parameter + Formula + relations

[DomKum]

Hi Experts
May I request for help to correct this issue.
Trying to create a sphere with exiting points. Requirement is to create a sphere with parameter. I followed your youtube video but not able to fix the problem.
Not able to create formula to connect to radius of sphere.

Language=”VBSCRIPT”
‘ * * * * * * * * * * * * *
‘This MACRO is to create a parametric sphere with diameter as input
‘points in GS
‘ * * * * * * * * * * * * * – – – – – – – – – – – * * * * * * *

Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument

Set part1 = partDocument1.Part

Set parameters1 = part1.Parameters

Set hybridBodies1 = part1.HybridBodies

‘Set hybridShapes1 = hybridBody1.HybridShapes

Set axisSystems1 = part1.AxisSystems

msgbox (“Select the geometrical set with I/P points for creating Sphere”)

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

Set parameters1 = part1.Parameters

Dim length1 ‘As Dimension
Set length1 = parameters1.CreateDimension(“”, “LENGTH”, 0.000000)
length1.Rename “SPDia”
length1.Value = 25.000000

‘Spheredia=Inputbox(“Enter Diameter of sphere to be created”)

Dim iCount

Dim i ‘As Integer

oSelection.Search “CATGmoSearch.Point,sel”

iCount = oSelection.Count

For i = 1 to iCount

Set hybridShapePointOnSurface1 = oSelection.Item(i).Value

Dim reference1 ‘As reference
Set reference1 = part1.CreateReferenceFromObject(hybridShapePointOnSurface1)

Set hybridShapeFactory1 = part1.HybridShapeFactory

Dim relations1 ‘As Relations
Set relations1 = part1.Relations

Dim formula1 ‘As Formula
Set formula1 = relations1.CreateFormula(“Formula.2”, “”, length1, SPDia)

formula1.Rename “Formula.2”

Set hybridShapeSphere1 = hybridShapeFactory1.AddNewSphere(reference1, Nothing, SPDia, -45.000000, 45.000000, 0.000000, 180.000000)

hybridShapeSphere1.Limitation = 1

hybridBody1.AppendHybridShape hybridShapeSphere1

part1.InWorkObject = hybridShapeSphere1

hybridShapeSphere1.name = “Shpere for-” & oSelection.Item(i).Value.name

‘part1.Update

NEXT

part1.Update

msgbox (“Total number of sphere created -” & iCount)

End Sub

 

[LWolf]

Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument
Set part1 = partDocument1.Part
Set parameters1 = part1.Parameters
Set hybridBodies1 = part1.HybridBodies
Set axisSystems1 = part1.AxisSystems

MsgBox ("Select the geometrical set with I/P points for creating Sphere")

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

Set parameters1 = part1.Parameters

Dim length1 'As Dimension
Set length1 = parameters1.CreateDimension("", "LENGTH", 0)
length1.Rename "SPDia"
length1.Value = 25

'Spheredia=Inputbox("Enter Diameter of sphere to be created")

Dim iCount

Dim i 'As Integer

oSelection.Search "CATGmoSearch.Point, sel"

iCount = oSelection.Count

For i = 1 To iCount

Set hybridShapePointOnSurface1 = oSelection.item(i).Value

Dim reference1 'As reference
Set reference1 = part1.CreateReferenceFromObject(hybridShapePointOnSurface1)

Set hybridShapeFactory1 = part1.HybridShapeFactory

Dim relations1 'As Relations
Set relations1 = part1.Relations
Set hybridShapeSphere1 = hybridShapeFactory1.AddNewSphere(reference1, Nothing, length1.Value, -45#, 45#, 0#, 180#)
hybridShapeSphere1.Limitation = 1

Dim myradius
Set myradius = hybridShapeSphere1.Radius

Dim formula1 'As Formula
Set formula1 = relations1.CreateFormula("Formula.2", "", myradius, SPDia)
formula1.Rename "Formula.2"

hybridBody1.AppendHybridShape hybridShapeSphere1
part1.InWorkObject = hybridShapeSphere1
hybridShapeSphere1.name = "Shpere for-" & oSelection.item(i).Value.name

Next

part1.Update

MsgBox ("Total number of sphere created -" & iCount)

End Sub

regards,
LWolf

 

[LWolf]

two changes: in Set HybridShapeSphere1 you need a value of the radius...
and then I added myradius, which takes the sphereradius as its reference...

regards,
LWolf

 

[LWolf]

disregard my inputs... just realised you want to have the parameter controlling your sphere...

regards,
LWolf

 

[LWolf]

ok, sorry for all the spam, delete doesn't work for me today...
here is my last input, (i promise)
here is the working code... I changed the formula to go for the parameter.name ( Set formula1 = relations1.CreateFormula("Formula.2", "", myradius, parameters1.item("SPDia").name))

Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument
Set part1 = partDocument1.Part
Set parameters1 = part1.Parameters
Set hybridBodies1 = part1.HybridBodies
Set axisSystems1 = part1.AxisSystems

MsgBox ("Select the geometrical set with I/P points for creating Sphere")

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 hybridBody1 = hybridBodies1.Add()
Set hybridBody1 = CATIA.ActiveDocument.Part.InWorkObject
Set parameters1 = part1.Parameters
Dim length1 'As Dimension
Set length1 = parameters1.CreateDimension("MM", "LENGTH", 25)
length1.Rename "SPDia"
'Spheredia=Inputbox("Enter Diameter of sphere to be created")
Dim iCount
Dim i 'As Integer
oSelection.Search "CATGmoSearch.Point, sel"

iCount = oSelection.Count

For i = 1 To iCount

Set hybridShapePointOnSurface1 = oSelection.item(i).Value

Dim reference1 'As reference
Set reference1 = part1.CreateReferenceFromObject(hybridShapePointOnSurface1)

Set hybridShapeFactory1 = part1.HybridShapeFactory

Dim relations1 'As Relations
Set relations1 = part1.Relations
Set hybridShapeSphere1 = hybridShapeFactory1.AddNewSphere(reference1, Nothing, length1.Value, -45#, 45#, 0#, 180#)
hybridShapeSphere1.Limitation = 1

Dim myradius
Set myradius = hybridShapeSphere1.Radius
Dim formula1 'As Formula
Set formula1 = relations1.CreateFormula("Formula.2", "", myradius, parameters1.item("SPDia").name)
'formula1.Rename "Formula.2"

hybridBody1.AppendHybridShape hybridShapeSphere1
part1.InWorkObject = hybridShapeSphere1
hybridShapeSphere1.name = "Shpere for-" & oSelection.item(i).Value.name
​

Next

part1.Update

MsgBox ("Total number of sphere created -" & iCount)

End Sub

​

regards,
LWolf

 

[DomKum]

Thank you LWolf for your suggestion & guidance.
Its working now.

 

[DomKum]

Hi LWolf,

I just forgot to mention that with the code as below - I mean # included in the script, Macro is showing an error while I try to exeucte.
However replacing # with -45.000/etc its working fine.
Set hybridShapeSphere1 = hybridShapeFactory1.AddNewSphere(reference1, Nothing, length1.Value, -45#, 45#, 0#, 180#)