Create constraint with ilogic in Inventor 2018

[Anonymous]

Good day,

Does anyone know how to create a mate constraint with ilogic in 2018 (I know that inventor 2019 has the new ilogic features that makes this much easier.)

I would like to constrain the XY workplane of one part//assembly to the XY workplane of another part/assembly.

Please help......

Thanks

[mcgyvr]

Here is an example from the API help samples..

    Dim oAsmCompDef As AssemblyComponentDefinition
    oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition

    ' Get references to the two occurrences to constrain.
    ' This arbitrarily gets the first and second occurrence.
    Dim oOcc1 As ComponentOccurrence
    oOcc1 = oAsmCompDef.Occurrences.Item(1)

    Dim oOcc2 As ComponentOccurrence
    oOcc2 = oAsmCompDef.Occurrences.Item(2)

    ' Get the XY plane from each occurrence.  This goes to the
    ' component definition of the part to get this information.
    ' This is the same as accessing the part document directly.
    ' The work plane obtained is in the context of the part,
    ' not the assembly.
    Dim oPartPlane1 As WorkPlane
    oPartPlane1 = oOcc1.Definition.WorkPlanes.Item(3)

    Dim oPartPlane2 As WorkPlane
    oPartPlane2 = oOcc2.Definition.WorkPlanes.Item(3)

    ' Because we need the work plane in the context of the assembly
    ' we need to create proxies for the work planes.  The proxies
    ' represent the work planes in the context of the assembly.
    Dim oAsmPlane1 As WorkPlaneProxy
    Call oOcc1.CreateGeometryProxy(oPartPlane1, oAsmPlane1)

    Dim oAsmPlane2 As WorkPlaneProxy
    Call oOcc2.CreateGeometryProxy(oPartPlane2, oAsmPlane2)

    ' Create the constraint using the work plane proxies.
    Call oAsmCompDef.Constraints.AddMateConstraint(oAsmPlane1, oAsmPlane2, 0)