Points on Surface and normal line creation 1

[DomKum]

Hi All,

I am trying to create macro with input as GS in which only Surfaces are there and output expected is to create a point which is CG of each surface and then create a normal to respective surface with respective point as input.

I need help in putting this macro in loop i mean point and line to be created for all the surfaces in the input GS.
When I try to run this macro its failing in LINE 41 WHICH I have highlighted in red color.

Thanks in advance for any suggestion or guidance.


Language="VBSCRIPT"

Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument

Set part1 = partDocument1.Part

Set hybridBodies1 = part1.HybridBodies

'Set hybridShapeFactory1 = part1.HybridShapeFactory

Set parameters1 = part1.Parameters

MsgBox "Select Geometrical set."

Dim oSelection ' 'As Selection
Dim InputObjectType(0)

Set oSelection = CATIA.ActiveDocument.Selection
oSelection.Clear
InputObjectType(0) = "HybridBody"
Status = oSelection.SelectElement2(InputObjectType, "Select Geometrical set.", True)



Set hybridShapeFactory1 = part1.HybridShapeFactory

Set parameters1 = part1.Parameters

Set hybridShapeSurfaceExplicit1 = parameters1.Item("Surface.679") 'this is one of the surfaces in my GS but I want for all the surfaces in GS

Set hybridBody1 = hybridBodies1.Add()

part1.UpdateObject hybridBody1

Set reference1 = part1.CreateReferenceFromObject(hybridShapeSurfaceExplicit1)

Set parameters2 = part1.Parameters

[highlight #CC0000]Set hybridShapePointExplicit1 = parameters2.Item("")[/highlight]

Set reference2 = part1.CreateReferenceFromObject(hybridShapePointExplicit1)

Set hybridShapeLineNormal1 = hybridShapeFactory1.AddNewLineNormal(reference1, reference2, 0.000000, 1000.000000, False)

hybridBody1.AppendHybridShape hybridShapeLineNormal1

part1.InWorkObject = hybridShapeLineNormal1

part1.Update

End Sub

 

[DomKum]

Finally I could able to create FOR LOOP with displaying the count.

Can any one help me to create point on surface since I am unable to find the correct syntax.
This will help me to go forward.

Language="VBSCRIPT"

Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument

Set part1 = partDocument1.Part

Set hybridBodies1 = part1.HybridBodies

Set hybridBody1 = hybridBodies1.Add()
Set hybridBody1 = CATIA.ActiveDocument.Part.InWorkObject

part1.UpdateObject hybridBody1

Dim InputObjectType(0)

Set oSelection = CATIA.ActiveDocument.Selection
oSelection.Clear
InputObjectType(0) = "HybridBody"
Status = oSelection.SelectElement2(InputObjectType, "Select Geometrical set.", True)

Dim iCount
Dim i 'As Integer

oSelection.Search "CATGmoSearch.Surface,sel"
iCount = oSelection.Count

For i =1 to iCount
msgbox ("number " & i)

Set hybridShapeFactory1 = part1.HybridShapeFactory

Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(0.807715, -0.589573, 0.000000)

Set parameters1 = part1.Parameters

Set hybridShapeSurfaceExplicit1 = parameters1.Item(i)

Set reference1 = part1.CreateReferenceFromObject(hybridShapeSurfaceExplicit1)


Set hybridShapePointOnSurface1 = hybridShapeFactory1.AddNewPointOnSurface(reference1, hybridShapeDirection1, 0.000000)

part1.InWorkObject = hybridShapePointOnSurface1

part1.Update

Next

End Sub

 

[Little Cthulhu]

Datum geometry should not be retrieved from Parameters collection.

In your case simply get it from selection as you've already searched for all surfaces:

Set hybridShapeSurfaceExplicit1 = oSelection.Item(i).Value

 

[DomKum]

Thank you for kind response.
The only good thing in this code is it can display the number of Surfaces in a selected GS.
However the point is not getting created.

Language="VBSCRIPT"

Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument

Set part1 = partDocument1.Part

Set hybridBodies1 = part1.HybridBodies

Set hybridBody1 = hybridBodies1.Add()
Set hybridBody1 = CATIA.ActiveDocument.Part.InWorkObject

part1.UpdateObject hybridBody1

Dim InputObjectType(0)

Set oSelection = CATIA.ActiveDocument.Selection
oSelection.Clear
InputObjectType(0) = "HybridBody"
Status = oSelection.SelectElement2(InputObjectType, "Select Geometrical set.", True)

Dim iCount
Dim i 'As Integer

oSelection.Search "CATGmoSearch.Surface,sel"
iCount = oSelection.Count

For i =1 to iCount

msgbox ("number " & i) '----> Display the number of surfaces selected in a GS

Set hybridShapeFactory1 = part1.HybridShapeFactory

Set hybridShapeSurfaceExplicit1 = oSelection.Item(i).Value

Set reference1 = part1.CreateReferenceFromObject(hybridShapeSurfaceExplicit1)

Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(0.807715, -0.589573, 0.000000)

Set hybridShapePointOnSurface1 = hybridShapeFactory1.AddNewPointOnSurface(reference1, hybridShapeDirection1, 0.000000)

part1.InWorkObject = hybridShapePointOnSurface1

part1.Update

Next

End Sub

 

[TudorM]

It creates a new geometrical set as well

 

[Little Cthulhu]

It does get created, you have to place new feature in a desired container (body or geometrical set) manually with AppendHybridShape:

Set hybridShapePointOnSurface1 = hybridShapeFactory1.AddNewPointOnSurface(reference1, hybridShapeDirection1, 0.000000)
hybridBody1.HybridShapes.AppendHybridShape hybridShapePointOnSurface1

I insist you download ferdo's great "Portable Script Center" and refer to it's samples.

 

[DomKum]

Mission accomplished.
Thank you Little Cthulhu for your patience and guidance.
Below is the MACRO for creating a point and Normal to surface line on input Surface in a GS.
Hope this will help new beginners like me.

'---------------------------------------
'This Macro is to create a point on Dead Surface
'in a selected Geometrical Set
'----------------------------------------
Language="VBSCRIPT"

Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument

Set part1 = partDocument1.Part

Set hybridBodies1 = part1.HybridBodies

'part1.UpdateObject hybridBody1

Dim InputObjectType(0)

msgbox ("Select the geometrical set")

Set oSelection = CATIA.ActiveDocument.Selection
oSelection.Clear
InputObjectType(0) = "HybridBody"
Status = oSelection.SelectElement2(InputObjectType, "Select Geometrical set.", True)

Set hybridBody1 = hybridBodies1.Add()
Set hybridBody1 = CATIA.ActiveDocument.Part.InWorkObject

Dim iCount
Dim i 'As Integer

oSelection.Search "CATGmoSearch.Surface,sel" '-----With this all the surfaces will be searched in a selected GS
iCount = oSelection.Count '-----Each selected item is counted

For i =1 to iCount
'----------------
'Below line msgbox can be made as comment. This line is only for displaying the
'total number of Surfaces available in a selected GS
'----------------

msgbox ("number " & i)

set hybridShapeFactory1 = part1.HybridShapeFactory

Set hybridShapeSurfaceExplicit1 = oSelection.Item(i).Value

Dim reference1 'As Reference

Set reference1 = part1.CreateReferenceFromObject(hybridShapeSurfaceExplicit1)

Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(0.5, 0.5, 0.000000)

Dim hybridShapePointOnSurface1 'As HybridShapePointOnSurface
Set hybridShapePointOnSurface1 = hybridShapeFactory1.AddNewPointOnSurface(reference1, hybridShapeDirection1, 0.000000)

hybridBody1.AppendHybridShape hybridShapePointOnSurface1

part1.InWorkObject = hybridShapePointOnSurface1

'Set reference2 = part1.CreateReferenceFromObject(hybridShapePointCoord1)

Set reference2 = hybridShapePointOnSurface1 '---->Created point is taken as reference to create a line

Set hybridShapeLineNormal1 = hybridShapeFactory1.AddNewLineNormal(reference1, reference2, 0.000000, 100.000000, False)

hybridBody1.AppendHybridShape hybridShapeLineNormal1

part1.InWorkObject = hybridShapeLineNormal1

part1.Update

Next

End Sub

 

[DomKum]

MACRO is updated to rename the point and line created with parent surface name.
Any suggestion to improvements this will be helpful to me as well new beginners.
'---------------------------------------
'This Macro is to create a point on Dead Surface
'in a selected Geometrical Set
'----------------------------------------
Language="VBSCRIPT"

Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument

Set part1 = partDocument1.Part

Set hybridBodies1 = part1.HybridBodies

'part1.UpdateObject hybridBody1

Dim InputObjectType(0)

msgbox ("Select the geometrical set")

Set oSelection = CATIA.ActiveDocument.Selection
oSelection.Clear
InputObjectType(0) = "HybridBody"
Status = oSelection.SelectElement2(InputObjectType, "Select Geometrical set.", True)

Set hybridBody1 = hybridBodies1.Add()
Set hybridBody1 = CATIA.ActiveDocument.Part.InWorkObject

Dim iCount
Dim i 'As Integer

oSelection.Search "CATGmoSearch.Surface,sel" '-----With this all the surfaces will be searched
iCount = oSelection.Count '-----Each selected item is counted

For i =1 to iCount
'----------------
'Below line msgbox can be made as comment. This line is only for displaying the
'total number of Surfaces available in a selected GS
'----------------

'msgbox ("number " & i) '--- It will display only count but not the name of item selected

'msgbox (i) '-----this will only display the number or count

'-----------With the statement as below each item name in the selected GS will be displayed
Set USel = CATIA.ActiveDocument.Selection
MsgBox(USel.Item(i).Value.Name)
'--------------- 09-Macro_to_display_selected_items.catvbs - reference macro for this statement

set hybridShapeFactory1 = part1.HybridShapeFactory

Set hybridShapeSurfaceExplicit1 = oSelection.Item(i).Value

Dim reference1 'As Reference

Set reference1 = part1.CreateReferenceFromObject(hybridShapeSurfaceExplicit1)

Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(0.5, 0.5, 0.000000)

Dim hybridShapePointOnSurface1 'As HybridShapePointOnSurface
Set hybridShapePointOnSurface1 = hybridShapeFactory1.AddNewPointOnSurface(reference1, hybridShapeDirection1, 0.000000)

hybridBody1.AppendHybridShape hybridShapePointOnSurface1

part1.InWorkObject = hybridShapePointOnSurface1


'----> Below line will rename the new point created with sufix as POINT & PARENT SURFACE NAME
hybridShapePointOnSurface1.name = "Point for - " & USel.Item(i).Value.Name

Set reference2 = hybridShapePointOnSurface1 '---->Created point is taken as reference to create a line

Set hybridShapeLineNormal1 = hybridShapeFactory1.AddNewLineNormal(reference1, reference2, 0.000000, 50.000000, False)

hybridBody1.AppendHybridShape hybridShapeLineNormal1

part1.InWorkObject = hybridShapeLineNormal1

'---->Below line will rename the new LINE created with sufix as LINE & PARENT SURFACE NAME
hybridShapeLineNormal1.name = "Line for - " & USel.Item(i).Value.Name


part1.Update

Next

End Sub