hello,
This macro will create a dimension between the user selection and the origin
Preconditions:
- a sketch must be opened
- an object (line, point, etc...) must be selected in the sketch
Sub main()
Dim swApp As Object
Dim Part As Object
Dim boolstatus As Boolean
Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
Dim swSelMgr As SldWorks.SelectionMgr
Set swSelMgr = Part.SelectionManager
Dim selObj As Object
Set selObj = swSelMgr.GetSelectedObject6(1, 0)
boolstatus = Part.Extension.SelectByID2("Point1@Origin", "EXTSKETCHPOINT", 0, 0, 0, True, 0, Nothing, 0)
' If you don't want to create the dimension automatically, remove the lines below
Dim UserPreference As Boolean
UserPreference = swApp.GetUserPreferenceToggle(swUserPreferenceToggle_e.swInputDimValOnCreate)
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False
Dim myDisplayDim As Object
Set myDisplayDim = Part.AddDimension2(0, 0, 0)
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, UserPreference
End Sub