Turn off 2D sketch via code

[NachoShaw]

Hi

how can i turn off the 2D sketch on an assembly just like the clicking of the tick box in Views?

need to turn this off for every assembly i open automatically. Can it be done?

Thanks

[VdVeek]

I think it's a much better way to set the visibility of all the sketches in all parts to unvisible instead of turning the visibility off by the "Object Visibility" Command. I use a VBA-script to switch the visibility of each sketch in an assembly. You can test this script, but at large assemblies it can take some time. See attachment for the VBA-script.

Rob.

[GosponZ]

'Attribute VB_Name = "Hide_Sketches_And_planes"
Sub Hide_Sketches_And_planes()

'catch and skip errors
On Error Resume Next

    ' Get the active document.
    Dim oDoc As Document
    Set oDoc = ThisApplication.ActiveDocument

    If oDoc.DocumentType = kAssemblyDocumentObject Then
    Call HideAssemblyComponents

    ElseIf oDoc.DocumentType = kPartDocumentObject Then
    Call HidePartComponents

    Else
    MsgBox ("The active file is no assembly or part. Script can't be used here.")
    Exit Sub
    End If
    
End Sub

Private Sub HideAssemblyComponents()

Dim oAsmDoc As AssemblyDocument
Set oAsmDoc = ThisApplication.ActiveDocument
'get user input as True or False
Dim Vis As Boolean
Dim result
result = MsgBox("Hide all sketches and workplanes?" & vbCrLf & vbCrLf & "Click Yes to hide all sketches and workplanes." & vbCrLf & "Click No to Show all sketches and worplanes.", vbYesNoCancel)
Select Case result
    Case vbYes
        Vis = False
    Case vbNo
        Vis = True
    Case vbCancel
        Exit Sub
End Select
'catch and skip errors
On Error Resume Next

Dim oSetch As PlanarSketch
Dim oWorkPlane As WorkPlane
Dim oDoc As Inventor.Document

'Iterate tru all referenced documents and change visibility
For Each oDoc In oAsmDoc.AllReferencedDocuments
    For Each oWorkPlane In oDoc.ComponentDefinition.WorkPlanes
    oWorkPlane.Visible = Vis
    Next
    'set work axis visibility
    For Each oWorkAxis In oDoc.ComponentDefinition.WorkAxes
    oWorkAxis.Visible = Vis
    Next
    'set work point visibility
    For Each oWorkPoint In oDoc.ComponentDefinition.WorkPoints
    oWorkPoint.Visible = Vis
    Next
    For Each oSketch In oDoc.ComponentDefinition.Sketches
    oSketch.Visible = Vis
    Next
Next

'change visibility from active assembly document
For Each oWorkPlane In oAsmDoc.ComponentDefinition.WorkPlanes
    oWorkPlane.Visible = Vis
    Next
    'set work axis visibility
    For Each oWorkAxis In oAsmDoc.ComponentDefinition.WorkAxes
    oWorkAxis.Visible = Vis
    Next
    'set work point visibility
    For Each oWorkPoint In oAsmDoc.ComponentDefinition.WorkPoints
    oWorkPoint.Visible = Vis
    Next
    For Each oSketch In oAsmDoc.ComponentDefinition.Sketches
    oSketch.Visible = Vis
    Next
    
ThisApplication.ActiveDocument.Update
End Sub

Private Sub HidePartComponents()

Dim oPartDoc As PartDocument
Set oPartDoc = ThisApplication.ActiveDocument
'get user input as True or False
Dim Vis As Boolean
Dim result
result = MsgBox("Hide all sketches and workplanes?" & vbCrLf & vbCrLf & "Click Yes to hide all sketches and workplanes." & vbCrLf & "Click No to Show all sketches and worplanes.", vbYesNoCancel)
Select Case result
    Case vbYes
        Vis = False
    Case vbNo
        Vis = True
    Case vbCancel
        Exit Sub
End Select

Dim oSetch As PlanarSketch
Dim oWorkPlane As WorkPlane
Dim oDoc As Inventor.Document
'change visibility from active part document
For Each oWorkPlane In oPartDoc.ComponentDefinition.WorkPlanes
    oWorkPlane.Visible = Vis
    Next
    'set work axis visibility
    For Each oWorkAxis In oPartDoc.ComponentDefinition.WorkAxes
    oWorkAxis.Visible = Vis
    Next
    'set work point visibility
    For Each oWorkPoint In oPartDoc.ComponentDefinition.WorkPoints
    oWorkPoint.Visible = Vis
    Next
    For Each oSketch In oPartDoc.ComponentDefinition.Sketches
    oSketch.Visible = Vis
    Next
ThisApplication.ActiveDocument.Update
End Sub

Working for me 

[NachoShaw]

Hi

thanks for the replies and hte code. The routine does create a very large lag (my assemblies are large) and also, it doesnt turn off the 2D sketches. Isnt there a similar function the check box that we tick to turn everything off?

i'll take a look 🙂

Cheers

[NachoShaw · Accepted solution]

Solution

Dim oDoc as Inventor.Document = _invApp.ActiveDocument
oDoc.ObjectVisibility.Sketches = False

Thanks

[GosponZ]

Nice stuff on this link http://www.kwikmcad.com/icode/macros/macros.aspx

bdw did you see pm?

[NachoShaw]

Hi

Yes i saw the PM :). The tools will be on the App store as soon as i get the time to get them completed. Drawing tool first hopefully within the next 2 months.

Cheers