iLogic Solid Body Visibility

Issue:

You want to be able to control the visibility of Solid Bodies in a Multi Body part file using  your iLogic rule.

Solution:

Here is a quick example that demonstrates several options to toggle the visibility of solid bodies on and off.

'define the document as a component definition

Dim oCompDef as ComponentDefinition

oCompDef = ThisDoc.Document.ComponentDefinition

'define the solidbody

Dim oBody as SurfaceBody

'add each solid body name to a list

Dim MyArrayList As New ArrayList

i = 1

For Each SurfaceBody in oCompDef.SurfaceBodies

oBody = oCompDef.SurfaceBodies.Item(i)

MyArrayList.add(oBody.Name)

i = i +1

Next

'add Show and Hide all options to the list

MyArrayList.add(" *Show All")

MyArrayList.add(" *Hide All")

'present the user with the list and record the selection

sBody  = InputListBox("Select a Solid Body to Toggle Visibility.", _

MyArrayList, "", "iLogic", "List of Solid Bodies")

'toggle all on or all off, if those options were selected

If sBody = " *Show All" Then

          i = 1

          For Each SurfaceBody in oCompDef.SurfaceBodies

            oBody = oCompDef.SurfaceBodies.Item(i)

          oBody.Visible = True

            i = i +1

          Next

ElseIf sBody = " *Hide All"

            i = 1

          For Each SurfaceBody in oCompDef.SurfaceBodies

            oBody = oCompDef.SurfaceBodies.Item(i)

          oBody.Visible = False

            i = i +1

          Next

End If

'compare the user selection to the solid body names

'and toggle the visibility for the one the matches (if any)

i = 1

For Each SurfaceBody in oCompDef.SurfaceBodies

oBody = oCompDef.SurfaceBodies.Item(i)

If sBody = oBody.Name Then

          If oBody.Visible = False Then

          oBody.Visible = True

            Else

          oBody.Visible = False

            End If

End If

MyArrayList.add(oBody.Name)

i = i +1

Next