Catia select a feature from a specific instance in an assembly

Question

Lets say I have an assembly like this:

MainProduct:
-Product1 (Instance of Part1)
-Product2 (Instance of Part2)
-Product3 (Instance of Part2)
-Product4 (Instance of Part3)
...

Now, I want to copy/paste a feature from Product3 into another one.
But I run into problems when selecting the feature programmatically, because there are 2 instances of the part of that feature.

I can't control which feature will be selected by CATIA.ActiveDocument.Selection.Add(myExtractReference)
Catia always selects the feature from Product2 instead of the feature from Product3. So the position of the pasted feature will be wrong!

Does anybody know this problem and has a solution to it?

Edit: The feature reference which I want to copy already exists as a variable because it was newly created (an extract of selected geometry)

Answer 1

I could get help else where. Still want to share my solution. It's written in Python but in VBA its almost the same. The clue is to access CATIA.Selection.Item(1).LeafProduct in order to know where the initial selection was made.

import win32com.client
import pycatia

CATIA = win32com.client.dynamic.DumbDispatch('CATIA.Application')
c_doc = CATIA.ActiveDocument
c_sel = c_doc.Selection
c_prod   = c_doc.Product

# New part where the feature should be pasted
new_prod = c_prod.Products.AddNewComponent("Part", "")
new_part_doc = new_prod.ReferenceProduct.Parent

# from user selection
sel_obj = c_sel.Item(1).Value

sel_prod_by_user = c_sel.Item(1).LeafProduct  #  reference to the actual product where the selection was made
doc_from_sel = sel_prod_by_user.ReferenceProduct.Parent  # part doc from selection
hb = doc_from_sel.Part.HybridBodies.Add()  # new hybrid body for the extract. will be deleted later on
extract = doc_from_sel.Part.HybridShapeFactory.AddNewExtract(sel_obj)
hb.AppendHybridShape(extract)
doc_from_sel.Part.Update()

# Add the extract to the selection and copy it
c_sel.Clear()
c_sel.Add(extract)
sel_prod_by_catia = c_sel.Item(1).LeafProduct  # reference to the product where Catia makes the selection
c_sel_copy()  # will call Selection.Copy from VBA. Buggy in Python.

# Paste the extract into the new part in a new hybrid body
c_sel.Clear()
new_hb = new_part_doc.Part.HybridBodies.Item(1)
c_sel.Add(new_hb)
c_sel.PasteSpecial("CATPrtResultWithOutLink")
new_part_doc.Part.Update()
new_extract = new_hb.HybridShapes.Item(new_hb.HybridShapes.Count)

# Redo changes in the part, where the selection was made
c_sel.Clear()
c_sel.Add(hb)
c_sel.Delete()

# Create axis systems from Position object of sel_prd_by_user and sel_prd_by_catia
prod_list = [sel_prod_by_user, sel_prod_by_catia]
axs_list = []
for prod in prod_list:
    pc_pos = pycatia.in_interfaces.position.Position(prod.Position) # conversion to pycata's Position object, necessary
                                                                    # in order to use Position.GetComponents
    ax_comp = pc_pos.get_components()
    axs = new_part_doc.Part.AxisSystems.Add()
    axs.PutOrigin(ax_comp[9:12])
    axs.PutXAxis(ax_comp[0:3])
    axs.PutYAxis(ax_comp[3:6])
    axs.PutZAxis(ax_comp[6:9])
    axs_list.append(axs)
    new_part_doc.Part.Update()

# Translate the extract from axis system derived from sel_prd_by_catia to sel_prd_by_user
extract_ref = new_part_doc.Part.CreateReferenceFromObject(new_extract)
tgt_ax_ref = new_part_doc.Part.CreateReferenceFromObject(axs_list[0])
ref_ax_ref = new_part_doc.Part.CreateReferenceFromObject(axs_list[1])
new_extract_translated = new_part_doc.Part.HybridShapeFactory.AddNewAxisToAxis(extract_ref, ref_ax_ref, tgt_ax_ref)
new_hb.AppendHybridShape(new_extract_translated)
new_part_doc.Part.Update()