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Fabric pattern completed via powerCopy Automation. Method is the following three steps →
STEP1. BeginInstanceFactory: to initialize the InstanceFactory with the reference and the document where it is stored. This step must be called once at the beginning whatever the number of instantiations are done.
STEP2. It is composed of five methods that must be called in the order. This set of five methods can be called in a loop in order to make several instantiations.
a. The method BeginInstantiate: to initialize all data of the reference.
b. The method PutInputData: to set a value to any input.
c. The method GetParameter: to retrieve published parameter.
d. The method Instantiate: to recreate the reference.
e. The method EndInstantiate: to indicate the instantiation is done.
STEP3. EndInstantiateFactory: to end instantiation and cleaning the InstanceFactory. When doing several instantiations in a loop, this step must be called just once at the end of all instantiations.

Some useful CATIA vba samples, since v5Automation was overwhelming for newbies like me.
'opening statement /intersectionPt
'---------------------------------------
Dim partDocument1 As PartDocument
Set partDocument1 = CATIA.ActiveDocument
Dim part1 As Part
Set part1 = partDocument1.Part
'add geom set here
Dim hybridBody1 As HybridBody
Set hybridBody1 = part1.HybridBodies.Add()
hybridBody1.Name = "Geometrical Set.New"
part1.Update
'used geom set
Dim hybridBody2 As HybridBody
Set hybridBody2 = part1.HybridBodies.Item("Geometrical Set.1")
Dim hybridBody3 As HybridBody
Set hybridBody3 = part1.HybridBodies.Item("Geometrical Set.2").HybridBodies.Item("Multi Output.1 (Intersect)")
'---------------------------------------
'selection set /color
'---------------------------------------
Dim colorCount
colorCount = hybridBody1.HybridShapes.Count
For i = 1 To colorCount
Call partDocument1.Selection.Add(hybridBody1.HybridShapes.Item(i))
Dim visProperties1 As VisPropertySet
Set visProperties1 = partDocument1.Selection.VisProperties
visProperties1.SetRealColor 255, 255, 0, 1 'yellow(255,255,0)
partDocument1.Selection.Clear
Next i
'---------------------------------------
'measurable, parameter, formula
'---------------------------------------
'create line WITHOUT parameter first
Dim line1 As HybridShapeLineAngle
Set line1 = part1.HybridShapeFactory.AddNewLineAngle( , , , , , , , )
Dim angleFormula01 As Formula
Set angleFormula01 = part1.relations.CreateFormula( , , line1.Angle, )
hybridBody1.AppendHybridShape line1
part1.InWorkObject = line1
Dim TheMeasurable01 As Measurable
Set TheMeasurable01 = CATIA.ActiveDocument.GetWorkbench("SPAWorkbench").GetMeasurable( )
Dim lineMeasurable01 As Double
lineMeasurable01 = TheMeasurable01.Length
Dim MeasurableRealStOff01 As RealParam
Set MeasurableRealStOff01 = part1.Parameters.CreateReal("Real.measurable stOff", lineMeasurable01)
Dim MeasurableRealEdOff01 As RealParam
Set MeasurableRealEdOff01 = part1.Parameters.CreateReal("Real.measurable edOff", lineMeasurable01)
Dim lengthFormula011 As Formula
Set lengthFormula011 = part1.relations.CreateFormula( , , line1.BeginOffset, )
Dim lengthFormula012 As Formula
Set lengthFormula012 = part1.relations.CreateFormula( , , line1.EndOffset, )
'---------------------------------------

Finally got hands on CATIA scripting. Most confusing thing about CATIA vba is the tree structure. Within Part Document only, CATIA has the following structure.
+-- PartDocument
+---- Part
+------ HybridShapeFactory
+-------- HybridBodies
+---------- HybridBody
+------------ HybridShapes
+-------------- HybridShapeAnd also, since CATIA has multiple ways to create a geometry,
"Dim ...... As ......" lines get a little tricky. Point Geometry for example, has 9 types including intersection point.
HybridShapePointBetween
HybridShapePointCenter
HybridShapePointCoord
HybridShapePointExplicit
HybridShapePointOnCurve
HybridShapePointOnPlane
HybridShapePointOnSurface
HybridShapePointTangent
HybridShapeInterSection
'Module h_planeM (THIS IS ONE MODULE ONLY !!!)
Option Explicit
'Author: YukiukiH
'Date: 10/18/2008
'compatibility: CATIA V5R18
'----------------------------------------------------------------------------------------------
Sub CATMain()
'opening statement
Dim partDocument1 As PartDocument
Set partDocument1 = CATIA.ActiveDocument
Dim part1 As Part
Set part1 = partDocument1.Part
'add geom set here
Dim hybridBody1 As HybridBody
Set hybridBody1 = part1.HybridBodies.Add()
hybridBody1.Name = "D_planeM"
part1.Update
'useg geom set
Dim hybridBody2 As HybridBody
Set hybridBody2 = part1.HybridBodies.Item("D_MidL")
Dim hybridBody3 As HybridBody
Set hybridBody3 = part1.HybridBodies.Item("D_normalM")
Dim i As Integer
Dim j As Integer
j = 0
Dim k As Integer
'Loop
'----------------------------------------------------------------------------------------------
'----------------------------------------------------------------------------------------------
Dim lineCount As Integer
lineCount = hybridBody2.HybridShapes.Count
For i = 1 To lineCount Step 9
'input
Dim line01 As HybridShapeLinePtPt
Set line01 = hybridBody2.HybridShapes.Item(i)
Dim lineNormal01 As HybridShapeLineNormal
Set lineNormal01 = hybridBody3.HybridShapes.Item(i + j)
'output
Dim plane01 As HybridShapePlane2Lines
Set plane01 = part1.HybridShapeFactory.AddNewPlane2Lines(line01, lineNormal01)
hybridBody1.AppendHybridShape plane01
part1.InWorkObject = plane01
'---------------------------------------
For k = 1 To 8
'input
Set line01 = hybridBody2.HybridShapes.Item(i + k)
Set lineNormal01 = hybridBody3.HybridShapes.Item(i + j + k)
'output
Set plane01 = part1.HybridShapeFactory.AddNewPlane2Lines(line01, lineNormal01)
hybridBody1.AppendHybridShape plane01
part1.InWorkObject = plane01
Next k
'---------------------------------------
j = j + 1
Next i
'----------------------------------------------------------------------------------------------
'----------------------------------------------------------------------------------------------
part1.Update 'has to be before SetRealColor
'color
'---------------------------------------
Dim colorCount
colorCount = hybridBody1.HybridShapes.Count
For i = 1 To colorCount
Call partDocument1.Selection.Add(hybridBody1.HybridShapes.Item(i))
Dim visProperties1 As VisPropertySet
Set visProperties1 = partDocument1.Selection.VisProperties
visProperties1.SetRealColor 0, 0, 0, 1 'blk(0, 0, 0)
partDocument1.Selection.Clear
Next i
'---------------------------------------
End Sub