How to get part position

[AnJanson]

Hi,

I have a quiet simple question. How can I get the xyz position of a part/ComponentOccurrence in an assembly.

I did some tests and found the Transformation.Translation vector.

But the values for x, y and z are only one tenth of the real value (e.g. x is 2222, but the vector.x property gives me 222.2).

My assembly untis are in mm.

Regards Andreas

[bshbsh · Accepted solution]

inventor always uses centimeters internally. you need to convert it to the units you need (eg. the model units). it's simple in the case of cm-mm, but there are built-in unit conversion functions as well.

[MechMachineMan · Accepted solution]

Sample:

Sub Main()

On Error Goto Handler:
	Dim oDoc As AssemblyDocument
	oDoc = ThisApplication.ActiveDocument
	
	If oDoc Is Nothing Then
        Exit Sub
    End If
    
    'Ensure you are at the right point to select objects.
    Select Case True
        Case Not oDoc.ActivatedObject Is Nothing
            If oDoc.ActivatedObject.Type = ObjectTypeEnum.kDocumentObject Then
                oDoc = oDoc.ActivatedObject
            Else
                MsgBox ("Invalid active object")
                Exit Sub
            End If
        Case oDoc.ActivatedObject Is Nothing
            'Continue without revising anything
        Case Else
            MsgBox ("Invalid Activated Object!")
    End Select
On Error Goto 0

    Dim oSS As SelectSet
    oSS = oDoc.SelectSet
      If oSS.Count >= 1

		Call ProcessBulkLocations(oSS)
      End If
	
	
	Exit Sub
Handler:
	MsgBox("Doc Not an Assembly!")
End Sub

Sub ProcessBulkLocations(oSS As SelectSet)
    For Each oItem In oSS
        If oItem.Type = ObjectTypeEnum.kComponentOccurrenceObject Then

           	Call GetOccOrigin(oItem)
        End If
    Next
End Sub

Sub GetOccOrigin(oOcc As ComponentOccurrence)

	Dim oUOM As UnitsOfMeasure
	oUOM = ThisApplication.ActiveDocument.UnitsOfMeasure

	' Get the current transformation matrix from the occurrence.
   	Dim oTransform As Matrix
   	oTransform = oOcc.Transformation

	Dim oOriginLocation As Vector
	oOriginLocation = oTransform.Translation

	ptX = oUOM.ConvertUnits(oOriginLocation.X, "cm", "in")
	ptY = oUOM.ConvertUnits(oOriginLocation.Y, "cm", "in")
	ptZ = oUOM.ConvertUnits(oOriginLocation.Z, "cm", "in")

	MsgBox(ptX & vbLf & ptY & vbLf & ptZ)
   	' Move the occurrence honoring any existing constraints.
   	''oTransform.SetTranslation ThisApplication.TransientGeometry.CreateVector(2, 2, 3)
   	''oOccurrence.Transformation = oTransform

   	' Move the occurrence ignoring any constraints.
   	'Anything that causes the assembly to recompute will cause the
   	'occurrence to reposition itself to honor the constraints.
   	''oTransform.SetTranslation ThisApplication.TransientGeometry.CreateVector(3, 4, 5)
   	''Call oOccurrence.SetTransformWithoutConstraints(oTransform)

End Sub

[AnJanson]

Thank you Justin for the snippet and thank you János for the information, that Inventor always uses cm internally. 

Regards Andreas

[amichaudJ6E3R]

Hi,

I think I have a similar request. I have this assembly with a form where the user can choose between having 1, 2 or 3 of the same part (but 3 different occurrences)

Those parts are constrained in 2 axis, but can move freely in the third axis. I'd like to be able to capture, or get, the current position of those parts somehow and put that one coordinate in a parameter that can be exported into a XML file.

So I made this dummy assembly that recreates exactly the problem that I have, just not the real thing. There's a form in there that should open with the document. In that form you have the option to load 1, 2 or 3 parts, and the ability to save the parameters to a XML .

But right now, I really don't know where to start to capture that position. And I'm a beginner in VB and iLogic so that code above really makes very little sense to me. My plan B would be to constrain those parts to some plane and have a slider change the offset, but at first, I'd like to see if there's a more elegant way of doing this. Also, I like that very intuitive way of just grabbing the part and positioning it manually (without having to rely on a slider), I'd like to retain that.

I guess I just need someone to either, explain that snippet above, or send me in some direction to help me start.