Macro To Extract A Surface In Space (& Understanding Selection Object)

[dctene2]

Hello, I've hit a wall writing a macro and am humbly asking for some assistance.

Context:

I have a CATProduct composed of a single CATPart that represents an assembly of several flat panels. The CATPart contains several Part Bodies that each represent a single panel in the assembly. To describe the assembly, imagine a bookshelf without any backing. So essentially, it is a box frame with panels inside that represent the shelves.​

Problem:

I want to recreate the assembly but with each panel being its own CATPart within the same Product.​

Proposed Solution:

I've created a Seed Model CATPart that represents a single panel. This Seed Model is a Pad whose sketch is a projection of the boundary of an isolated planar surface. The isolated surface is in a Geometrical Set labeled "External References". For the purposes of simplicity, the planar surface is a simple rectangle.

The macro I am writing will insert a "New From" version of the Seed Model into the Product and prompt the user to select a planar surface in space. The intent is to select a face on the original multi-body CATPart that will then be extracted into the Seed Part and replace the isolated surface. As a result, the Pad is then updated to represent one of the panels in space.​

Issue:

Establishing the selected surface as a usable object in the Macro code​

The issue, I believe, is caused by the selected Planar Face being a feature of a CATPart that is not the active part (The Seed Model is the active part in this example). I am not sure how to get this Planar Face feature (i.e. the selected surface) into my new part.

Note that if I select a surface on the active part, it creates the Extract with no issue.

Below is the part of the code where I try to select a planar surface to be extracted into the New From part. It results in an empty Extract in the tree but with an error:

Extract.2 | Invalid, empty or missing input element. One mandatory input element is invalid, empty, or missing. There is no solution for this operation.​

Sub CATMain()
[indent]Dim oDoc As Document
Set oDoc = CATIA.ActiveDocument

Dim oSelection
Set oSelection = oDoc.Selection

Dim arraySelection(0)
arraySelection(0) = "Planar Face"

dim Status
Status = oSelection.SelectElement2(arraySelection, "Select a Planar Face...", False)

If (InStr(1, Status, "Normal") > 0 Then
[indent]Dim selectedObject
Set selectedObject = oSelection.Item(1).Reference

Dim partDoc1 As PartDocument
Set partDoc1 = oDoc.Application.Documents.Item("Seed_Model.CATPart")

Dim part1 As Part
Set part1 = partDoc1.Part

Dim hsf1 As HybridShapeFactory
Set hsf1 = part1.HybridShapeFactory

Dim hse1 As HybridShapeExtract
Set hse1 = hsf1.AddNewExtract(selectedObject)

hse1.PropagationType = 3
hse1.ComplementaryExtract = False
hse1.IsFederated = False

Dim hbs1 As HybridBodies
Set hbs1 = part1.HybridBodies

Dim hb1 As HybridBody
Set hb1 = hbs1.Item("External References")

hb1.AppendHybridShape hse1

part1.InWorkObject = hse1

part1.Update
[/indent]
End If

oSelection.Clear
[/indent]
End Sub

Any help or insight would be greatly appreciated. Thank you everyone for your time.

 

[LWolf]

I think you should create the extract in your Assembly CATPart. Then copy-paste the selection into the new part.

regards,
LWolf

 

[Little Cthulhu]

Solved exactly the same problem couple of months ago. Follow LWolf's advice and create extract in the source part.

 

[dctene2]

Solved! I created the extract within the source part, copied it, pasted special "As Result" in the target part, then deleted the extract from the source part. Thank you!