New Bounding Box issue 2

[jzecha]

Hello,

I created the Bounding Box macro from the Portable Script Center.
When I try to run it on a part, i click the axis it creates, i click a plane, and it begins to run.
It creates a bunch of geometry and then fails.
Here is the failure notification:

Execute the script "BoundingBox.CATScript".
The scripting engine for CATScript has reported the following error:

Source: CATIAPart
Description: The method Update Failed
Line:609
Column:16

See the language reference guide or the V5 Automation APIs documentation.
Line: 609 shows: par1.update.

Does anybody know what is going on or what I can do to fix this?

 

[ferdo]

HI,

Which CATIA release, what operating system, 32 or 64 bit ? You said is a CATScript, correct? What kind of CATPart is it? Is it Enable Hybrid Design mode or not?

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[jzecha]

I am running Windows 7 Professional 64 bit, Catia V5 R23.
It is the CATScript out of the Portable Script Center.
Hybrid design is disabled.
Its fairly simple part.

 

[ferdo]

I don't have CATIA now (neither the script) but you can comment that line and see what is going on.

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[jzecha]

The macro fails at part1.update.

'----------------------------------------------------------------------------------------------------------------------------------
'creation  sweep
'----------------------------------------------------------------------------------------------------------------------------------

                set sweepref_1 = part1.createreferencefromobject(standard_body_sketch3 )
                set guide1 = part1.createreferencefromobject(line_guide )
                Dim sweep1 as HybridShapeSweepExplicit
                set sweep1 =hybridShapeFactory1.AddNewSweepExplicit(sweepref_1,guide1 )
                hybridBody2.AppendHybridShape sweep1
                part1.InWorkObject = sweep1
                part1.update

 

[ferdo]

Last version checked was 21 and it was OK. Probably in 23 (or newer) is something else....now I don't have v5 and I didn't try to migrate in v6...

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[JeniaL]

this works ok with v5r23 sp3
you have to adopt it to vba...sorry trying to stay out of CatScript

Private Sub OkAndExit_Click()
Me.Hide
'Get CATIA or Launch it if necessary.
    On Error Resume Next
    Set MyCATIA = GetObject(, "CATIA.Application")
        If Err.Number <> 0 Then
        Set MyCATIA = CreateObject("CATIA.Application")
        MyCATIA.Visible = False
    End If
    On Error GoTo 0
'Make sure they have axis ready and want to start
    MyCATIA.DisplayFileAlerts = False
    Dim Message, Style, Title, Response, MyString
    Message = ("PRESS OK AND SELECT AXIS SYSTEM" & _
        (Chr(13)) & _
        "THE AXIS SYSTEM MUST BE BASED ON TOOLING DIRECTION")
        
    Style = vbYesNo    'Define buttons.
    
    If MsgBox(Message, Style) = vbYes Then
        'Declare variables
        Dim axis
        Dim remake
        Dim partDocument1 As PartDocument
        Dim part1 As Part
        Dim axisref As Object
        Dim shapeFactory1 As ShapeFactory
        Dim hybridShapeFactory1 As HybridShapeFactory
        Dim sStatus As String
        Dim hybridShapeD1, hybridShapeD2, hybridShapeD3 As HybridShapeDirection
        Dim Default, a1, a2, a3, a4, a5, a6 'To change the offsets of the box
        Dim bodies1 As Bodies
        Dim body1 As Body
        Dim reference1 As Reference
        Dim HybridShapeExtremum1, HybridShapeExtremum2, HybridShapeExtremum3 As HybridShapeExtremum
        Dim HybridShapeExtremum4, HybridShapeExtremum5, HybridShapeExtremum6 As HybridShapeExtremum
        Dim originCoord(2)
        Dim SELECTION As Object

        Set partDocument1 = MyCATIA.ActiveDocument
        If (InStr(partDocument1.Name, ".CATPart")) <> 0 Then
            Set part1 = partDocument1.Part
            Set SELECTION = partDocument1.SELECTION
            part1.Update
            Set hybridShapeFactory1 = part1.HybridShapeFactory
            ReDim sFilter(0)
            'MsgBox "Select the axis to base the bounding on."
            sFilter(0) = "AxisSystem"
            sStatus = SELECTION.SelectElement2(sFilter, "Select the axis to base the bounding on.", False)
            Dim axiscoord(2)
            Dim axissyst
            Set axissyst = SELECTION.Item(1).Value
            Set axisref = SELECTION.Item(1).Value
            ref_name_systaxis = axissyst.Name

            axissyst.IsCurrent = 1
            axissyst.Name = "BBoxAxis"
 
            axname = axissyst.Name
            Dim originpoint As HybridShapePointCoord
            axissyst.GetOrigin originCoord
            Set originpoint = hybridShapeFactory1.AddNewPointCoord(originCoord(0), originCoord(1), originCoord(2))
            Set axisref = part1.CreateReferenceFromObject(originpoint)
            axissyst.GetXAxis axiscoord
            Set hybridShapeD1 = hybridShapeFactory1.AddNewDirectionByCoord(axiscoord(0), axiscoord(1), axiscoord(2))
            axissyst.GetYAxis axiscoord
            Set hybridShapeD2 = hybridShapeFactory1.AddNewDirectionByCoord(axiscoord(0), axiscoord(1), axiscoord(2))
            axissyst.GetZAxis axiscoord
            Set hybridShapeD3 = hybridShapeFactory1.AddNewDirectionByCoord(axiscoord(0), axiscoord(1), axiscoord(2))

            Dim Plane_line_1 As HybridShapeLinePtDir
            Set Plane_line_1 = hybridShapeFactory1.AddNewLinePtDir(originpoint, hybridShapeD1, 0, 0, False)
            Dim Plane_line_2 As HybridShapeLinePtDir
            Set Plane_line_2 = hybridShapeFactory1.AddNewLinePtDir(originpoint, hybridShapeD2, 0, 0, False)

            SELECTION.Clear

            Set partDocument1 = MyCATIA.ActiveDocument
            Set part1 = partDocument1.Part
              
            Dim oBodies As Bodies
            Set oBodies = part1.Bodies

            'J is defined to make unique names for Axis and the Body for the bounding box
            Dim j As Integer
            j = oBodies.Count

            Set bodies1 = part1.Bodies
            Set body1 = bodies1.Add()
            body1.Name = "Bounding Box." & j
            
            Set hybridBodies1 = body1.HybridBodies
            Set hybridBody1 = hybridBodies1.Add
            hybridBody1.Name = "definition_points"

            ' Ask for face selection, that belongs to object to boundary
            ReDim sFilter(0)
            MsgBox "SELECT A  FACE THAT BELONGS TO THE SOLID TO BE BOUNDED."
            sFilter(0) = "Face"
            sStatus = SELECTION.SelectElement2(sFilter, "Select a face that belongs to the solid to be bounded.", False)
            If (sStatus = "Cancel") Then
                Exit Sub
            End If

            Set reference1 = SELECTION.Item(1).Value
            Dim hybridShapeExtract1 As HybridShapeExtract
            Set hybridShapeExtract1 = hybridShapeFactory1.AddNewExtract(reference1)
            hybridShapeExtract1.PropagationType = 1
            hybridShapeExtract1.ComplementaryExtract = False
            hybridShapeExtract1.IsFederated = False
            Set reference1 = hybridShapeExtract1

            'Create the 6 Extrenum items for the Solid/Surf.  May not be single points, will be solved with next points
            Set HybridShapeExtremum1 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD1, 1)
            Set HybridShapeExtremum2 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD1, 0)
            Set HybridShapeExtremum3 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD2, 1)
            Set HybridShapeExtremum4 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD2, 0)
            Set HybridShapeExtremum5 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD3, 1)
            Set HybridShapeExtremum6 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD3, 0)
            part1.Update
                
            ' Creates Geometrical Set under the Solid, to contain the construction elements

            Dim hybridBody2 As HybridBody
            Set hybridBody2 = hybridBodies1.Item("definition_points")

            hybridBody2.AppendHybridShape HybridShapeExtremum1
            part1.InWorkObject = HybridShapeExtremum1
            HybridShapeExtremum1.Name = "max_X"
            hybridBody2.AppendHybridShape HybridShapeExtremum2
            part1.InWorkObject = HybridShapeExtremum2
            HybridShapeExtremum2.Name = "min_X"
            hybridBody2.AppendHybridShape HybridShapeExtremum3
            part1.InWorkObject = HybridShapeExtremum3
            HybridShapeExtremum3.Name = "max_Y"
            hybridBody2.AppendHybridShape HybridShapeExtremum4
            part1.InWorkObject = HybridShapeExtremum4
            HybridShapeExtremum4.Name = "min_Y"
            hybridBody2.AppendHybridShape HybridShapeExtremum5
            part1.InWorkObject = HybridShapeExtremum5
            HybridShapeExtremum5.Name = "max_Z"
            hybridBody2.AppendHybridShape HybridShapeExtremum6
            part1.InWorkObject = HybridShapeExtremum6
            HybridShapeExtremum6.Name = "min_Z"

            part1.Update

            ' Creates a 6 single points using the Extrenums as refs, so if the Extrenum was a line or surf, you can still offset planes to these points

            Dim Ref1 As Reference
            Set Ref1 = part1.CreateReferenceFromObject(HybridShapeExtremum1)
            Dim Point1 As HybridShapePointCoord
            Set Point1 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref1)
            hybridBody2.AppendHybridShape Point1
            Set point_ref11 = part1.CreateReferenceFromObject(Point1)
            Dim Ref2 As Reference
            Set Ref2 = part1.CreateReferenceFromObject(HybridShapeExtremum2)
            Dim Point2 As HybridShapePointCoord
            Set Point2 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref2)
            hybridBody2.AppendHybridShape Point2
            Set point_ref12 = part1.CreateReferenceFromObject(Point2)
            Dim Ref3 As Reference
            Set Ref3 = part1.CreateReferenceFromObject(HybridShapeExtremum3)
            Dim Point3 As HybridShapePointCoord
            Set Point3 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref3)
            hybridBody2.AppendHybridShape Point3
            Set point_ref13 = part1.CreateReferenceFromObject(Point3)
            Dim Ref4 As Reference
            Set Ref4 = part1.CreateReferenceFromObject(HybridShapeExtremum4)
            Dim Point4 As HybridShapePointCoord
            Set Point4 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref4)
            hybridBody2.AppendHybridShape Point4
            Set point_ref14 = part1.CreateReferenceFromObject(Point4)
            Dim Ref5 As Reference
            Set Ref5 = part1.CreateReferenceFromObject(HybridShapeExtremum5)
            Dim Point5 As HybridShapePointCoord
            Set Point5 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref5)
            hybridBody2.AppendHybridShape Point5
            Set point_ref5 = part1.CreateReferenceFromObject(Point5)
            Dim Ref6 As Reference
            Set Ref6 = part1.CreateReferenceFromObject(HybridShapeExtremum6)
            Dim Point6 As HybridShapePointCoord
            Set Point6 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref6)
            hybridBody2.AppendHybridShape Point6
            Set point_ref6 = part1.CreateReferenceFromObject(Point6)

            part1.Update

            axissyst.IsCurrent = 1

            'Create a sketch, will the the X and Y boundary

            Set sketches1 = hybridBody1.HybridSketches
            
            Set reference_axis_syst = part1.CreateReferenceFromName("Selection_RSur:(Face:(Brp:(BBoxAxis;1);None:());BBoxAxis)")
            Set standard_body_sketch1 = sketches1.Add(reference_axis_syst)
            Set factory2D1 = standard_body_sketch1.OpenEdition()
            Set geometricElements1 = standard_body_sketch1.GeometricElements
            Set axis2D1 = geometricElements1.Item("AbsoluteAxis")
            Set line_HDirection = axis2D1.GetItem("HDirection")
            line_HDirection.ReportName = 1
            Set line_VDirection = axis2D1.GetItem("VDirection")
            line_VDirection.ReportName = 2
    
            ' Creates a square in the sketch
            ponto = 20000
            Set point_ref_1 = factory2D1.CreatePoint(-ponto, -ponto)
            point_ref_1.ReportName = 3
            Set point_ref_2 = factory2D1.CreatePoint(ponto, -ponto)
            point_ref_2.ReportName = 4
            Set point_ref_3 = factory2D1.CreatePoint(ponto, ponto)
            point_ref_3.ReportName = 5
            Set point_ref_4 = factory2D1.CreatePoint(-ponto, ponto)
            point_ref_4.ReportName = 6
            
            Set line_ref_1_2 = factory2D1.CreateLine(-ponto, -ponto, ponto, -ponto)
            line_ref_1_2.ReportName = 7
            line_ref_1_2.StartPoint = point_ref_1
            line_ref_1_2.EndPoint = point_ref_2
        
            Set line_ref_2_3 = factory2D1.CreateLine(ponto, -ponto, ponto, ponto)
            line_ref_2_3.ReportName = 8
            line_ref_2_3.StartPoint = point_ref_2
            line_ref_2_3.EndPoint = point_ref_3
            
            Set line_ref_3_4 = factory2D1.CreateLine(-ponto, ponto, ponto, ponto)
            line_ref_3_4.ReportName = 9
            line_ref_3_4.StartPoint = point_ref_4
            line_ref_3_4.EndPoint = point_ref_3
            
            Set line_ref_4_1 = factory2D1.CreateLine(-ponto, -ponto, -ponto, ponto)
            line_ref_4_1.ReportName = 10
            'line_ref_4_1.Construction = True
            line_ref_4_1.StartPoint = point_ref_1
            line_ref_4_1.EndPoint = point_ref_4
    
            ' Create Reference lines and constraints
            Set reference_line_ref_1_2 = part1.CreateReferenceFromObject(line_ref_1_2)
            Set reference_line_ref_2_3 = part1.CreateReferenceFromObject(line_ref_2_3)
            Set reference_line_ref_3_4 = part1.CreateReferenceFromObject(line_ref_3_4)
            Set reference_line_ref_4_1 = part1.CreateReferenceFromObject(line_ref_4_1)
            
            Set electrode_constraints = standard_body_sketch1.Constraints

            Set constraint_toto_2 = electrode_constraints.AddBiEltCst(catCstTypeDistance, point_ref11, reference_line_ref_2_3)
            Set constraint_toto_3 = electrode_constraints.AddBiEltCst(catCstTypeDistance, point_ref13, reference_line_ref_3_4)
            Set constraint_toto_4 = electrode_constraints.AddBiEltCst(catCstTypeDistance, reference_line_ref_4_1, point_ref12)
            Set constraint_toto_1 = electrode_constraints.AddBiEltCst(catCstTypeDistance, reference_line_ref_1_2, point_ref14)

            Dim length1 As Dimension
            Set length1 = constraint_toto_1.Dimension
            length1.Value = 0
            Dim length2 As Dimension
            Set length2 = constraint_toto_2.Dimension
            length2.Value = 0
            Dim length3 As Dimension
            Set length3 = constraint_toto_3.Dimension
            length3.Value = 0
            Dim length4 As Dimension
            Set length4 = constraint_toto_4.Dimension
            length4.Value = 0
            
            standard_body_sketch1.CloseEdition
            part1.Update

'----------------------------------------------------------------------------------------------------------------------------------
' Creation of the Max Z and Min Z planes
'----------------------------------------------------------------------------------------------------------------------------------

            Dim plan_inferieur As HybridShapePlaneOffsetPt
            Dim plan_origin As HybridShapePlane2Lines
            Dim Origin_line_1 As Reference
            Set Origin_line_1 = part1.CreateReferenceFromObject(line_HDirection)
            Dim Origin_line_2 As Reference
            Set Origin_line_2 = part1.CreateReferenceFromObject(line_VDirection)
            Set plan_origin = hybridShapeFactory1.AddNewPlane2Lines(Origin_line_1, Origin_line_2)
            Dim ref_plan_origin As Reference
            Set ref_plan_origin = part1.CreateReferenceFromObject(plan_origin)
            Set Ref6 = part1.CreateReferenceFromObject(HybridShapeExtremum6)
            Set plan_inferieur = hybridShapeFactory1.AddNewPlaneOffsetPt(ref_plan_origin, point_ref6)
            hybridBody2.AppendHybridShape plan_inferieur
            part1.InWorkObject = plan_inferieur

            Dim plan_superieur As HybridShapePlaneOffsetPt
            Set Ref5 = part1.CreateReferenceFromObject(HybridShapeExtremum5)
            Set plan_superieur = hybridShapeFactory1.AddNewPlaneOffsetPt(ref_plan_origin, point_ref5)
            hybridBody2.AppendHybridShape plan_superieur
            part1.InWorkObject = plan_superieur

            part1.Update
            
'----------------------------------------------------------------------------------------------------------------------------------
' Creates the line that sweeps around the XY Sketch boundary
'----------------------------------------------------------------------------------------------------------------------------------

            Dim Point_inf As HybridShapePointCoord
            Set Point_inf = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, point_ref6)
            hybridBody2.AppendHybridShape Point_inf
            Dim ref_point_inf As Reference
            Set ref_point_inf = part1.CreateReferenceFromObject(Point_inf)

            Dim proj_pt_inf As HybridShapeProject
            Set proj_pt_inf = hybridShapeFactory1.AddNewProject(point_ref6, plan_superieur)
            hybridBody2.AppendHybridShape proj_pt_inf
            part1.InWorkObject = proj_pt_inf

            Dim Point_sup As HybridShapePointCoord
            Set Point_sup = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, proj_pt_inf)
            hybridBody2.AppendHybridShape Point_sup
            Dim ref_point_sup As Reference
            Set ref_point_sup = part1.CreateReferenceFromObject(Point_sup)

            Dim line_guide As HybridShapeLinePtPt
            Set line_guide = hybridShapeFactory1.AddNewLinePtPt(ref_point_sup, ref_point_inf)
            hybridBody2.AppendHybridShape line_guide
            part1.InWorkObject = line_guide
            Set ref_guideline = part1.CreateReferenceFromObject(line_guide)

            Dim oStart As Length
            Set oStart = line_guide.BeginOffset
            oStart.Value = 1
            Dim oEnd As Length
            Set oEnd = line_guide.EndOffset
            oEnd.Value = 1

            Set constraints_for_z = part1.Constraints
            Set constraint_dz = constraints_for_z.AddMonoEltCst(catCstTypeLength, ref_guideline)
            Set length_dz = constraint_dz.Dimension
            
            part1.Update

'----------------------------------------------------------------------------------------------------------------------------------
' Second Sketch, basically the XY boundary sketch placed down to Min Z
'----------------------------------------------------------------------------------------------------------------------------------

            Set sketches2 = hybridBody1.HybridSketches
            Set standard_body_sketch2 = sketches2.Add(plan_inferieur)

            Set factory2D2 = standard_body_sketch2.OpenEdition()
            Set geometricElements2 = standard_body_sketch2.GeometricElements
            Set axis2D1 = geometricElements1.Item("AbsoluteAxis")

            pont = 200000
            Set point_ref1_1 = factory2D2.CreatePoint(-pont, -pont)
            Set point_ref1_2 = factory2D2.CreatePoint(pont, -pont)
            Set point_ref1_3 = factory2D2.CreatePoint(pont, pont)
            Set point_ref1_4 = factory2D2.CreatePoint(-pont, pont)
    
            Set line_ref1_1_2 = factory2D2.CreateLine(-pont, -pont, pont, -pont)
            line_ref1_1_2.StartPoint = point_ref1_1
            line_ref1_1_2.EndPoint = point_ref1_2
    
            Set line_ref1_2_3 = factory2D2.CreateLine(pont, -pont, pont, pont)
            line_ref1_2_3.StartPoint = point_ref1_2
            line_ref1_2_3.EndPoint = point_ref1_3
    
            Set line_ref1_3_4 = factory2D2.CreateLine(-pont, pont, pont, pont)
            line_ref1_3_4.StartPoint = point_ref1_4
            line_ref1_3_4.EndPoint = point_ref1_3
    
            Set line_ref1_4_1 = factory2D2.CreateLine(-pont, -pont, -pont, pont)
            line_ref1_4_1.StartPoint = point_ref1_1
            line_ref1_4_1.EndPoint = point_ref1_4

            Set reference_line_ref1_1_2 = part1.CreateReferenceFromObject(line_ref1_1_2)
            Set reference_line_ref1_2_3 = part1.CreateReferenceFromObject(line_ref1_2_3)
            Set reference_line_ref1_3_4 = part1.CreateReferenceFromObject(line_ref1_3_4)
            Set reference_line_ref1_4_1 = part1.CreateReferenceFromObject(line_ref1_4_1)

            Set reference_line_ref_1_2 = part1.CreateReferenceFromObject(line_ref_1_2)
            Set reference_line_ref_2_3 = part1.CreateReferenceFromObject(line_ref_2_3)
            Set reference_line_ref_3_4 = part1.CreateReferenceFromObject(line_ref_3_4)
            Set reference_line_ref_4_1 = part1.CreateReferenceFromObject(line_ref_4_1)

            Set proj_1_2 = factory2D2.CreateProjection(reference_line_ref_1_2)
            Set proj_2_3 = factory2D2.CreateProjection(reference_line_ref_2_3)
            Set proj_3_4 = factory2D2.CreateProjection(reference_line_ref_3_4)
            Set proj_4_1 = factory2D2.CreateProjection(reference_line_ref_4_1)

            Set ref_line_sk1_1_2 = part1.CreateReferenceFromObject(proj_1_2)
            Set ref_line_sk1_2_3 = part1.CreateReferenceFromObject(proj_2_3)
            Set ref_line_sk1_3_4 = part1.CreateReferenceFromObject(proj_3_4)
            Set ref_line_sk1_4_1 = part1.CreateReferenceFromObject(proj_4_1)
    
            Set electrode_constraints = standard_body_sketch2.Constraints
            Set constraint_toto_11 = electrode_constraints.AddBiEltCst(catCstTypeDistance, reference_line_ref1_1_2, ref_line_sk1_1_2)
            Set constraint_toto_12 = electrode_constraints.AddBiEltCst(catCstTypeDistance, ref_line_sk1_2_3, reference_line_ref1_2_3)
            Set constraint_toto_13 = electrode_constraints.AddBiEltCst(catCstTypeDistance, ref_line_sk1_3_4, reference_line_ref1_3_4)
            Set constraint_toto_14 = electrode_constraints.AddBiEltCst(catCstTypeDistance, reference_line_ref1_4_1, ref_line_sk1_4_1)
            'Dim length11 As Dimension
            Set length11 = constraint_toto_11.Dimension
            length11.Value = 1
            Dim length12 As Dimension
            Set length12 = constraint_toto_12.Dimension
            length12.Value = 1
            Dim length13 As Dimension
            Set length13 = constraint_toto_13.Dimension
            length13.Value = 1
            Dim length14 As Dimension
            Set length14 = constraint_toto_14.Dimension
            length14.Value = 1
            
            standard_body_sketch2.CloseEdition
            part1.Update
            
'----------------------------------------------------------------------------------------------------------------------------------
' Offset from Sketch2, using the Relations so you can change the offsets
'----------------------------------------------------------------------------------------------------------------------------------

            Set sketches3 = hybridBody1.HybridSketches
            Set standard_body_sketch3 = sketches3.Add(plan_inferieur)
            Set factory2D3 = standard_body_sketch3.OpenEdition()
            Set geometricElements3 = standard_body_sketch3.GeometricElements
            Set axis2D1 = geometricElements1.Item("AbsoluteAxis")

            Set reference_line_ref1_1_2 = part1.CreateReferenceFromObject(line_ref1_1_2)
            Set reference_line_ref1_2_3 = part1.CreateReferenceFromObject(line_ref1_2_3)
            Set reference_line_ref1_3_4 = part1.CreateReferenceFromObject(line_ref1_3_4)
            Set reference_line_ref1_4_1 = part1.CreateReferenceFromObject(line_ref1_4_1)
            
            Set proj1_1_2 = factory2D3.CreateProjection(reference_line_ref1_1_2)
            Set proj1_2_3 = factory2D3.CreateProjection(reference_line_ref1_2_3)
            Set proj1_3_4 = factory2D3.CreateProjection(reference_line_ref1_3_4)
            Set proj1_4_1 = factory2D3.CreateProjection(reference_line_ref1_4_1)

            Set ref_proj1_1_2 = part1.CreateReferenceFromObject(proj1_1_2)
            Set ref_proj1_2_3 = part1.CreateReferenceFromObject(proj1_2_3)
            Set ref_proj1_3_4 = part1.CreateReferenceFromObject(proj1_3_4)
            Set ref_proj1_4_1 = part1.CreateReferenceFromObject(proj1_4_1)

            Set constraints_dim = standard_body_sketch3.Constraints
            Set constraint_dx = constraints_dim.AddMonoEltCst(catCstTypeLength, ref_proj1_1_2)
            Set constraint_dy = constraints_dim.AddMonoEltCst(catCstTypeLength, ref_proj1_2_3)
            Set length_dx = constraint_dx.Dimension
            dx_value = length_dx.Value
            Set length_dy = constraint_dy.Dimension
            dy_value = length_dy.Value

            standard_body_sketch3.CloseEdition
            part1.Update

            ' Create the offset parameters
            Dim string_1 As String
            string_1 = "Offset_Bbox_Max_X." & j
            Dim string_2 As String
            string_2 = "Offset_Bbox_Min_X." & j
            Dim string_3 As String
            string_3 = "Offset_Bbox_Max_Y." & j
            Dim string_4 As String
            string_4 = "Offset_Bbox_Min_Y." & j
            Dim string_5 As String
            string_5 = "Offset_Bbox_Max_Z." & j
            Dim string_6 As String
            string_6 = "Offset_Bbox_Min_Z." & j
            Dim string_7 As String
            string_7 = "Bbox_dx." & j
            Dim string_8 As String
            string_8 = "Bbox_dy." & j
            Dim string_9 As String
            string_9 = "Bbox_dz." & j

            Dim Offset_Bbox_Max_X As RealParam
            Set Offset_Bbox_Max_X = part1.Parameters.CreateDimension(string_1, "Length", 0)
            Dim Offset_Bbox_Min_X As RealParam
            Set Offset_Bbox_Min_X = part1.Parameters.CreateDimension(string_2, "Length", 0)
            Dim Offset_Bbox_Max_Y As RealParam
            Set Offset_Bbox_Max_Y = part1.Parameters.CreateDimension(string_3, "Length", 0)
            Dim Offset_Bbox_Min_Y As RealParam
            Set Offset_Bbox_Min_Y = part1.Parameters.CreateDimension(string_4, "Length", 0)
            Dim Offset_Bbox_Max_Z As RealParam
            Set Offset_Bbox_Max_Z = part1.Parameters.CreateDimension(string_5, "Length", 0)
            Dim Offset_Bbox_Min_Z As RealParam
            Set Offset_Bbox_Min_Z = part1.Parameters.CreateDimension(string_6, "Length", 0)
            Set Bbox_dx_hidden = part1.Parameters.CreateDimension(string_7, "Length", dx_value)
            Set Bbox_dy_hidden = part1.Parameters.CreateDimension(string_8, "Length", dy_value)
            Set Bbox_dz_hidden = part1.Parameters.CreateDimension(string_9, "Length", length_dz.Value)
            Bbox_dx_hidden.Hidden = True
            Bbox_dy_hidden.Hidden = True
            Bbox_dz_hidden.Hidden = True
            Set Bbox_dx = part1.Parameters.CreateDimension(string_7, "Length", 0)
            Set Bbox_dy = part1.Parameters.CreateDimension(string_8, "Length", 0)
            Set Bbox_dz = part1.Parameters.CreateDimension(string_9, "Length", 0)
            
            Dim Formula_1 As Formula
            Set Formula_1 = part1.Relations.CreateFormula("formula_Bbox_1." & j, "", length14, "Offset_Bbox_Min_X." & j)
            Dim Formula_2 As Formula
            Set Formula_2 = part1.Relations.CreateFormula("formula_Bbox_2." & j, "", length12, "Offset_Bbox_Max_X." & j)
            Dim Formula_3 As Formula
            Set Formula_3 = part1.Relations.CreateFormula("formula_Bbox_4." & j, "", length11, "Offset_Bbox_Min_Y." & j)
            Dim Formula_4 As Formula
            Set Formula_4 = part1.Relations.CreateFormula("formula_Bbox_4." & j, "", length13, "Offset_Bbox_Max_Y." & j)
            Dim Formula_5 As Formula
            Set Formula_5 = part1.Relations.CreateFormula("formula_Bbox_5." & j, "", oEnd, " Offset_Bbox_Min_Z." & j)
            Dim Formula_6 As Formula
            Set Formula_6 = part1.Relations.CreateFormula("formula_Bbox_6." & j, "", oStart, " Offset_Bbox_Max_Z." & j)
            Dim Formula_7 As Formula
            Set Formula_7 = part1.Relations.CreateFormula("formula_Bbox_7." & j, "", Bbox_dx, "Bbox_dx." & j & "+Offset_Bbox_Min_X." & j & "+Offset_Bbox_Max_X." & j & "-2mm")
            Dim Formula_8 As Formula
            Set Formula_8 = part1.Relations.CreateFormula("formula_Bbox_8." & j, "", Bbox_dy, "Bbox_dy." & j & "+Offset_Bbox_Min_Y." & j & "+Offset_Bbox_Max_Y." & j & "-2mm")
            Dim Formula_9 As Formula
            Set Formula_9 = part1.Relations.CreateFormula("formula_Bbox_9." & j, "", Bbox_dz, "Bbox_dz." & j & "+Offset_Bbox_Min_Z." & j & "+Offset_Bbox_Max_Z." & j & "-2mm")

'----------------------------------------------------------------------------------------------------------------------------------
' Sweep the Z line around the XY boundary.  This will be closed
'----------------------------------------------------------------------------------------------------------------------------------
                
            Set sweepref_1 = part1.CreateReferenceFromObject(standard_body_sketch3)
            Set guide1 = part1.CreateReferenceFromObject(line_guide)
            Dim sweep1 As HybridShapeSweepExplicit
            Set sweep1 = hybridShapeFactory1.AddNewSweepExplicit(sweepref_1, guide1)
            hybridBody2.AppendHybridShape sweep1
            part1.InWorkObject = sweep1
            part1.Update

            ' Close the Sweep
            Set shapeFactory1 = part1.ShapeFactory
            Set hybridBodies1 = body1.HybridBodies
            Set hybridBody1 = hybridBodies1.Item("definition_points")
            Dim hybridShapes1 As HybridShapes
            Set hybridShapes1 = hybridBody1.HybridShapes
            
            Dim refer1 As Reference
            Set refer1 = part1.CreateReferenceFromObject(sweep1)
    
            Dim closeSurface1 As CloseSurface
            Set closeSurface1 = shapeFactory1.AddNewCloseSurface(refer1)
            closeSurface1.Name = "BoundingBox"
            part1.Update

            SELECTION.Clear
            SELECTION.Add hybridBody1
            SELECTION.VisProperties.SetShow catVisPropertyNoShowAttr
            SELECTION.Clear
            SELECTION.Add body1
            SELECTION.VisProperties.SetRealColor 0, 0, 0, 0
            SELECTION.VisProperties.SetRealOpacity 150, 1
            SELECTION.VisProperties.SetRealWidth 2, 1
            part1.Update
            axissyst.Name = "Bounding Box Axis." & j
            
        Else
            MsgBox "The active document must be a CATPart"
        End If

    End If
Unload BoundingBox
End Sub

 

[jzecha]

I am fairly new to coding, I have only messed with CATScripts.
How do I Adapt the VB6 code you provided to VBA?
I have no preference over any of the codes, as long as I can get them to work.

 

[JeniaL]

here's working code.checked on catia v5r25sp3

Sub CATMain()

    'Make sure they have axis ready and want to start
    CATIA.DisplayFileAlerts = False
    Dim Message, Style, Title, Response, MyString
    Message = ("PRESS OK AND SELECT AXIS SYSTEM" & _
        (Chr(13)) & _
        "THE AXIS SYSTEM MUST BE BASED ON TOOLING DIRECTION")
        
    Style = vbYesNo    'Define buttons.
    
    If MsgBox(Message, Style) = vbYes Then
        'Declare variables
        Dim axis
        Dim remake
        Dim partDocument1 As PartDocument
        Dim part1 As Part
        Dim axisref As Object
        Dim shapeFactory1 As ShapeFactory
        Dim hybridShapeFactory1 As hybridShapeFactory
        Dim sStatus As String
        Dim hybridShapeD1, hybridShapeD2, hybridShapeD3 As HybridShapeDirection
        Dim Default, a1, a2, a3, a4, a5, a6 'To change the offsets of the box
        Dim bodies1 As Bodies
        Dim body1 As Body
        Dim reference1 As Reference
        Dim HybridShapeExtremum1, HybridShapeExtremum2, HybridShapeExtremum3 As HybridShapeExtremum
        Dim HybridShapeExtremum4, HybridShapeExtremum5, HybridShapeExtremum6 As HybridShapeExtremum
        Dim originCoord(2)
        Dim SELECTION As Object

        Set partDocument1 = CATIA.ActiveDocument
        If (InStr(partDocument1.Name, ".CATPart")) <> 0 Then
            Set part1 = partDocument1.Part
            Set SELECTION = partDocument1.SELECTION
            part1.Update
            Set hybridShapeFactory1 = part1.hybridShapeFactory
            ReDim sFilter(0)
            MsgBox "Select the axis to base the bounding on."
            sFilter(0) = "AxisSystem"
            sStatus = SELECTION.SelectElement2(sFilter, "Select the axis to base the bounding on.", False)
            Dim axiscoord(2)
            Dim axissyst
            Set axissyst = SELECTION.Item(1).Value
            Set axisref = SELECTION.Item(1).Value
            ref_name_systaxis = axissyst.Name

            axissyst.IsCurrent = 1
            axissyst.Name = "BBoxAxis"
 
            axname = axissyst.Name
            Dim originpoint As HybridShapePointCoord
            axissyst.GetOrigin originCoord
            Set originpoint = hybridShapeFactory1.AddNewPointCoord(originCoord(0), originCoord(1), originCoord(2))
            Set axisref = part1.CreateReferenceFromObject(originpoint)
            axissyst.GetXAxis axiscoord
            Set hybridShapeD1 = hybridShapeFactory1.AddNewDirectionByCoord(axiscoord(0), axiscoord(1), axiscoord(2))
            axissyst.GetYAxis axiscoord
            Set hybridShapeD2 = hybridShapeFactory1.AddNewDirectionByCoord(axiscoord(0), axiscoord(1), axiscoord(2))
            axissyst.GetZAxis axiscoord
            Set hybridShapeD3 = hybridShapeFactory1.AddNewDirectionByCoord(axiscoord(0), axiscoord(1), axiscoord(2))

            Dim Plane_line_1 As HybridShapeLinePtDir
            Set Plane_line_1 = hybridShapeFactory1.AddNewLinePtDir(originpoint, hybridShapeD1, 0, 0, False)
            Dim Plane_line_2 As HybridShapeLinePtDir
            Set Plane_line_2 = hybridShapeFactory1.AddNewLinePtDir(originpoint, hybridShapeD2, 0, 0, False)

            SELECTION.Clear

            Set partDocument1 = CATIA.ActiveDocument
            Set part1 = partDocument1.Part
              
            Dim oBodies As Bodies
            Set oBodies = part1.Bodies

            'J is defined to make unique names for Axis and the Body for the bounding box
            Dim j As Integer
            j = oBodies.Count

            Set bodies1 = part1.Bodies
            Set body1 = bodies1.add()
            body1.Name = "Bounding Box." & j
            
            Set hybridBodies1 = body1.hybridBodies
            Set hybridBody1 = hybridBodies1.add
            hybridBody1.Name = "definition_points"

            ' Ask for face selection, that belongs to object to boundary
            ReDim sFilter(0)
            MsgBox "Select a face that belongs to the solid to be bounded."
            sFilter(0) = "Face"
            sStatus = SELECTION.SelectElement2(sFilter, "Select a face that belongs to the solid to be bounded.", False)
            If (sStatus = "Cancel") Then
                Exit Sub
            End If

            Set reference1 = SELECTION.Item(1).Value
            Dim hybridShapeExtract1 As HybridShapeExtract
            Set hybridShapeExtract1 = hybridShapeFactory1.AddNewExtract(reference1)
            hybridShapeExtract1.PropagationType = 1
            hybridShapeExtract1.ComplementaryExtract = False
            hybridShapeExtract1.IsFederated = False
            Set reference1 = hybridShapeExtract1

            'Create the 6 Extrenum items for the Solid/Surf.  May not be single points, will be solved with next points
            Set HybridShapeExtremum1 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD1, 1)
            Set HybridShapeExtremum2 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD1, 0)
            Set HybridShapeExtremum3 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD2, 1)
            Set HybridShapeExtremum4 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD2, 0)
            Set HybridShapeExtremum5 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD3, 1)
            Set HybridShapeExtremum6 = hybridShapeFactory1.AddNewExtremum(reference1, hybridShapeD3, 0)
            part1.Update
                
            ' Creates Geometrical Set under the Solid, to contain the construction elements

            Dim hybridBody2 As hybridbody
            Set hybridBody2 = hybridBodies1.Item("definition_points")

            hybridBody2.AppendHybridShape HybridShapeExtremum1
            part1.InWorkObject = HybridShapeExtremum1
            HybridShapeExtremum1.Name = "max_X"
            hybridBody2.AppendHybridShape HybridShapeExtremum2
            part1.InWorkObject = HybridShapeExtremum2
            HybridShapeExtremum2.Name = "min_X"
            hybridBody2.AppendHybridShape HybridShapeExtremum3
            part1.InWorkObject = HybridShapeExtremum3
            HybridShapeExtremum3.Name = "max_Y"
            hybridBody2.AppendHybridShape HybridShapeExtremum4
            part1.InWorkObject = HybridShapeExtremum4
            HybridShapeExtremum4.Name = "min_Y"
            hybridBody2.AppendHybridShape HybridShapeExtremum5
            part1.InWorkObject = HybridShapeExtremum5
            HybridShapeExtremum5.Name = "max_Z"
            hybridBody2.AppendHybridShape HybridShapeExtremum6
            part1.InWorkObject = HybridShapeExtremum6
            HybridShapeExtremum6.Name = "min_Z"

            part1.Update

            ' Creates a 6 single points using the Extrenums as refs, so if the Extrenum was a line or surf, you can still offset planes to these points

            Dim Ref1 As Reference
            Set Ref1 = part1.CreateReferenceFromObject(HybridShapeExtremum1)
            Dim Point1 As HybridShapePointCoord
            Set Point1 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref1)
            hybridBody2.AppendHybridShape Point1
            Set point_ref11 = part1.CreateReferenceFromObject(Point1)
            Dim Ref2 As Reference
            Set Ref2 = part1.CreateReferenceFromObject(HybridShapeExtremum2)
            Dim Point2 As HybridShapePointCoord
            Set Point2 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref2)
            hybridBody2.AppendHybridShape Point2
            Set point_ref12 = part1.CreateReferenceFromObject(Point2)
            Dim Ref3 As Reference
            Set Ref3 = part1.CreateReferenceFromObject(HybridShapeExtremum3)
            Dim Point3 As HybridShapePointCoord
            Set Point3 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref3)
            hybridBody2.AppendHybridShape Point3
            Set point_ref13 = part1.CreateReferenceFromObject(Point3)
            Dim Ref4 As Reference
            Set Ref4 = part1.CreateReferenceFromObject(HybridShapeExtremum4)
            Dim Point4 As HybridShapePointCoord
            Set Point4 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref4)
            hybridBody2.AppendHybridShape Point4
            Set point_ref14 = part1.CreateReferenceFromObject(Point4)
            Dim Ref5 As Reference
            Set Ref5 = part1.CreateReferenceFromObject(HybridShapeExtremum5)
            Dim Point5 As HybridShapePointCoord
            Set Point5 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref5)
            hybridBody2.AppendHybridShape Point5
            Set point_ref5 = part1.CreateReferenceFromObject(Point5)
            Dim Ref6 As Reference
            Set Ref6 = part1.CreateReferenceFromObject(HybridShapeExtremum6)
            Dim Point6 As HybridShapePointCoord
            Set Point6 = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, Ref6)
            hybridBody2.AppendHybridShape Point6
            Set point_ref6 = part1.CreateReferenceFromObject(Point6)

            part1.Update

            axissyst.IsCurrent = 1

            'Create a sketch, will the the X and Y boundary

            Set sketches1 = hybridBody1.HybridSketches
            
            Set reference_axis_syst = part1.CreateReferenceFromName("Selection_RSur:(Face:(Brp:(BBoxAxis;1);None:());BBoxAxis)")
            Set standard_body_sketch1 = sketches1.add(reference_axis_syst)
            Set factory2D1 = standard_body_sketch1.OpenEdition()
            Set geometricElements1 = standard_body_sketch1.GeometricElements
            Set axis2D1 = geometricElements1.Item("AbsoluteAxis")
            Set line_HDirection = axis2D1.GetItem("HDirection")
            line_HDirection.ReportName = 1
            Set line_VDirection = axis2D1.GetItem("VDirection")
            line_VDirection.ReportName = 2
    
            ' Creates a square in the sketch
            ponto = 20000
            Set point_ref_1 = factory2D1.CreatePoint(-ponto, -ponto)
            point_ref_1.ReportName = 3
            Set point_ref_2 = factory2D1.CreatePoint(ponto, -ponto)
            point_ref_2.ReportName = 4
            Set point_ref_3 = factory2D1.CreatePoint(ponto, ponto)
            point_ref_3.ReportName = 5
            Set point_ref_4 = factory2D1.CreatePoint(-ponto, ponto)
            point_ref_4.ReportName = 6
            
            Set line_ref_1_2 = factory2D1.CreateLine(-ponto, -ponto, ponto, -ponto)
            line_ref_1_2.ReportName = 7
            line_ref_1_2.StartPoint = point_ref_1
            line_ref_1_2.EndPoint = point_ref_2
        
            Set line_ref_2_3 = factory2D1.CreateLine(ponto, -ponto, ponto, ponto)
            line_ref_2_3.ReportName = 8
            line_ref_2_3.StartPoint = point_ref_2
            line_ref_2_3.EndPoint = point_ref_3
            
            Set line_ref_3_4 = factory2D1.CreateLine(-ponto, ponto, ponto, ponto)
            line_ref_3_4.ReportName = 9
            line_ref_3_4.StartPoint = point_ref_4
            line_ref_3_4.EndPoint = point_ref_3
            
            Set line_ref_4_1 = factory2D1.CreateLine(-ponto, -ponto, -ponto, ponto)
            line_ref_4_1.ReportName = 10
            'line_ref_4_1.Construction = True
            line_ref_4_1.StartPoint = point_ref_1
            line_ref_4_1.EndPoint = point_ref_4
    
            ' Create Reference lines and constraints
            Set reference_line_ref_1_2 = part1.CreateReferenceFromObject(line_ref_1_2)
            Set reference_line_ref_2_3 = part1.CreateReferenceFromObject(line_ref_2_3)
            Set reference_line_ref_3_4 = part1.CreateReferenceFromObject(line_ref_3_4)
            Set reference_line_ref_4_1 = part1.CreateReferenceFromObject(line_ref_4_1)
            
            Set electrode_constraints = standard_body_sketch1.Constraints

            Set constraint_toto_2 = electrode_constraints.AddBiEltCst(catCstTypeDistance, point_ref11, reference_line_ref_2_3)
            Set constraint_toto_3 = electrode_constraints.AddBiEltCst(catCstTypeDistance, point_ref13, reference_line_ref_3_4)
            Set constraint_toto_4 = electrode_constraints.AddBiEltCst(catCstTypeDistance, reference_line_ref_4_1, point_ref12)
            Set constraint_toto_1 = electrode_constraints.AddBiEltCst(catCstTypeDistance, reference_line_ref_1_2, point_ref14)

            Dim length1 As Dimension
            Set length1 = constraint_toto_1.Dimension
            length1.Value = 0
            Dim length2 As Dimension
            Set length2 = constraint_toto_2.Dimension
            length2.Value = 0
            Dim length3 As Dimension
            Set length3 = constraint_toto_3.Dimension
            length3.Value = 0
            Dim length4 As Dimension
            Set length4 = constraint_toto_4.Dimension
            length4.Value = 0
            
            standard_body_sketch1.CloseEdition
            part1.Update

'----------------------------------------------------------------------------------------------------------------------------------
' Creation of the Max Z and Min Z planes
'----------------------------------------------------------------------------------------------------------------------------------

            Dim plan_inferieur As HybridShapePlaneOffsetPt
            Dim plan_origin As HybridShapePlane2Lines
            Dim Origin_line_1 As Reference
            Set Origin_line_1 = part1.CreateReferenceFromObject(line_HDirection)
            Dim Origin_line_2 As Reference
            Set Origin_line_2 = part1.CreateReferenceFromObject(line_VDirection)
            Set plan_origin = hybridShapeFactory1.AddNewPlane2Lines(Origin_line_1, Origin_line_2)
            Dim ref_plan_origin As Reference
            Set ref_plan_origin = part1.CreateReferenceFromObject(plan_origin)
            Set Ref6 = part1.CreateReferenceFromObject(HybridShapeExtremum6)
            Set plan_inferieur = hybridShapeFactory1.AddNewPlaneOffsetPt(ref_plan_origin, point_ref6)
            hybridBody2.AppendHybridShape plan_inferieur
            part1.InWorkObject = plan_inferieur

            Dim plan_superieur As HybridShapePlaneOffsetPt
            Set Ref5 = part1.CreateReferenceFromObject(HybridShapeExtremum5)
            Set plan_superieur = hybridShapeFactory1.AddNewPlaneOffsetPt(ref_plan_origin, point_ref5)
            hybridBody2.AppendHybridShape plan_superieur
            part1.InWorkObject = plan_superieur

            part1.Update
            
'----------------------------------------------------------------------------------------------------------------------------------
' Creates the line that sweeps around the XY Sketch boundary
'----------------------------------------------------------------------------------------------------------------------------------

            Dim Point_inf As HybridShapePointCoord
            Set Point_inf = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, point_ref6)
            hybridBody2.AppendHybridShape Point_inf
            Dim ref_point_inf As Reference
            Set ref_point_inf = part1.CreateReferenceFromObject(Point_inf)

            Dim proj_pt_inf As HybridShapeProject
            Set proj_pt_inf = hybridShapeFactory1.AddNewProject(point_ref6, plan_superieur)
            hybridBody2.AppendHybridShape proj_pt_inf
            part1.InWorkObject = proj_pt_inf

            Dim Point_sup As HybridShapePointCoord
            Set Point_sup = hybridShapeFactory1.AddNewPointCoordWithReference(0, 0, 0, proj_pt_inf)
            hybridBody2.AppendHybridShape Point_sup
            Dim ref_point_sup As Reference
            Set ref_point_sup = part1.CreateReferenceFromObject(Point_sup)

            Dim line_guide As HybridShapeLinePtPt
            Set line_guide = hybridShapeFactory1.AddNewLinePtPt(ref_point_sup, ref_point_inf)
            hybridBody2.AppendHybridShape line_guide
            part1.InWorkObject = line_guide
            Set ref_guideline = part1.CreateReferenceFromObject(line_guide)

            Dim oStart As Length
            Set oStart = line_guide.BeginOffset
            oStart.Value = 1
            Dim oEnd As Length
            Set oEnd = line_guide.EndOffset
            oEnd.Value = 1

            Set constraints_for_z = part1.Constraints
            Set constraint_dz = constraints_for_z.AddMonoEltCst(catCstTypeLength, ref_guideline)
            Set length_dz = constraint_dz.Dimension
            
            part1.Update

'----------------------------------------------------------------------------------------------------------------------------------
' Second Sketch, basically the XY boundary sketch placed down to Min Z
'----------------------------------------------------------------------------------------------------------------------------------

            Set sketches2 = hybridBody1.HybridSketches
            Set standard_body_sketch2 = sketches2.add(plan_inferieur)

            Set factory2D2 = standard_body_sketch2.OpenEdition()
            Set geometricElements2 = standard_body_sketch2.GeometricElements
            Set axis2D1 = geometricElements1.Item("AbsoluteAxis")

            pont = 200000
            Set point_ref1_1 = factory2D2.CreatePoint(-pont, -pont)
            Set point_ref1_2 = factory2D2.CreatePoint(pont, -pont)
            Set point_ref1_3 = factory2D2.CreatePoint(pont, pont)
            Set point_ref1_4 = factory2D2.CreatePoint(-pont, pont)
    
            Set line_ref1_1_2 = factory2D2.CreateLine(-pont, -pont, pont, -pont)
            line_ref1_1_2.StartPoint = point_ref1_1
            line_ref1_1_2.EndPoint = point_ref1_2
    
            Set line_ref1_2_3 = factory2D2.CreateLine(pont, -pont, pont, pont)
            line_ref1_2_3.StartPoint = point_ref1_2
            line_ref1_2_3.EndPoint = point_ref1_3
    
            Set line_ref1_3_4 = factory2D2.CreateLine(-pont, pont, pont, pont)
            line_ref1_3_4.StartPoint = point_ref1_4
            line_ref1_3_4.EndPoint = point_ref1_3
    
            Set line_ref1_4_1 = factory2D2.CreateLine(-pont, -pont, -pont, pont)
            line_ref1_4_1.StartPoint = point_ref1_1
            line_ref1_4_1.EndPoint = point_ref1_4

            Set reference_line_ref1_1_2 = part1.CreateReferenceFromObject(line_ref1_1_2)
            Set reference_line_ref1_2_3 = part1.CreateReferenceFromObject(line_ref1_2_3)
            Set reference_line_ref1_3_4 = part1.CreateReferenceFromObject(line_ref1_3_4)
            Set reference_line_ref1_4_1 = part1.CreateReferenceFromObject(line_ref1_4_1)

            Set reference_line_ref_1_2 = part1.CreateReferenceFromObject(line_ref_1_2)
            Set reference_line_ref_2_3 = part1.CreateReferenceFromObject(line_ref_2_3)
            Set reference_line_ref_3_4 = part1.CreateReferenceFromObject(line_ref_3_4)
            Set reference_line_ref_4_1 = part1.CreateReferenceFromObject(line_ref_4_1)

            Set proj_1_2 = factory2D2.CreateProjection(reference_line_ref_1_2)
            Set proj_2_3 = factory2D2.CreateProjection(reference_line_ref_2_3)
            Set proj_3_4 = factory2D2.CreateProjection(reference_line_ref_3_4)
            Set proj_4_1 = factory2D2.CreateProjection(reference_line_ref_4_1)

            Set ref_line_sk1_1_2 = part1.CreateReferenceFromObject(proj_1_2)
            Set ref_line_sk1_2_3 = part1.CreateReferenceFromObject(proj_2_3)
            Set ref_line_sk1_3_4 = part1.CreateReferenceFromObject(proj_3_4)
            Set ref_line_sk1_4_1 = part1.CreateReferenceFromObject(proj_4_1)
    
            Set electrode_constraints = standard_body_sketch2.Constraints
            Set constraint_toto_11 = electrode_constraints.AddBiEltCst(catCstTypeDistance, reference_line_ref1_1_2, ref_line_sk1_1_2)
            Set constraint_toto_12 = electrode_constraints.AddBiEltCst(catCstTypeDistance, ref_line_sk1_2_3, reference_line_ref1_2_3)
            Set constraint_toto_13 = electrode_constraints.AddBiEltCst(catCstTypeDistance, ref_line_sk1_3_4, reference_line_ref1_3_4)
            Set constraint_toto_14 = electrode_constraints.AddBiEltCst(catCstTypeDistance, reference_line_ref1_4_1, ref_line_sk1_4_1)
            'Dim length11 As Dimension
            Set length11 = constraint_toto_11.Dimension
            length11.Value = 1
            Dim length12 As Dimension
            Set length12 = constraint_toto_12.Dimension
            length12.Value = 1
            Dim length13 As Dimension
            Set length13 = constraint_toto_13.Dimension
            length13.Value = 1
            Dim length14 As Dimension
            Set length14 = constraint_toto_14.Dimension
            length14.Value = 1
            
            standard_body_sketch2.CloseEdition
            part1.Update
            
'----------------------------------------------------------------------------------------------------------------------------------
' Offset from Sketch2, using the Relations so you can change the offsets
'----------------------------------------------------------------------------------------------------------------------------------

            Set sketches3 = hybridBody1.HybridSketches
            Set standard_body_sketch3 = sketches3.add(plan_inferieur)
            Set factory2D3 = standard_body_sketch3.OpenEdition()
            Set geometricElements3 = standard_body_sketch3.GeometricElements
            Set axis2D1 = geometricElements1.Item("AbsoluteAxis")

            Set reference_line_ref1_1_2 = part1.CreateReferenceFromObject(line_ref1_1_2)
            Set reference_line_ref1_2_3 = part1.CreateReferenceFromObject(line_ref1_2_3)
            Set reference_line_ref1_3_4 = part1.CreateReferenceFromObject(line_ref1_3_4)
            Set reference_line_ref1_4_1 = part1.CreateReferenceFromObject(line_ref1_4_1)
            
            Set proj1_1_2 = factory2D3.CreateProjection(reference_line_ref1_1_2)
            Set proj1_2_3 = factory2D3.CreateProjection(reference_line_ref1_2_3)
            Set proj1_3_4 = factory2D3.CreateProjection(reference_line_ref1_3_4)
            Set proj1_4_1 = factory2D3.CreateProjection(reference_line_ref1_4_1)

            Set ref_proj1_1_2 = part1.CreateReferenceFromObject(proj1_1_2)
            Set ref_proj1_2_3 = part1.CreateReferenceFromObject(proj1_2_3)
            Set ref_proj1_3_4 = part1.CreateReferenceFromObject(proj1_3_4)
            Set ref_proj1_4_1 = part1.CreateReferenceFromObject(proj1_4_1)

            Set constraints_dim = standard_body_sketch3.Constraints
            Set constraint_dx = constraints_dim.AddMonoEltCst(catCstTypeLength, ref_proj1_1_2)
            Set constraint_dy = constraints_dim.AddMonoEltCst(catCstTypeLength, ref_proj1_2_3)
            Set length_dx = constraint_dx.Dimension
            dx_value = length_dx.Value
            Set length_dy = constraint_dy.Dimension
            dy_value = length_dy.Value

            standard_body_sketch3.CloseEdition
            part1.Update

            ' Create the offset parameters
            Dim string_1 As String
            string_1 = "Offset_Bbox_Max_X." & j
            Dim string_2 As String
            string_2 = "Offset_Bbox_Min_X." & j
            Dim string_3 As String
            string_3 = "Offset_Bbox_Max_Y." & j
            Dim string_4 As String
            string_4 = "Offset_Bbox_Min_Y." & j
            Dim string_5 As String
            string_5 = "Offset_Bbox_Max_Z." & j
            Dim string_6 As String
            string_6 = "Offset_Bbox_Min_Z." & j
            Dim string_7 As String
            string_7 = "Bbox_dx." & j
            Dim string_8 As String
            string_8 = "Bbox_dy." & j
            Dim string_9 As String
            string_9 = "Bbox_dz." & j

            Dim Offset_Bbox_Max_X As RealParam
            Set Offset_Bbox_Max_X = part1.Parameters.CreateDimension(string_1, "Length", 0)
            Dim Offset_Bbox_Min_X As RealParam
            Set Offset_Bbox_Min_X = part1.Parameters.CreateDimension(string_2, "Length", 0)
            Dim Offset_Bbox_Max_Y As RealParam
            Set Offset_Bbox_Max_Y = part1.Parameters.CreateDimension(string_3, "Length", 0)
            Dim Offset_Bbox_Min_Y As RealParam
            Set Offset_Bbox_Min_Y = part1.Parameters.CreateDimension(string_4, "Length", 0)
            Dim Offset_Bbox_Max_Z As RealParam
            Set Offset_Bbox_Max_Z = part1.Parameters.CreateDimension(string_5, "Length", 0)
            Dim Offset_Bbox_Min_Z As RealParam
            Set Offset_Bbox_Min_Z = part1.Parameters.CreateDimension(string_6, "Length", 0)
            Set Bbox_dx_hidden = part1.Parameters.CreateDimension(string_7, "Length", dx_value)
            Set Bbox_dy_hidden = part1.Parameters.CreateDimension(string_8, "Length", dy_value)
            Set Bbox_dz_hidden = part1.Parameters.CreateDimension(string_9, "Length", length_dz.Value)
            Bbox_dx_hidden.Hidden = True
            Bbox_dy_hidden.Hidden = True
            Bbox_dz_hidden.Hidden = True
            Set Bbox_dx = part1.Parameters.CreateDimension(string_7, "Length", 0)
            Set Bbox_dy = part1.Parameters.CreateDimension(string_8, "Length", 0)
            Set Bbox_dz = part1.Parameters.CreateDimension(string_9, "Length", 0)
            
            Dim Formula_1 As Formula
            Set Formula_1 = part1.Relations.CreateFormula("formula_Bbox_1." & j, "", length14, "Offset_Bbox_Min_X." & j)
            Dim Formula_2 As Formula
            Set Formula_2 = part1.Relations.CreateFormula("formula_Bbox_2." & j, "", length12, "Offset_Bbox_Max_X." & j)
            Dim Formula_3 As Formula
            Set Formula_3 = part1.Relations.CreateFormula("formula_Bbox_4." & j, "", length11, "Offset_Bbox_Min_Y." & j)
            Dim Formula_4 As Formula
            Set Formula_4 = part1.Relations.CreateFormula("formula_Bbox_4." & j, "", length13, "Offset_Bbox_Max_Y." & j)
            Dim Formula_5 As Formula
            Set Formula_5 = part1.Relations.CreateFormula("formula_Bbox_5." & j, "", oEnd, " Offset_Bbox_Min_Z." & j)
            Dim Formula_6 As Formula
            Set Formula_6 = part1.Relations.CreateFormula("formula_Bbox_6." & j, "", oStart, " Offset_Bbox_Max_Z." & j)
            Dim Formula_7 As Formula
            Set Formula_7 = part1.Relations.CreateFormula("formula_Bbox_7." & j, "", Bbox_dx, "Bbox_dx." & j & "+Offset_Bbox_Min_X." & j & "+Offset_Bbox_Max_X." & j & "-2mm")
            Dim Formula_8 As Formula
            Set Formula_8 = part1.Relations.CreateFormula("formula_Bbox_8." & j, "", Bbox_dy, "Bbox_dy." & j & "+Offset_Bbox_Min_Y." & j & "+Offset_Bbox_Max_Y." & j & "-2mm")
            Dim Formula_9 As Formula
            Set Formula_9 = part1.Relations.CreateFormula("formula_Bbox_9." & j, "", Bbox_dz, "Bbox_dz." & j & "+Offset_Bbox_Min_Z." & j & "+Offset_Bbox_Max_Z." & j & "-2mm")

'----------------------------------------------------------------------------------------------------------------------------------
' Sweep the Z line around the XY boundary.  This will be closed
'----------------------------------------------------------------------------------------------------------------------------------
                
            Set sweepref_1 = part1.CreateReferenceFromObject(standard_body_sketch3)
            Set guide1 = part1.CreateReferenceFromObject(line_guide)
            Dim sweep1 As HybridShapeSweepExplicit
            Set sweep1 = hybridShapeFactory1.AddNewSweepExplicit(sweepref_1, guide1)
            hybridBody2.AppendHybridShape sweep1
            part1.InWorkObject = sweep1
            part1.Update

            ' Close the Sweep
            Set shapeFactory1 = part1.ShapeFactory
            Set hybridBodies1 = body1.hybridBodies
            Set hybridBody1 = hybridBodies1.Item("definition_points")
            Dim hybridShapes1 As HybridShapes
            Set hybridShapes1 = hybridBody1.HybridShapes
            
            Dim refer1 As Reference
            Set refer1 = part1.CreateReferenceFromObject(sweep1)
    
            Dim closeSurface1 As CloseSurface
            Set closeSurface1 = shapeFactory1.AddNewCloseSurface(refer1)
            closeSurface1.Name = "BoundingBox"
            part1.Update

            SELECTION.Clear
            SELECTION.add hybridBody1
            SELECTION.VisProperties.SetShow catVisPropertyNoShowAttr
            SELECTION.Clear
            SELECTION.add body1
            SELECTION.VisProperties.SetRealColor 0, 0, 0, 0
            SELECTION.VisProperties.SetRealOpacity 150, 1
            SELECTION.VisProperties.SetRealWidth 2, 1
            part1.Update
            axissyst.Name = "Bounding Box Axis." & j
            
        Else
            MsgBox "The active document must be a CATPart"
        End If

    End If

End Sub

work around on message boxes

 

[jzecha]

Thanks for the quick reply.
The Macro will run, but some of my parts are very complex with no straight edges to create an axis off of.
When I try to run the Macro off of the axis i created, i get a bounding box that is nothing like my part.
Any advice on how to attack this problem?

 

[ferdo]

This macro was done with the purpose to create a bounding box of a CATPart, no mater how complex is it. The macro is replacing somehow the Rough Stock command in GSD. This command is available only if you have a NC license (hope I'm not doing a mistake, if yes, please correct me).

There are a lot of threads about this subject, you can search the forum, the rough stock command is working like Measure Inertia command and this is not always the best choice, the volume created is not always the minimum (hope you are looking for this solution and not something else).

With the macro, depending on how you choose the axis, you can have a smaller volume then measure inertia, especially for complex parts (I just notice that you have to create the axis first)

All what you have to do is to compare the volume resulting from BBLx * BBLy * BBLz for both solutions.

The best example which I had are parts done with sheet metal design license. If you want the bounding box for an unfolded part you have to obtain the minimum area (BBLx * BBLy , for example) which for sure you will not obtain every time with measure inertia command.

It would be great if you could post here a sample dumb part to see what you want in fact. Anyway, hope the pictures attached are good enough to explain what was going on.

JeniaL, star from me for your work.

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

- EU

 

[JeniaL]

Ferdo you are right about NC license. i don't know who is a an author of this macro but i converted this to vb and changed some message boxes for my purposes. thanks to an author.
he bounding box action also can be recorded with macro recorder. extremum point command should be used. axis system must be defined before.

@ jzecha upload catia file.. this macro works pretty well with very complex shapes.