iLogic: Delete All Sick Assembly Constraints

Issue:
You sometimes end up with a large number of broken (sick) assembly constraints, due to a particular workflow (such as swapping out a base component). You know why this is happening and don't mind fixing the assembly, but you wish there was a way to delete all of the sick assembly constraints at once, so you can re-constrain the assembly without having to be bothered by the alerts.

Solution:
Here is a quick iLogic snippet to help with this:

* A special thanks to Brendan Henderson for letting me know about a coding error I had when I first posted this. Check out Brendan's own blog at: http://www.blh.com.au/#/blog/4572268941             

Dim oAssDoc As AssemblyDocument

oAssDoc = ThisApplication.ActiveDocument

Dim oConstraint As AssemblyConstraint

RUSure = MessageBox.Show _

("Are you sure you want to Delete all sick constraints?",  _

"iLogic",MessageBoxButtons.YesNo)

If RUSure = vbNo Then

Return

Else

          i = 0

          For Each oConstraint In oAssDoc.ComponentDefinition.Constraints

            If oConstraint.HealthStatus <> oConstraint.HealthStatus.kUpToDateHealth And _

            oConstraint.HealthStatus <> oConstraint.HealthStatus.kSuppressedHealth Then

          oConstraint.Delete

            i = i + 1

          End If

          Next

End If

MessageBox.Show(" A total of "&  i & " constraints were deleted.", "iLogic")

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

iLogic Replace Derived Reference

Issue:
You wish there was an option in parts created from derived components to replace the derived component.

Solution:
Here is a quick iLogic rule that will allow you to browse for a new file with which you can replace the derived reference of an existing derived component.

UPDATE:
A reader recently pointed out a limitation of this iLogic snippet stemming from its use of the API's FileDescriptor.ReplaceReference method. This method requires that the file being replaced and
the replacement file must share ancestry, that is to say that one file was saved from the other file, or both files were saved from the same "parent" file. Simply being aware of this will result in predictable results, but if you were attempting to use this snippet to replace two completely different files you might not have been able to get this to work.

Thanks to Peter for taking the time to bring my attention to this!

Dim oDoc as Document

oDoc = ThisDoc.Document

Dim oRefFile As FileDescriptor

Dim oOrigRefName As Object     

For Each oRefFile In oDoc.file.ReferencedFileDescriptors

'get the full file path to the original internal references

oOrigRefName = oRefFile.FullFileName

'present a File Selection dialog

Dim oFileDlg As inventor.FileDialog = Nothing

InventorVb.Application.CreateFileDialog(oFileDlg)

oFileDlg.InitialDirectory = oOrigRefName

oFileDlg.CancelError = True

On Error Resume Next

oFileDlg.ShowOpen()

If Err.Number <> 0 Then

Return

ElseIf oFileDlg.FileName <> "" Then

selectedfile = oFileDlg.FileName

End if

‘replace the reference

oRefFile.ReplaceReference (selectedfile)     

InventorVb.DocumentUpdate()

oOrigRefName = “”                                        

Next

iLogicVb.UpdateWhenDone = True