Adding WorkPlane With Refrence to Face Using API C#

[hariharanhZXJ8L]

Hello Guys,

I am facing the Problem on Creating Work Plane on Assembly with reference to Face Object. 

can you please someone to help me to resolve the Issue ?

Here is my code :

WorkPlanes oPlanes = docDef.WorkPlanes
Face oFace = InventorApp.CommandManager.Pick(SelectionFilterEnum.kAllPlanarEntities, "Please Select the Face for - AssyRefRight");
WorkPlane plane = oPlanes.AddByPlaneAndOffset(oFace, 3);
plane.AutoResize = true;
plane.Name = "AssyRefRight";

Thanks

HARI

[vpeuvion]

Hello, what is your problem? The code looks correct to me.

I tested it quickly on iLogic and it works.

Sub main
    Dim oDoc As PartDocument = ThisApplication.ActiveDocument
    Dim docDef As PartComponentDefinition = oDoc.ComponentDefinition
    Dim oPlanes As WorkPlanes = docDef.WorkPlanes
    Dim oFace As Face = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAllPlanarEntities, "Please Select the Face for - AssyRefRight")
    Dim plane As WorkPlane = oPlanes.AddByPlaneAndOffset(oFace, 3)
    plane.AutoResize = True
    plane.Name = "AssyRefRight"
End Sub

Vincent.

[hariharanhZXJ8L]

For Part Doc It seems Working Good, I need to create plane in Assembly Doc.
It seems "AddByPlaneAndOffset" Is not working, do you have any other solution to create Work Planes in Assembly with reference to Face ?

[vpeuvion]

Sorry, I hadn't seen that your question was about assemblies. AddByPlaneAndOffset does not work for assemblies. This post should be able to help you.

https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/create-work-planes-in-assembly-ilogi...

Vincent.

[vpeuvion]

This should work for your case (tested on iLogic):

Sub Main
    Dim oAsmDoc As AssemblyDocument = ThisApplication.ActiveDocument
    Dim oAsmCompDef As AssemblyComponentDefinition = oAsmDoc.ComponentDefinition
	Dim oFace As FaceProxy = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAllPlanarEntities, "Please Select the Face for - AssyRefRight")
	Dim oWPlane As WorkPlane
	oWPlane = AddWorkPlaneInAssemblyOffset(oFace, 3)
	oWPlane.Name = "AssyRefRight"
End Sub

Function AddWorkPlaneInAssemblyOffset(oFace As Object, oOffset As Double) As WorkPlane
	Dim uOM As UnitsOfMeasure = ThisDoc.Document.UnitsOfMeasure
	Dim oAsm As AssemblyDocument = ThisApplication.ActiveDocument
	Dim oDef As AssemblyComponentDefinition = oAsm.ComponentDefinition
	Dim oOriginPnt As Point
	Dim oXaxis As UnitVector
	Dim oYaxis As UnitVector
	oOriginPnt = ThisApplication.TransientGeometry.CreatePoint(0#, 0#, 0#)
	oXaxis = ThisApplication.TransientGeometry.CreateUnitVector(1#, 0#, 0#)
	oYaxis = ThisApplication.TransientGeometry.CreateUnitVector(0#, 1#, 0#)
	Dim oPlane As WorkPlane = oDef.WorkPlanes.AddFixed(oOriginPnt, oXaxis, oYaxis)
	oPlane.AutoResize = True
	oDef.Constraints.AddFlushConstraint(oFace, oPlane, uOM.ConvertUnits(oOffset, uOM.LengthUnits, UnitsTypeEnum.kDatabaseLengthUnits))
	oPlane.AutoResize = False
	Return oPlane
End Function

Vincent.

[hariharanhZXJ8L]

how do you decide the unit vector direction ?

In your Example you have created the plane normal to XY direction

	oXaxis = ThisApplication.TransientGeometry.CreateUnitVector(1#, 0#, 0#)
	oYaxis = ThisApplication.TransientGeometry.CreateUnitVector(0#, 1#, 0#)

what if I select the face  normal to YZ ?

In this case the output is not good.

Thanks

HARI

[vpeuvion · Accepted solution]

Hi.
Have you tested the code on iLogic?
The plane is still created relative to the XY plane but is repositioned by the constraint that is applied to it next.
I did some tests on my side, the plane created is parallel to the selected face every time.

Vincent.