Catia: 2D Points to 3D Points

Question

I have a Catia part where I have a few sketches on different planes. I need to be able to convert these sketches into 3D points which I copy to a new part document. I have tried to use the Search and Selection commands in VB script in order to use a macro to pick up all the 2D points in my sketch and convert them to 3D points but to no avail.

Sub CATMain()

Set oSel = CATIA.ActiveDocument.Selection

strArray(0)=”Part”

Msgbox “Please select parts to join.”

sStatus = oSel.SelectElement3(strArray, “Select parts”, False, CATMultiSelTriggWhenUserValidatesSelection, false)

iCount = oSel.Count

For i= 1 to iCount

Set myObject2 = oSel.Item(i).value

oSel.Search “Name=Point,sel”

ReDim copies(iCount)

For k=1 to iCount
Set copies(k)=oSel.Item(k).Value
oSel.Add copies(k)
oSel.Copy


Next ‘k
Next ‘i


Set part2 = CATIA.Documents.Add(“CATPart”)

part2.Product.PartNumber = “My New Part”

Dim GSet1 As HybridBody
Set GSet1 = part2.Part.HybridBodies.Item(1)
GSet1.Name = “My Geometry”

Set partDocument2= CATIA.ActiveDocument
Dim ActSel As Selection
Set ActSel=partDocument2.Selection
ActSel.Add GSet1

ActSel.PasteSpecial(“CATPrtResultWithOutLink” )


ActSel.Clear

End Sub

If the answer is good for you please mark it as correct. – C R Johnson Jan 14 '19 at 20:44 — C R Johnson, Jan 14 '19 at 20:44

score 0 · Accepted Answer · answered Jan 10 '19 at 15:36

You have to disassemble the sketch to get at the points as something you can copy

The disassemble command is exposed in VB via the HybridShapeFactory.AddNewDatums method.

Option Explicit


Sub CATMain()


Dim oPart As part
Set oPart = CATIA.ActiveDocument.part

Dim oHSF As HybridShapeFactory
Set oHSF = oPart.HybridShapeFactory

Dim sx As Sketch
Set sx = oPart.HybridBodies.item("Geometrical Set.1").HybridSketches.item("Sketch.1")


'make a temporary body
Dim targetGS As HybridBody
Set targetGS = oPart.HybridBodies.add
targetGS.name = "TMP_BODY___DELETE_ME"

'create a datum curve from the sketch
Dim sxRef As Reference
Set sxRef = oPart.CreateReferenceFromObject(sx)

'make a zero-translate from the sketch
'This is required because AddNewDatums functions needs a HybridShape feature
Dim oZero As HybridShapeTranslate
Set oZero = oHSF.AddNewTranslate(sxRef, oHSF.AddNewDirectionByCoord(0#, 0#, 1#), 0#)

Call targetGS.AppendHybridShape(oZero)
Call oPart.UpdateObject(oZero)

'now do the disassembly    
Dim oZeroRef As Reference
Set oZeroRef = oPart.CreateReferenceFromObject(oZero)

'un-datum the curve by making a zero translate

    Dim domains() As Variant
    domains = oHSF.AddNewDatums(oZeroRef)

    Dim i As Integer
    For i = 0 To UBound(domains)
        Call targetGS.AppendHybridShape(domains(i))
    Next

    Call oPart.Update


'now we can copy the resulting points...

    Dim oSel As Selection
    Set oSel = CATIA.ActiveDocument.Selection

    Call oSel.add(targetGS)
    Call oSel.Search("'Generative Shape Design'.Point,sel")


    'copy paste into the new part

  MsgBox ("There are " & oSel.count & " points ready to copy")
    < YOUR COPY PASTE CODE GOES HERE>
    'delete the temporary geo set

    Call oHSF.DeleteObjectForDatum(oPart.CreateReferenceFromObject(targetGS))

End Sub

Catia: 2D Points to 3D Points

1 Answers1