pycatia.in_interfaces.selection

Module initially auto generated using V5Automation files from CATIA V5 R28 on 2020-07-03 17:02:05.216737

Warning

The notes denoted “CAA V5 Visual Basic Help” are to be used as reference only. They are there as a guide as to how the visual basic / catscript functions work and thus help debugging in pycatia.

class pycatia.in_interfaces.selection.Selection(com_object, child_object=<class 'pycatia.in_interfaces.selected_element.SelectedElement'>)

Note

CAA V5 Visual Basic Help (2020-07-03 17:02:05.216737)

System.IUnknown
System.IDispatch
System.CATBaseUnknown
System.CATBaseDispatch
System.AnyObject
Selection

Represents the selection.
The Selection object contains the features the end user selected, usually with
the mouse, and which are candidates as subjects for the next
action.

A feature possess parent objects in the specification tree (hierarchy). For
example, the Pad below possess parent objects in the specification
tree:

+——–+
!Product3!
+——–+
!
+- Product2 (Product2.1)
! !
! +- Product1 (Product1.1)
! !
! +- Part1 (Part1.1)
! !
! +- Part1
! !
! +- PartBody
! !
+——————+
! +- Pad.1 ! Selected feature
!
! !
+——————+
! +- Sketch.1
+- Part2 (Part2.1)


For a given selected feature, its parent objects which are exposed to
automation can be accessed through a recursive call to the AnyObject.Parent
property. When a given feature is selected, there are three
possibilities:

The feature is exposed to automation (a Pad for example, this is the common
case): the feature can be accessed by all Selection object
methods
The feature is not exposed to automation, but at least one of its parent
objects is exposed to automation (a DMU Navigator URL for example: the
Hyperlink is not exposed to automation, but the root Product, which contains
the Hyperlink, is exposed to automation):
no access is given to the feature through the Count2 and Item2 methods
of the Selection object
nevertheless, the first parent object of the feature, which is exposed
to automation (the root Product in our example) can be accessed through the
Item2 and Count2 methods
The Search, Delete, VisProperties, Copy, Cut, Paste and PasteSpecial
methods of the Selection object, take into account the
feature.
For example, if the user:
Puts a DMU Navigator URL in the clipboard
Runs a script calling the PasteSpecial method
then, during the paste, the DMU Navigator URL will be
pasted
The feature is not exposed to automation, and he has no parent object which
is exposed to automation (a ResourcesList object of a .CATProcess for
example):
no access is given to the feature through the Count2 and Item2 methods
of the Selection object
no access is given neither to any parent object of the feature through
the Item2 and Count2 methods
The Search, Delete, VisProperties, Copy, Cut, Paste and PasteSpecial
methods of the Selection object take into account the
feature.
For example, if the user:
Go to the “DPM - Process and Resource Definition”
workshop
Puts a ResourcesList object in the clipboard
Runs a script calling the Selection.PasteSpecial
method
then, during the paste, the ResourcesList object will be
pasted.

Note: The Selection object can be accessed through the Document.Selection
property . However, when the active window contains the tree described above,
the Selection object to use is the one associated to the Product3 Document ,
which can be accessed through the application of the Document.Selection to this
document. You will, for example, determine the Selection object the following
way:

Set ActiveProductDocument = CATIA.ActiveDocument
Set Product3 = ActiveProductDocument.Product
Set Product3Products = Product3.Products
Set Product2Dot1 = Product3Products.Item(“Product2.1”) : Set Product2 = Product2Dot1.ReferenceProduct
Set ProductDocument2 = Product2.Parent
Set Product2Products = Product2.Products
Set Product1Dot1 = Product2Products.Item(“Product1.1”) : Set Product1 = Product1Dot1.ReferenceProduct
Set ProductDocument1 = Product1.Parent
Set Product1Products = Product1.Products
Set Part1Dot1 = Product1Products.Item(“Part1.1”) : Set Part1 = Part1Dot1.ReferenceProduct
Set PartDocument1 = Part1.Parent
Set Selection = ActiveProductDocument.Selection


Another Selection object, such as:

Set ProductDocument2Selection = ProductDocument2.Selection
Set ProductDocument1Selection = ProductDocument1.Selection
Set PartDocument1Selection = PartDocument1.Selection


(lets take ProductDocument2Selection for example) can only be used if, among
the different Window , there is at least one whose root Document is
ProductDocument2 . Otherwise, results are unpredictable.
add(i_object: AnyObject) → None

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Sub Add(AnyObject iObject)

Creates a SelectedElement object which Value property is the given
automation object, and adds it to the selection.
Note: In a product structure aggregating a “Part1 (Part1.1)” Part document,
if you double-clic Part1 in the spectification tree:

the “Part Design” workbench becomes active
the Part1 node is inside a blue button

Here, Part1 is the UI Active Object.
Some editors, such as CatalogDocument editors, do not possess any UI Active
Object.
When this method is used in a CATAnalysis context, a CATPart (such as Part1
in our example) must be UI active. Otherwise, Selection.Add does not work
correctly (the 3D is not highlighted properly).
Role: Creates a SelectedElement object and adds it to the current
selection. Depending on the type of the parent Document of the Selection
object:

if it is one of the following:
CATIAPartDocument
CATIADrawingDocument
CATIAMaterialDocument
CATIAAnalysisDocument
CATIAFunctionalDocument
then, regarding the created SelectedElement , the SelectedElement.Value
property will be equal to iObject
Otherwise:
first case: the specification tree contains a
path:
whose leaf node is iObject
the UI Active Object belongs to the path
then, the method will create a SelectedElement object corresponding
to this path.
Otherwise: the method will create a SelectedElement object
corresponding to the first path, in the specification tree, whose leaf node is
iLeafNode

Example:
This example creates a SelectedElement object, which Value property is
the ObjectToAdd automation object, the SelectedElement being added to the
current selection.

CATIA.ActiveDocument.Selection.Add(ObjectToAdd)
Parameters:

i_object (AnyObject) –

Return type:

None

clear() → None

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Sub Clear()

Clears the selection.

Example:
This example clears the selection. The selection is then
empty.

CATIA.ActiveDocument.Selection.Clear()
Return type:

None

copy() → None

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Sub Copy()

Copies, in a copy and paste operation.
Role: Puts the contents of the selection in the clipboard, but leaves the
selected elements in the document, and clears the selection. This is the
programming equivalent of the Copy command from the Edit
menu.
Note: The method (and the script execution) fails if one of the following
errors occurs:

The CSO is empty. The Copy operation could not be
performed.
No CSO element remains after the filtering through the UI active
object. The Copy operation could not be performed.

Note: If a selected feature is not exposed to automation, it will be copied
into the clipboard all the way.

Example:
This example copies, in a copy and paste operation. A selected DMU
Navigator URL will be put into the clipboard although it is not exposed to
automation.

CATIA.ActiveDocument.Selection.Copy()
Return type:

None

property count: int

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384)
o Property Count() As long (Read Only)

Deprecated:
V5R16 #Count2 . The Count and Item Methods have been replaced by the
Count2 and Item2 methods because they did not process correctly features which
are not exposed to automation (such as a ResourcesList feature of a .CATProcess
document).
Return type:

int

property count2: int

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384)
o Property Count2() As long (Read Only)

Returns the number of SelectedElement objects contained by the current
selection.
Role: This method returns the number of SelectedElement objects contained
by the Selection. The Value property of a given SelectedElement object is an
automation object associated to a selected feature.
Return type:

int

cut() → None

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Sub Cut()

Cuts, in a cut and paste operation.
Role: Puts the contents of the selection in the clipboard, and removes the
selected elements from the document, and clears the selection. This is the
programming equivalent of the Cut command from the Edit
menu.
Note: The method (and the script execution) fails if one of the following
errors occurs:

The CSO is empty. The Cut operation could not be
performed.
No CSO element remains after the filtering through the UI active
object. The Cut operation could not be performed.

Note: If a selected feature is not exposed to automation, it will be copied
into the clipboard and removed from the document all the
way.

Example:
This example cuts, in a cut and paste opertation. A selected DMU
Navigator URL will be put into the clipboard and removed from the document,
although it is not exposed to automation.

CATIA.ActiveDocument.Selection.Cut()
Return type:

None

delete() → None

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Sub Delete()

Deletes all selected objects.
Role: For all the SelectedElement objects contained by the selection, the
SelectedElement.Value automation object is deleted from the
document.
Note: If a selected feature is not exposed to automation, it will deleted
all the way.

Example:
This example deletes all the selected objects. A selected DMU Navigator
URL will be removed from the document, although it is not exposed to
automation.

CATIA.ActiveDocument.Selection.Delete()
Return type:

None

filter_correspondence(i_filter_type: tuple) → bool

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func FilterCorrespondence(CATSafeArrayVariant iFilterType) As
boolean

Specifies if the automation objects appearing as Value property of
SelectedElement objects fit a given filter.
Role: FilterCorrespondence filters the selection with respect to provided
automation types. The use of this method coupled with the use of the
SelectElement2 will enable to offer a multi-selection written programmatically,
which is the common way to write multi-selection is CATIA.
It will enable, for example, to write a script reproducing the
functionalities of the “Fillet” command of the “Part Design”
workbench.
This method, called before a loop onto SelectElement2 calls, will enable if
all the selection objects correspond to the filter (which will be the same as
the filter given to SelectElement2 ), to take them into account, and,
otherwise, to clear the selection.
This multi-selection written programmatically will generally be used
coupled with the fact that already selected elements remain selected during the
selections.

Parameters:

iFilterType
An array of strings constants to be used as a filter for the kind
of element to which current selection object must correspond. See the
iFilterType parameter of the

SelectElement2 method.
oAllFit
All current selection objects fit the iFilterType filter, i.e.
regarding each of the current selection objects, they all fit one of the
iFilterType string constant.
Example:

The following example scripts an edge fillet creation command. It
supposes that a part is currently edited,
containing a Pad. It loops onto the following:




it asks the end user to select an edge (see

TriDimFeatEdge ). If the selected edge has not already been selected, the
selected edge is added to the selection, otherwise it is removed from the
selection
it asks the end user if another edge has to be selected
until the answer of the user to the preceding question is
no.
Then, it creates an edge fillet (see ConstRadEdgeFillet ) taking into
account all the selected edges as fillet specifications.

Note: The edges which were selected before the script execution are taken
into account. Nevertheless, if, before the script execution, the selection
contained an object which was not a TriDimFeatEdge element, the selection is
cleared before the first selection proposal.
Note: During the selection of a given edge, the edges already selected
remain highlighted.

Dim Document,Part,Selection,ShapeFactory,EdgeSaveAllocatedCount,EdgeIndex,
AllEdgesHaveBeenSelected,AllFit
Dim EdgeSaveCount,SelectedEdge,SelectedElementBelongsToSaveVariables,AlreadySelectedEdgeIndex
Dim OtherEdgeAnswer,Fillet
Set Document = CATIA.ActiveDocument : Set Part = Document.Part
: Set Selection = Document.Selection
Set ShapeFactory = Part.ShapeFactory
ReDim InputObjectType(0) : InputObjectType(0)=”TriDimFeatEdge” : EdgeSaveCount = 0
‘We determine if the selection contains an object which is not a
TriDimFeatEdge element
AllFit = Selection.FilterCorrespondence(InputObjectType)
‘If the selection contains an object which is not a TriDimFeatEdge element,
we clear the selection
if (Not AllFit) then Selection.Clear
EdgeSaveAllocatedCount = Selection.Count+10 : ReDim EdgeSave(EdgeSaveAllocatedCount-1)
‘We loop onto interactive selections
AllEdgesHaveBeenSelected = false
do while (Not AllEdgesHaveBeenSelected)
‘ We save the selection content in save variables.
‘ This corresponds to the fact that:
‘ - we want that, during the following call to SelectElement2, the
TriDimFeatEdge elements previously selected
‘ remain highlighted
‘ - this is done using the False value for the
iObjectSelectionBeforeCommandUsePossibility
‘ parameter of the SelectElement2 method, the selection containing the
TriDimFeatEdge elements. It requires that
‘ the selection content be saved
if (EdgeSaveAllocatedCount < Selection.Count) then
EdgeSaveAllocatedCount = EdgeSaveAllocatedCount + 10
: ReDim EdgeSave(EdgeSaveAllocatedCount-1)
end if
for EdgeIndex = 0 to Selection.Count2-1
Set EdgeSave(EdgeIndex) = Selection.Item2(EdgeIndex+1).Value
next
EdgeSaveCount = Selection.Count
‘ We propose to the user that he select an edge
Status=Selection.SelectElement2(InputObjectType,”Select an
edge”,false)
if (Status=”Cancel”) then
Selection.Clear : Exit Sub
end if
‘ We save the selected edge in a dedicated variable
Set SelectedEdge = Selection.Item2(1).Value
‘ We merge the selected element with the save variables, and put the
result in the selection.
‘ At first, we determine if the selected edge already belongs to the
EdgeSave array
EdgeIndex = 0 : SelectedElementBelongsToSaveVariables = False
do while ((EdgeIndex < EdgeSaveCount) And (Not
SelectedElementBelongsToSaveVariables))
if (EdgeSave(EdgeIndex).Name=SelectedEdge.Name)
then
SelectedElementBelongsToSaveVariables = True
AlreadySelectedEdgeIndex = EdgeIndex
end if
EdgeIndex = EdgeIndex + 1
loop
‘ Effective merge
if (Not SelectedElementBelongsToSaveVariables) then
‘ The selected element does not belong to the save variables. We add
the save variables to the selection
for EdgeIndex = 0 to EdgeSaveCount-1
Selection.Add EdgeSave(EdgeIndex)
next
else
‘ We remove the selected element from the save
variables
for EdgeIndex = AlreadySelectedEdgeIndex to EdgeSaveCount-2
Set EdgeSave(EdgeIndex) = EdgeSave(EdgeIndex+1)
next
EdgeSaveCount = EdgeSaveCount - 1
‘ We clear the selection
Selection.Clear
‘ We add the save variables to the selection
for EdgeIndex = 0 to EdgeSaveCount -1
Selection.Add EdgeSave(EdgeIndex)
next
end if
‘ We ask the end user if another edge has to be selected
OtherEdgeAnswer = msgbox (“do you want to select another edge?”,3,”Edge Fillet Definition”)
if (OtherEdgeAnswer = 2) then Exit Sub
if (OtherEdgeAnswer = 7) then AllEdgesHaveBeenSelected = true
loop
‘We create an edge fillet taking into account all the selected edges as
fillet specifications
if (Selection.Count > 0) then
Set Fillet = ShapeFactory.AddNewEdgeFilletWithConstantRadius(Selection.Item(1).Value, 1, 5.0)
Fillet.EdgePropagation = 1
for EdgeIndex = 2 to Selection.Count
Fillet.AddObjectToFillet
Selection.Item(EdgeIndex).Value
next
Part.Update : Selection.Clear : Selection.Add Fillet
end if
Parameters:

i_filter_type (tuple) –

Return type:

bool

find_object(i_object_type: str) → AnyObject

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func FindObject(CATBSTR iObjectType) As AnyObject

Finds an object in the current selection and deletes it from the
selection.
Role: Determines the first automation object specified in
SelectedElement.Value (for the SelectedElement objects contained in the current
selection), or which is a Parent (see AnyObject.Parent ) of the automation
object specified in SelectedElement.Value , which type is equal to the type
specified in input. It returns directly the automation object and deletes the
corresponding SelectedElement object from the current
selection.
Note: If the string specified in input is he “CATIAProduct” string, the
possible automation object specified in SelectedElement.LeafProduct is also
looked at.

Example:
This example searches a Pad object in the current selection and puts it
into FoundObject.

Dim FoundObject As AnyObject
Set FoundObject = CATIA.ActiveDocument.Selection.FindObject(“CATIAPad”)
Parameters:

i_object_type (str) –

Return type:

AnyObject

indicate_or_select_element_2d(i_message: str, i_filter_type: tuple, i_object_selection_before_command_use_possibility: bool, i_tooltip: bool, i_triggering_on_mouse_move: bool) → str

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func IndicateOrSelectElement2D(CATBSTR iMessage,
CATSafeArrayVariant iFilterType,
boolean iObjectSelectionBeforeCommandUsePossibility,
boolean iTooltip,
boolean iTriggeringOnMouseMove,
boolean oObjectSelected,
CATSafeArrayVariant oDocumentWindowLocation) As CATBSTR

Runs an interactive command enabling both indication and selection, 2D
version.
Role: IndicateOrSelectElement2D asks the end user to select either a
location into the window, or a feature (in the geometry or in the specification
tree).
During execution, when entering this method, the active document must be a
2D document. See Document.Indicate2D and SelectElement3

Parameters:

iMessage
A string which instructs the user that he must select a location
into the document window or select an object.
iFilterType
An array of strings constants defining the automation object types
with which the selection will be filtered.
iObjectSelectionBeforeCommandUsePossibility
Enables the script to support the possibility, for the user, to
select a required object before running the script. See


SelectElement2 .
iTooltip
Displays a tooltip as soon as an object is located under the mouse
without being selected.
iTriggeringOnMouseMove
Triggers as soon as a mouse move event is detected. This option beeing
set, oOutputState may be valued to “MouseMove”.
oObjectSelected
Flag précising if the user choosed the selection or the indication.

oDocumentWindowLocation
An array made of 2 doubles: X, Y - coordinates array of the location
the user specified in the document window. This parameter is valuated only if
oObjectSelected equals to false.
oOutputState
The state of the interactive command once IndicateOrSelectElement2D
returns. The possible values are the same than the values described regarding
the oOutputState parameter of the SelectElement2 method, except that the
“MouseMove” value can also be returned.
Example:

The following example suppose a drawing is currently edited. It
creates a point (see

Point2D ), and asks the end user to click to define the circle
center.
When it is done, as the mouse moves without clicking the left button, the
script determines the location into the drawing window, and the script creates
a temporary circle as a feedback.
A click into the document window or the selection of a point creates
definitively the circle (see Circle2D ) located at the specified location
(whether the location is a location into the drawing window or whether it is
the existing point location).

Dim Document,Selection,DrawingSheets,DrawingSheet,DrawingViews,WindowLocation(1),DrawingView,
Factory2D,Radius,Circle2D
Dim HardCodedPoint,Status,XCenter,YCenter,InputObjectType(0),TempCircleHasBeenCreatedAtLeastOnce,
ExistingPoint
Dim ObjectSelected
Set Document = CATIA.ActiveDocument : Set Selection = Document.Selection
: Set DrawingSheets = Document.Sheets
Set DrawingSheet = DrawingSheets.ActiveSheet : Set DrawingViews = DrawingSheet.Views
Set DrawingView = DrawingViews.ActiveView : Set Factory2D = DrawingView.Factory2D
‘We create a point
Set HardCodedPoint = Factory2D.CreatePoint(700.,400.)
HardCodedPoint.ReportName = 1 : HardCodedPoint.Construction = False
‘We propose to the user to click to define the circle
center
Status=Document.Indicate2D(“click to define the circle
center”,WindowLocation)
if (Status = “Cancel” Or Status = “Undo” Or Status = “Redo”) then Exit Sub
XCenter = WindowLocation(0) : YCenter = WindowLocation(1)
‘We propose to the user that he specify a location into the drawing window
or a point
InputObjectType(0)=”Point2D”
Status = “MouseMove” : TempCircleHasBeenCreatedAtLeastOnce = 0
Status=Selection.IndicateOrSelectElement2D(
“select a point or click to locate the circle radius point”, _
InputObjectType,false,false,true, _ObjectSelected,WindowLocation)
‘ We loop onto mouse moves without click
do while (Status = “MouseMove”)
if (TempCircleHasBeenCreatedAtLeastOnce) then
Selection.Add Circle2D : Selection.Delete
end if
Radius = Sqr(((WindowLocation(0)-XCenter)*(WindowLocation(0)-XCenter))+ _
((WindowLocation(1)-YCenter)*(WindowLocation(1)-YCenter)))
Set Circle2D = Factory2D.CreateClosedCircle(XCenter,YCenter,Radius)
TempCircleHasBeenCreatedAtLeastOnce = 1
Status=Selection.IndicateOrSelectElement2D(“select a point or click to
locate the circle radius point”, _
InputObjectType,false,false,true, _
ObjectSelected,WindowLocation)
loop
‘We go out if necessary
if (Status = “Cancel” Or Status = “Undo” Or Status = “Redo”) then
if (TempCircleHasBeenCreatedAtLeastOnce) then
Selection.Add Circle2D : Selection.Add HardCodedPoint : Selection.Delete
end if
Exit Sub
end if
‘We determine the possible selected point coordinates
if (ObjectSelected) then
Set ExistingPoint = Selection.Item2(1).Value : ExistingPoint.GetCoordinates WindowLocation
: Selection.Clear
end if
‘We clean-up the temporary circle
if (TempCircleHasBeenCreatedAtLeastOnce) then
Selection.Add Circle2D : Selection.Delete
end if
‘We create the circle
Radius = Sqr(((WindowLocation(0)-XCenter)*(WindowLocation(0)-XCenter))+ _
((WindowLocation(1)-YCenter)*(WindowLocation(1)-YCenter)))
Set Circle2D = Factory2D.CreateClosedCircle(XCenter,YCenter,Radius) : Selection.Add Circle2D
Parameters:

  • i_message (str) –

  • i_filter_type (tuple) –

  • i_object_selection_before_command_use_possibility (bool) –

  • i_tooltip (bool) –

  • i_triggering_on_mouse_move (bool) –

  • o_object_selected (bool) –

  • o_document_window_location (tuple) –

Return type:

str

indicate_or_select_element_3d(i_planar_geometric_object: AnyObject, i_message: str, i_filter_type: tuple, i_object_selection_before_command_use_possibility: bool, i_tooltip: bool, i_triggering_on_mouse_move: bool) → tuple

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func IndicateOrSelectElement3D(AnyObject
iPlanarGeometricObject,
CATBSTR iMessage,
CATSafeArrayVariant iFilterType,
boolean iObjectSelectionBeforeCommandUsePossibility,
boolean iTooltip,
boolean iTriggeringOnMouseMove,
boolean oObjectSelected,
CATSafeArrayVariant oWindowLocation2D,
CATSafeArrayVariant oWindowLocation3D) As CATBSTR

Runs an interactive command enabling both indication and selection, 3D
version.
Role: IndicateOrSelectElement3D asks the end user to select either a
location into the window, or a feature (in the geometry or in the specification
tree).
During execution, when entering this method, the active document must be a
3D document. See Document.Indicate3D and SelectElement3

Parameters:

iPlanarGeometricObject
A planar geometric object.
iMessage
A string which instructs the user that he must select a location
into the document window or select an object.
iFilterType
An array of strings constants defining the automation object types
with which the selection will be filtered.
iObjectSelectionBeforeCommandUsePossibility
Enables the script to support the possibility, for the user, to
select a required object before running the script. See


SelectElement2 .
iTooltip
Displays a tooltip as soon as an object is located under the mouse
without being selected.
iTriggeringOnMouseMove
Triggers as soon as a mouse move event is detected. This option being
set, oOutputState may be valued to “MouseMove”.
oObjectSelected
Flag precising if the user chose the selection or the indication.

oWindowLocation2D
X, Y - coordinates array of the location the user specified into the
document window. This parameter is valuated only if oObjectSelected equals to
false.
oWindowLocation3D
X, Y, Z - coordinates array of the location the user specified in the
document window. This parameter is valuated only if oObjectSelected equals to
false.
oOutputState
The state of the interactive command once IndicateOrSelectElement3D
returns. The possible values are the same than the values described regarding
the oOutputState parameter of the SelectElement2 method, except that the
“MouseMove” value can also be returned.
Example:

The following example suppose a part is currently edited, containing
a plane. It creates a point
(see

HybridShapePointOnPlane ), asks the end user to select a location into the
part window, onto the Plane.1 plane, or to select a point.
As the mouse moves without clicking the left button, the location into the
drawing window is determined, and the script creates a temporary point as a
feedback.
A click into the document window or the selection of a point creates
definitively the point (see HybridShapePointOnPlane ) located at the specified
location (whether the location is a location into the part window or whether it
is the existing point location).

Dim Document,Part,HybridShapeFactory,Selection,Body,HybridShapePlane,PlaneReference,
HardCodedPoint,Point
Dim InputObjectType(0),WindowLocation2D(1),WindowLocation3D(2),
TempPointHasBeenCreatedAtLeastOnce,Status
Dim ObjectSelected,ExistingPoint
Set Document = CATIA.ActiveDocument : Set Part = Document.Part
Set HybridShapeFactory = Part.HybridShapeFactory : Set Selection = Document.Selection
Set Body = Part.Bodies.Item(“PartBody”)
Set HybridShapePlane = Body.HybridShapes.Item(“Plane.1”)
Set PlaneReference = Part.CreateReferenceFromObject(HybridShapePlane)
‘We create a point
Set HardCodedPoint = HybridShapeFactory.AddNewPointOnPlane(PlaneReference,30.,30.)
Body.InsertHybridShape HardCodedPoint : Part.InWorkObject = HardCodedPoint : Part.Update
‘We propose to the user that he specify a location into the part window or
a point
InputObjectType(0)=”HybridShapePointOnPlane”
Status = “MouseMove” : TempPointHasBeenCreatedAtLeastOnce = 0 : Selection.Clear
Status=Selection.IndicateOrSelectElement3D(HybridShapePlane,”select a
point or click to locate the point”, _
InputObjectType,false,false,true, _
ObjectSelected,WindowLocation2D,WindowLocation3D)
‘ We loop onto mouse moves without click
do while (Status = “MouseMove”)
if (TempPointHasBeenCreatedAtLeastOnce) then
Selection.Add Point : Selection.Delete
end if
Set Point = HybridShapeFactory.AddNewPointOnPlane(PlaneReference,WindowLocation2D(0),
WindowLocation2D(1))
Body.InsertHybridShape Point : Part.InWorkObject = Point : Part.Update
TempPointHasBeenCreatedAtLeastOnce = 1
Status=Selection.IndicateOrSelectElement3D(HybridShapePlane,”select a
point or click to locate the point”, _
InputObjectType,false,false,true, _
ObjectSelected,WindowLocation2D,WindowLocation3D)
loop
‘We go out if necessary
if (Status = “Cancel” Or Status = “Undo” Or Status = “Redo”) then
if (TempPointHasBeenCreatedAtLeastOnce) then
Selection.Add Point : Selection.Add HardCodedPoint : Selection.Delete : Part.Update
end if
Exit Sub
end if
‘We determine the possible selected point coordinates
if (ObjectSelected) then
Set ExistingPoint = Selection.Item2(1).Value
WindowLocation2D(0) = ExistingPoint.XOffset.Value
WindowLocation2D(1) = ExistingPoint.YOffset.Value
Selection.Clear
end if
‘We clean up the temporary point
if (TempPointHasBeenCreatedAtLeastOnce) then
Selection.Add Point : Selection.Delete
end if
‘We create the point
Set Point = HybridShapeFactory.AddNewPointOnPlane(PlaneReference,WindowLocation2D(0),
WindowLocation2D(1))
Body.InsertHybridShape Point : Part.InWorkObject = Point : Part.Update
Parameters:

  • i_planar_geometric_object (AnyObject) –

  • i_message (str) –

  • i_filter_type (tuple) –

  • i_object_selection_before_command_use_possibility (bool) –

  • i_tooltip (bool) –

  • i_triggering_on_mouse_move (bool) –

Return type:

str

item(i_index: int) → SelectedElement

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func Item(long iIndex) As SelectedElement

Deprecated:
V5R16 #Item2 . The Count and Item Methods have been replaced by the
Count2 and Item2 methods because they did not process correctly features which
are not exposed to automation (such as a ResourcesList feature of a .CATProcess
document).
Parameters:

i_index (int) –

Return type:

SelectedElement

item2(i_index: int) → SelectedElement

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func Item2(long iIndex) As SelectedElement

Returns the iIndex-th SelectedElement object contained by the current
selection.
Role: Returns the iIndex-th SelectedElement object contained by the current
Selection. The Value property of the SelectedElement object is an automation
object associated to a selected feature.

Parameters:

iIndex
The index of the

SelectedElement object to return, 1≤iIndex≤Selection.Count2 .

oSelectedElement
The SelectedElement object
Example:

See the

SelectElement3 method first example.
Parameters:

i_index (int) –

Return type:

SelectedElement

items()
Returns:

[self.child_object()]

paste() → None

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Sub Paste()

Puts the contents of the clipboard in the document at the indicated
location.
Role: After the execution of the Paste method, there may be, among the
pasted features, some which are not exposed to automation. If the selected
feature after which the clipboard must be pasted is not exposed to automation,
the Paste will be done all the way.
Note: The method (and the script execution) fails if one of the following
errors occurs:

The CSO is empty. The Paste operation could not be
performed.
No CSO element remains after the filtering through the UI active
object. The Paste operation could not be performed.

Example:
This example pastes, in a cut, or copy, and paste operation. A selected
DMU Navigator URL will be put into the clipboard and removed from the document,
although it is not exposed to automation.

CATIA.ActiveDocument.Selection.Paste()
Return type:

None

paste_special(i_format: str) → None

Note

CAA V5 Visual Basic Help (2020-07-03 17:02:05.216737))
o Sub PasteSpecial(CATBSTR iFormat)

Puts the contents of the clipboard in the document at the indicated
location, according to the specified format.
Role: After the execution of the Paste method, there may be, among the
pasted features, some which are not exposed to automation. If the selected
feature after which the clipboard must be pasted is not exposed to automation,
the Paste will be done all the way.
Note: The method (and the script execution) fails if one of the following
errors occurs:

The CSO is empty. The PasteSpecial operation could not be
performed.
No CSO element remains after the filtering through the UI active
object. The PasteSpecial operation could not be
performed.


Formats are:

In all the containers
“CATIA_LINK_FORMAT” to paste “Catia Link Source”,
“OLE_LINK_FORMAT” to paste “Ole Link Source”,
“OLE_EMBED_FORMAT” to paste “Ole Embed Source”.


In a Part container
“CATPrtCont” to paste “As Specified In Part Document”,
“CATPrtResultWithOutLink” to paste “AsResult”,
“CATPrtResult” to paste “AsResultWithLink”,
“CATMaterialCont” to paste “As material”,
“AsMaterialLink” to paste “As material link”,
“CATMechProdCont” to paste “As specified in Assembly”,
“CATProdCont” to paste “As specified in Product
Structure”,
“CATIA_SPEC” to paste “CATIA_SPEC”,
“CATIA_RESULT” to paste “CATIA_RESULT”.


In a Product container
“CATProdCont” to paste “As specified in Product
Structure”,
“CATSpecBreakLink” to paste “Break Link”.


In a Process container
“SPPProcessCont” to paste “Simple paste”,
“SPP_I” to paste “Paste with Items”,
“SPP_R” to paste “Paste with Resources”,
“SPP_IR” to paste “Paste with Items and Resources”,
“SPPI_I” to paste “Paste with Items and entire
hierarchy”,
“SPPI_R” to paste “Paste with Resources and entire
hierarchy”,
“SPPI_IR” to paste “Paste with Items and Resources and entire
hierarchy”.


In a Material container
“CATMaterialCont” to paste “As material”,
“AsMaterialLink” to paste “As material link”.


In a Catalog container
“CATDescriptionFormat” to paste “As defined in catalog
instanciation”,
“CATCtlgChapterFormat” to paste “As defined in catalog
document”.


In a Rendering Scene container
“CATRscLightContainer” to paste “As light”,
“CATRscEnvironmentContainer” to paste “As
environment”,
“CATRscShootingContainer” to paste “As shooting”,
“CATRscTurntableContainer” to paste “As turntable”.


In a Deneb Resource Program container
“DNBProgCont” to paste “Resource Program”.


In a Behavior container
“Behaviors” to paste “Behaviors”.


In a CATCamera container
“CATCameraContainer” to paste “Camera”.


To know more about those formats, refer to the interactive
command.

Example:
This example pastes, in a cut, or copy, and paste special operation. A
selected DMU Navigator URL will be pasted from the clipboard at the specified
location, although it is not exposed to automation.

CATIA.ActiveDocument.Selection.PasteSpecial
“CATPrtResultWithOutLink”
Parameters:

i_format (str) –

Returns:

None

remove(i_index)

Note

CAA V5 Visual Basic Help (2020-07-03 17:02:05.216737))
o Sub Remove(long iIndex)

Deprecated:
V5R16 #Remove2 . This method does the same as the Remove2 method, but
it does know how to manage features which are not exposed to automation (such
as a ResourcesList feature of a .CATProcess document).
Parameters:

i_index (int) –

Returns:

None

remove2(i_index)

Note

CAA V5 Visual Basic Help (2020-07-03 17:02:05.216737))
o Sub Remove2(long iIndex)

Removes the iIndex-th SelectedElement object contained by the current
selection.
Role: Removes the iIndex-th SelectedElement object contained by the current
selection.

Parameters:

iIndex
The index of the

SelectedElement object to remove, 1≤iIndex≤Selection.Count2
.

Example:
This example removes the second SelectedElement object contained by
the current selection.

CATIA.ActiveDocument.Selection.Remove2(2)
Parameters:

i_index (int) –

Returns:

None

search(i_string_bstr)

Note

CAA V5 Visual Basic Help (2020-07-03 17:02:05.216737))
o Sub Search(CATBSTR iStringBSTR)

Finds an object in the document using the Edit/Search
grammar.
Role: Finds an object in the document using the Edit/Search grammar, and
fills the selection with the found objects. A criterium is created, based on
the Search grammar, which defines in addition the depth of the investigation
field.
Note: After the execution of the Search method, there may be, among the
selected features, some which are not exposed to
automation.

Example:
The following example searches the objects matching the following
criterium in all the document: Part.Sketcher.Color=’White’ . A selected DMU
Navigator URL put into the selection although it is not exposed to
automation.

CATIA.ActiveDocument.Selection.Search(“Part.Sketcher.Color=’White’,all”)
Parameters:

i_string_bstr (str) –

Return type:

None

select_element2(i_filter_type: tuple, i_message: str, i_object_selection_before_command_use_possibility: bool) → str

Note

CAA V5 Visual Basic Help (2020-07-03 17:02:05.216737))
o Func SelectElement2(CATSafeArrayVariant iFilterType,
CATBSTR iMessage,
boolean iObjectSelectionBeforeCommandUsePossibility) As
CATBSTR

Runs an interactive selection command.
Role: SelectElement2 asks the end user to select a feature (in the geometry
or in the specification tree) in a Window of the active Document . During the
selection, when the end user will move the mouse above a feature which maps the
given filter, the mouse pointer will be the “hand” cursor, and when end user
will move the mouse above a feature which does not map the given filter, the
mouse pointer will be the “no entry” cursor.

If iObjectSelectionBeforeCommandUsePossibility is equal to
False:
The end user is asked to interactively select an appropriate element.
When this is done, the Selection object is cleared, and filled with the
selected element.

If iObjectSelectionBeforeCommandUsePossibility is equal to
True:
SelectElement2 determines whether the automation objects specified in
SelectedElement.Value, for the SelectedElement objects contained in the current
selection, or one of the parents of the automation objects (see
AnyObject.Parent ) is an appropriate element:
If it is the case, no interaction is asked to the end user, the
Selection object is cleared, and filled with the appropriate
element.
Otherwise, the Selection object is cleared, and the end user is
asked to interactively select an appropriate element. When this is done, the
selection is filled with the selected element.
Note: The Selection object on which the Selection.SelectElement2 method
must be called must be the Selection object obtained the following
way:
determine the active document, for example, in the following
case:

Product3
!
+- Product2 (Product2.1)
! !
! ! +———————+
! +-!Product1 (Product1.1)!
! +———-+———-+
! !
! +- Part1 (Part1.1)

! !
! +- Part1
! !
! +- PartBody
! !
+——————+
! +- Pad.1 !
Selected feature !
! !
+——————+
! +- Sketch.1

+- Part2 (Part2.1)


it will be Product3
call the Document.Selection property onto this
document
Otherwise, results are unpredictable. Note: During the selection scan
to find an automation object, a “Product” string constant specified in
iFilterType will imply that SelectElement2 will also look at the possible
automation object specified in SelectedElement.LeafProduct
.

After a call to SelectElement2, if the return value equals to “Normal”, a
call to the Count2 method will return one, and a call to Item2(1) will return
the selected element.

Note: If the scripting language is Visual Basic for Applications or Visual
Basic 6 Development Studio, then, you have to know that the use of an
interactive selection method such as this one from a form (dialog box) method
requires some constraints regarding the content of an average form
method.
If your macro possess a form method which calls the SelectElement2 method,
then, the content of an average form method of your macro must begin by a test,
which checks that no form method is currently being executed and, otherwise, go
out of the method. This constraint enable to prevent that, during the execution
of the SelectElement2 method from a form method, when CATIA asks the end user
to select a feature:

the users select a dialog object of a form (CATIA going on asking the
end user to select a feature)
this selection trigger the corresponding form method
this run CATIA automation objects methods, CATIA going on asking the
end user to select a feature

which would lead to unpredictable results.
The code will be the following way:

- macro module main variables:
Dim AFormMethodIsBeingExecuted As Boolean
- form method calling SelectElement2:
Private Sub
FormPossessingOneMethodCallingSelectElement2_Click()
Dim InputObjectType(0), Status
AFormMethodIsBeingExecuted = True
InputObjectType(0)=”TriDimFeatEdge”
Status=Selection.SelectElement2(InputObjectType,”Select an
edge”,false)
AFormMethodIsBeingExecuted = False
End Sub
- average form method:
Private Sub AverageForm_Click()
If (AFormMethodIsBeingExecuted) Then Exit Sub
…
‘ content of the form method itself
…
End Sub

Parameters:

iFilterType
An array of strings constants defining the automation object types
with which the selection will be filtered. During the selection, when the end
user will move the mouse (above the geometry or the specification tree), if the
feature under the mouse does not map iFilterType, the cursor will be the “no
entry” cursor.
The resulting filter is a logical OR of the supplied strings
constants. For instance if the array contains two elements “Point” and “Line”,
when the end user will move the mouse above the geometry, if there is a feature
under a mouse, which is a

HybridShapePointCoord object (you have to know that the Point object is
a parent object of the HybridShapePointCoord object ), then, the cursor will be
a “hand” cursor. At the opposite, if there is a feature under a mouse, which is
neither a Point nor a Line, the cursor will be a “no entry”
cursor.

Beside the automation object names, the CATSelectionFilter value names
are supported.
iMessage
A string which instructs the user what to select. This string is
displayed in the message area located at the left of the power input area.

iObjectSelectionBeforeCommandUsePossibility
Enables the script to support the possibility, for the user, to select
a required object before running the script.

If the scripter:

writes a script calling SelectElement2, giving as iFilterType
parameter an array containing one string: “Pad”
for the first call to SelectElement2 made by the script, the
iObjectSelectionBeforeCommandUsePossibility is set to
True
the scripter associates the script to an Icon. He will proceed as
following:
in the Tools menu, select the Customize item. A window
appears.
select the Commands Tab. The window contains two
lists.
in the list on the left, select the Macros
value
select the “Show Properties” push button
select the button on the right of the Icon label. A window
containing a list of icons appears
select an Icon
select the Close button. The window containing the icon list
disappears
in the list on the right, push the key 1 of the mouse, the
cursor beeing on the macro to associate to an Icon. Then drag to a desired
Toolbar. The Icon has been added to the
Toolbar.


Then the user will be able to implement the following
scenario:

select a Pad
select the Icon mentioned above. This runs the
script.


During the execution of the script, the script will detect that the
selected Pad is required as input, and the first call to SelectElement2 will
not ask to the user to interactively select a Pad: the Pad selected before the
script execution will be taken.
Note:Regarding the features selected by the user (a Pad in the example
above), all the automation objects specified in SelectedElement.Value for the
current selection SelectedElement objects must be used: if an automation object
specified in SelectedElement.Value is not asked by the input filter, the
SelectElement2 method will ask the user to interactively select an appropriate
element.

A False value for the iObjectSelectionBeforeCommandUsePossibility parameter
may be used although the selection is not empty before entering the method.
This enables that, during the selection, the selected elements remain
highlighted.
Caution: After a call to SelectElement2 , the
iObjectSelectionBeforeCommandUsePossibility parameter being set to False, the
elements which were selected before the call to SelectElement2 are not any more
in the selection (unless the user selected one of them!). Consequently, such a
use of the False value for the iObjectSelectionBeforeCommandUsePossibility
parameter requires the following code:

save the selection content in save variables
call the SelectElement2 method, the
iObjectSelectionBeforeCommandUsePossibility parameter being set to
False
copy the selected element to a dedicated variable
merge the selected element with the save variables, and put the result
in the selection. This mean:
if the selected element does not belong to the save variables, add
the save variables to the selection
otherwise, remove the selected element from the save variables,
clear the selection and then, add the save variables to the
selection

oOutputState
The state of the selection command once SelectElement2 returns. It can
be either “Normal” (the selection has succeeded), “Cancel” (the user wants to
cancel the VB command, which must exit immediately), “Undo” or
“Redo”.
Note:The “Cancel” value is returned if one of the following cases
occured:

an external command has been selected
the ESCAPE key has been selected
another window has been selected, the window document beeing
another document than the current document

Caution:All scripts should exit (after the necessary cleanings) when
the “Cancel” value is returned.
If the script does not exit (beside the cleanings) when the “Cancel”
value is returned, but calls another interactive method such as SelectElement2
, and, during execution, the user select an external command (which triggers
the return of the “Cancel” value), then, the execution of the other interactive
method will display an error message.
Example:

The following example asks the end user to select a sketch (see


Sketch ) in the current window, and creates a Pad (see
ShapeFactory.AddNewPad ). If, before the script execution, a sketch was already
selected, it will be taken into account and the end user will ne be asked to
select a sketch.
Then, it asks the end user to select an edge of the pad, and creates an
edge fillet. Then, is asks the end user to select a 1-D entity whose geometry
is rectilinear (see CATSelectionFilter ), such as an edge of the
Pad.
Then, it asks the end user to select a pad face perpendicular to the 1-D
entity previously selected. Then, it creates a hole at the face selected point,
the hole direction being the direction of the 1-D selected
entity.
During the face selection, the 1-D entity previously selected is
highlighted.

Dim Document,Part,Selection,ShapeFactory,SketchHasBeenAcquiredAtLeastOnce,
EdgeHasBeenAcquiredAtLeastOnce
Dim FaceHasBeenAcquiredAtLeastOnce,MonoDimEntityHasBeenAcquiredAtLeastOnce,
FirstExtrudeNotFinished,FilletEdge
Dim PadNotFinished,Status,SketchForPad,Pad,FilletNotFinished,Fillet,
MonoDimEntityDeterminationNotFinished
Dim SelectedElement,MonoDimEntity,HoleNotFinished,PadFace,Hole,InputObjectType(0),
HoleLocation(2),MonoDimEntitySave
Dim SketchForPadPartBody
Set Document = CATIA.ActiveDocument : Set Part = Document.Part
Set Selection = Document.Selection
Set ShapeFactory = Part.ShapeFactory
SketchHasBeenAcquiredAtLeastOnce = False : EdgeHasBeenAcquiredAtLeastOnce = False
FaceHasBeenAcquiredAtLeastOnce = False : MonoDimEntityHasBeenAcquiredAtLeastOnce = False
FirstExtrudeNotFinished = True : PadNotFinished = True : ReDim SelectionAtBeginning(1)
‘We save the current selection content
ReDim SelectionAtBeginning(Selection.Count2)
for SelectionObjectIndex = 0 to Selection.Count2-1
Set SelectionAtBeginning(SelectionObjectIndex) = Selection.Item2(1).Value
next
SelectionAtBeginningLength = Selection.Count2
‘Feature creation
do while PadNotFinished
‘ We propose to the user that he select a sketch
InputObjectType(0)=”Sketch”
Status=Selection.SelectElement2(InputObjectType,”Select a
sketch”,true)
if ((Status = “Cancel”) Or (Status = “Undo”)) then
‘ We restore the selection to its initial content
Selection.Clear
for SelectionObjectIndex = 0 to SelectionAtBeginningLength-1
Selection.Add
SelectionAtBeginning(SelectionObjectIndex)
next
Exit Sub
elseif (Status = “Redo” And Not SketchHasBeenAcquiredAtLeastOnce ) then
‘ We do nothing: Redo has no meaning in this context
else
if (Status <> “Redo”) then Set SketchForPad = Selection.Item2(1).Value
SketchHasBeenAcquiredAtLeastOnce = True
‘ We determine the PartBody corresponding to the
Sketch
Set SketchForPadPartBody = SketchForPad.Parent.Parent
‘ We create the Pad
Set Pad = ShapeFactory.AddNewPad(SketchForPad,20.0)
Pad.SecondLimit.Dimension.Value = 0.0 : Part.Update
PadNotFinished = False
Selection.Clear
‘ We create the fillet and the hole
FilletNotFinished = True
do while (FilletNotFinished And Not
PadNotFinished)
‘ We propose to the user that he select an edge
InputObjectType(0)=”TriDimFeatEdge”
Status=Selection.SelectElement2(InputObjectType,”Select an
edge of the Pad”,false)
if (Status = “Cancel”) then
‘ We remove the pad, restore the selection to its initial
content and go out
Selection.Clear : Selection.Add(Pad) : Selection.Delete
Part.Update
Selection.Clear
for SelectionObjectIndex = 0 to SelectionAtBeginningLength-1
Selection.Add SelectionAtBeginning(SelectionObjectIndex)
next
Exit Sub
elseif (Status = “Redo” And Not EdgeHasBeenAcquiredAtLeastOnce ) then
‘ We do nothing: Redo has no meaning in this
context
elseif (Status = “Undo”) then
‘ We copy the sketch to the clipboard
Selection.Clear : Selection.Add(SketchForPad)
‘ We remove the pad
Selection.Clear : Selection.Add(Pad) : Selection.Delete : Part.Update
‘ We re-create the sketch
Selection.Clear : Selection.Add(SketchForPadPartBody) : Selection.Paste()
‘ We store the fact that the Pad is not finished
PadNotFinished = True
else
if (Status <> “Redo”) then Set FilletEdge = Selection.Item2(1).Value
EdgeHasBeenAcquiredAtLeastOnce = True
‘ Create the Fillet
Set Fillet = ShapeFactory.AddNewSolidEdgeFilletWithConstantRadius(FilletEdge,
catTangencyFilletEdgePropagation,5.0)
Part.Update
FilletNotFinished = False
Selection.Clear
‘ Determine the 1-D entity
MonoDimEntityDeterminationNotFinished = True
do while (MonoDimEntityDeterminationNotFinished And Not
FilletNotFinished)
‘ We propose to the user that he select 1-D entity whose
geometry is rectilinear
InputObjectType(0)=”RectilinearMonoDim”

Status=Selection.SelectElement2(InputObjectType, _

“Select a 1-D entity
whose geometry is rectilinear”,false)

if (Status = “Cancel”) then
‘ We remove the fillet, the pad, restore the selection
to its initial content and go out
Selection.Clear : Selection.Add(Fillet) : Selection.Delete
Selection.Clear : Selection.Add(Pad) : Selection.Delete
Part.Update
Selection.Clear
for SelectionObjectIndex = 0 to SelectionAtBeginningLength-1
Selection.Add SelectionAtBeginning(SelectionObjectIndex)
next
Exit Sub
elseif (Status = “Redo” And Not MonoDimEntityHasBeenAcquiredAtLeastOnce )
then
‘ We do nothing: Redo has no meaning in this context
elseif (Status = “Undo”) then
‘ We remove the fillet
Selection.Clear : Selection.Add(Fillet) : Selection.Delete
Part.Update
FilletNotFinished = True
else
if (Status = “Redo”) then
Selection.Clear : Selection.Add(MonoDimEntity)
else
Set SelectedElement = Selection.Item2(1)
Set MonoDimEntity = SelectedElement.Value
end if
MonoDimEntityHasBeenAcquiredAtLeastOnce = True
MonoDimEntityDeterminationNotFinished = False
‘ Create the Hole
HoleNotFinished = True
do while (HoleNotFinished And Not MonoDimEntityDeterminationNotFinished)
‘ We save the selection content in save
variables.
‘ This corresponds to the fact
that:
‘ - we want that, during the following call to
SelectElement2, the 1-D entity previously
‘ selected remain highlighted
‘ - this is done using the False value for the
iObjectSelectionBeforeCommandUsePossibility
‘ parameter, the selection containing the 1-D
entity. It requires that the selection
‘ content be saved
Set MonoDimEntitySave = Selection.Item2(1).Value
‘ We propose to the user that he select a
face
InputObjectType(0)=”Face”

Status=Selection.SelectElement2(InputObjectType, _

“Select a face
perpendicular to the 1-D entity”,false)
if (Status = “Cancel”) then
‘ We remove the fillet, the pad, restore the
selection to its initial content and go out
Selection.Clear : Selection.Add(Fillet) : Selection.Delete
Selection.Clear : Selection.Add(Pad) : Selection.Delete
Selection.Clear
for SelectionObjectIndex = 0 to SelectionAtBeginningLength-1
Selection.Add SelectionAtBeginning(SelectionObjectIndex)
next
Part.Update
Exit Sub
elseif (Status = “Redo” And Not FaceHasBeenAcquiredAtLeastOnce ) then
‘ We do nothing: Redo has no meaning in this context
elseif (Status = “Undo”) then
Selection.Clear
‘ The 1-D entity must be
re-selected
MonoDimEntityDeterminationNotFinished = True
else
if (Status <> “Redo”) then

Set SelectedElement = Selection.Item2(1)
Set PadFace = SelectedElement.Value
SelectedElement.GetCoordinates
HoleLocation
‘ We merge the selected element with the
save variables, and put the result in the selection
Selection.Add
MonoDimEntitySave
end if
FaceHasBeenAcquiredAtLeastOnce = True
‘ We create the Hole
Set Hole = Part.ShapeFactory.AddNewHoleFromPoint(HoleLocation(0),
HoleLocation(1),HoleLocation(2),PadFace,10.0)
Hole.ThreadingMode = 1 : Hole.ThreadSide = 0 :
Hole.Diameter.Value = 5.0
Hole.SetDirection
FilletEdge
Part.Update
HoleNotFinished = False
‘ We clear the selection
Selection.Clear
end if
loop
end if
loop
end if
loop
end if
loop
Parameters:

  • i_filter_type (tuple) –

  • i_message (str) –

  • i_object_selection_before_command_use_possibility (bool) –

Return type:

str

select_element3(i_filter_type: tuple, i_message: str, i_object_selection_before_command_use_possibility: bool, i_multi_selection_mode: int, i_tooltip: bool) → str

Note

CAA V5 Visual Basic Help (2020-07-03 17:02:05.216737))
o Func SelectElement3(CATSafeArrayVariant iFilterType,
CATBSTR iMessage,
boolean iObjectSelectionBeforeCommandUsePossibility,
CATMultiSelectionMode iMultiSelectionMode,
boolean iTooltip) As CATBSTR

Runs an interactive selection command, exhaustive version.
Role: SelectElement3 asks the end user to select a feature (in the geometry
or in the specification tree). It is identical to the SelectElement2 method
except that it manages complex uses through the specification of 2 more
parameters.

Parameters:

iFilterType
An array of strings constants defining the automation object types
with which the selection will be filtered.
iMessage
A string which instructs the user what to select. This string is
displayed in the message area located at the left of the power input area.

iObjectSelectionBeforeCommandUsePossibility
Enables the script to support the possibility, for the user, to
select required object(s) before running the script. See


SelectElement2 .
iMultiSelectionMode
The type of multi-selection which will be offered to the user.

iTooltip
Displays a tooltip as soon as an object is located under the mouse
without being selected.
oOutputState
The state of the selection command once SelectElement3 returns. It can
be either “Normal”, “Cancel”, “Undo” or “Redo”. See SelectElement2
.
Example:

This first example asks the end user to select several points (see


Point ) into the current Part window, drawing a trap, and performs a
symmetry with respect to the XZ plane on the selected points (see
HybridShapeSymmetry ). The points can be selected before the script be
run.

Dim Document,Part,Selection,HybridShapeFactory,HybridBodies,HybridBody,OriginElements,Plane,
PlaneReference,Status
Dim InputObjectType(0),PointIndex,PointReference,HybridShapeSymmetry
Set Document = CATIA.ActiveDocument : Set Part = Document.Part :
Set Selection = Document.Selection
Set HybridShapeFactory = Part.HybridShapeFactory
Set Bodies = Part.Bodies
Set Body = Bodies.Item(“PartBody”)
Set OriginElements = Part.OriginElements
Set Plane = OriginElements.PlaneZX
Set PlaneReference = Part.CreateReferenceFromObject(Plane)
‘We propose to the user that he select several points, drawing a
trap
InputObjectType(0)=”Point”
Status=Selection.SelectElement3(InputObjectType,”Select points”,
_
true,CATMultiSelTriggWhenSelPerf,false)
if (Status = “Cancel”) then Exit Sub
For PointIndex = 1 to Selection.Count2
Set PointReference = Part.CreateReferenceFromObject(Selection.Item2(PointIndex).Value)
Set HybridShapeSymmetry = HybridShapeFactory.AddNewSymmetry(PointReference,PlaneReference)
HybridShapeSymmetry.VolumeResult = False
Body.InsertHybridShape HybridShapeSymmetry
Part.InWorkObject = HybridShapeSymmetry
Part.Update
next
Selection.Clear


Example:

This second example illustrates the use of the
CATMultiSelTriggWhenUserValidatesSelection value for the

iMultiSelectionMode parameter. This example is a training tool
enabling the user to learn how to use the “Symmetry”
command of the “Geometry Modification” toolbar of the Drafting
workbench.

It creates a drawing containing a line and three points, and guides
the user in:

the selection of points
the selection of the symmetry axis

the selected points being moved by symmetry according to the selected
axis.

‘We create a drawing
Set Documents = CATIA.Documents : Set Document = Documents.Add(“Drawing”)
: Document.Standard = catISO
Set DrawingSheets = Document.Sheets : Set DrawingSheet = DrawingSheets.Item(“Sheet.1”)
DrawingSheet.PaperSize = catPaperA0 : DrawingSheet.Scale = 1.000000
: DrawingSheet.Orientation = catPaperLandscape
Set DrawingViews = DrawingSheet.Views : Set DrawingView = DrawingViews.ActiveView
Set Factory2D = DrawingView.Factory2D : Set Selection = Document.Selection
: Dim Coordinates(2)
ReDim InputObjectType(0) : Dim SelectedPoint(3) : SelectedPointCount = 0
‘We create a horizontal line with a zero ordinate
Set LineLeftExtremity = Factory2D.CreatePoint(-100.0, 0.0)
: LineLeftExtremity.ReportName = 3
Set LineRightExtremity = Factory2D.CreatePoint(100.0, 0.0)
: LineRightExtremity.ReportName = 4
Set Line2D = Factory2D.CreateLine(-100.0, 0.0, 100.0, 0.0) : Line2D.ReportName = 5
Line2D.StartPoint = LineLeftExtremity : Line2D.EndPoint = LineRightExtremity
‘We create three points
Set Point2D1 = Factory2D.CreatePoint(-50.0, 50.0)
: Point2D1.ReportName = 6 : Point2D1.Construction = False
Set Point2D2 = Factory2D.CreatePoint(0.0, 70.0) : Point2D2.ReportName = 7
: Point2D1.Construction = False
Set Point2D3 = Factory2D.CreatePoint(50.0, 50.0) : Point2D3.ReportName = 8
: Point2D3.Construction = False
‘We mention to the user that he will select the set of elements to be
symmetrized
msgbox “This tool will enable you to learn how to use the Symmetry
command.” & Chr(13) & Chr(13) & _
“Suppose you selected the Symmetry command.” & Chr(13) & _

“You will first select several points to be
symmetrized”
‘We propose to the user that he select several points
InputObjectType(0)=”Point2D”
Status=Selection.SelectElement3(InputObjectType,”Select the set of
elements to be symmetrized”, _true,CATMultiSelTriggWhenUserValidatesSelection,false)
if (Status = “Cancel”) then Exit Sub
‘We add the selected points to SelectedPoint
for PointIndex = 0 to Selection.Count2-1
Set SelectedPoint(PointIndex) = Selection.Item2(PointIndex+1).Value
: SelectedPointCount = SelectedPointCount+1
next
‘We mention to the user that he will select the axis from which the
elements will remain equidistant
msgbox “You will then select the line from which the elements will
remain equidistant”
‘We propose to the user that he select the line
InputObjectType(0)=”Line2D”
Status=Selection.SelectElement2(InputObjectType, _
“Select the line or axis from which
the elements will remain equidistant”,
false)
if (Status = “Cancel”) then Exit Sub
‘We move the selected points by symmetry according to the selected
line
for PointIndex = 0 to SelectedPointCount-1
Set CurrentPoint2D = SelectedPoint(PointIndex)
CurrentPoint2D.GetCoordinates Coordinates
CurrentPoint2D.SetData Coordinates(0),
-Coordinates(1)
next
Selection.Clear
‘We mention to the user that the points have successfully been
moved
msgbox “The points have successfully been moved.”
Parameters:

  • i_filter_type (tuple) –

  • i_message (str) –

  • i_object_selection_before_command_use_possibility (bool) –

  • i_multi_selection_mode (int) – enum cat_multi_selection_mode

  • i_tooltip (bool) –

Return type:

str

select_element4(i_filter_type: tuple, i_active_document_message: str, i_non_active_document_message: str, i_tooltip: bool, o_document: Document) → str

Note

CAA V5 Visual Basic Help (2020-07-03 17:02:05.216737))
o Func SelectElement4(CATSafeArrayVariant iFilterType,
CATBSTR iActiveDocumentMessage,
CATBSTR iNonActiveDocumentMessage,
boolean iTooltip,
Document oDocument) As CATBSTR

Runs an interactive selection command, enabling the selection in a non
active document.
Role: SelectElement4 asks the end user to select a feature (in the geometry
or in the specification tree) of a non active document. During the selection,
when end user will move the mouse above a window corresponding to a non active
document, when he will move the mouse above a feature which maps the given
filter, the mouse pointer will be the “hand” cursor. When he will move the
mouse above a feature which does not map the given filter, the mouse pointer
will be the “no entry” cursor.
This method may be used, for example, to write a script which does the
following:

a drawing is currently edited
request that the user select a reference plane in the 3D geometry (a
part)
creation of a front view in the drawing, projecting the 3D geometry
onto the selected reference plane


Compared to the SelectElement2 , the result of the selection will not be
accessed through the Count2 and Item2 methods of the current selection object,
but through the Count2 and Item2 methods of the Selection object aggregated by
the Document object returned through the oDocument
parameter.
Note:The Selection object aggregated by the Document object returned
through the oDocument parameter is emptied by before the effective interactive
selection.

Parameters:

iFilterType
An array of strings constants defining the automation object types
with which the selection will be filtered.
iActiveDocumentMessage
A string which instructs the user what to select, which will be
displayed into the active document. This string is displayed in the message
area located at the left of the power input area.
iNonActiveDocumentMessage
A string which instructs the user what to select, which will be
displayed into the non active document.
iTooltip
Displays a tooltip as soon as an object is located under the mouse
without being selected.
oOutputState
The state of the selection command once SelectElement3 returns. It
can be either “Normal”, “Cancel”, “Undo”.

Example:

The following example supposes a part, containing a pad, and drawing
are currently edited, the drawing
window beeing the current window. It asks the end user to select a 2-D
topological entity, such as a


Plane , in a part. Then it creates a front view in the drawing, projecting
the 3D geometry onto the selected 2-D topological entity.

Dim DrawingSelection,DrawingSheets,DrawingSheet,DrawingViews,DrawingFrontView
ReDim DrawingSelectionAtBeginning(1)
Dim Status,InputObjectType(0),Plane,Drawing,DrawingViewGenerativeBehavior,V1(2),V2(2),
PartDocument
Set Drawing = CATIA.ActiveDocument : Set DrawingSelection = Drawing.Selection
: Set DrawingSheets = Drawing.Sheets
Set DrawingSheet = DrawingSheets.ActiveSheet
‘We save the current selection content
ReDim
DrawingSelectionAtBeginning(DrawingSelection.Count2)
for SelectionObjectIndex = 0 to DrawingSelection.Count2-1
Set DrawingSelectionAtBeginning(SelectionObjectIndex) = DrawingSelection.Item2(1).Value
next
SelectionAtBeginningLength = DrawingSelection.Count2
‘Feature creation
InputObjectType(0)=”BiDimInfinite”
Status=DrawingSelection.SelectElement4(InputObjectType,”Select a 2-D
topological entity in a 3-D geometry”, _”Select a 2-D topologicalentity”,false,PartDocument)
if ((Status = “Cancel”) Or (Status = “Undo”) Or (Status = “Redo”)) then
‘ We restore the selection to its initial content
PartDocument.Selection.Clear
for SelectionObjectIndex = 0 to SelectionAtBeginningLength-1
DrawingSelection.Add
DrawingSelectionAtBeginning(SelectionObjectIndex)
next
Exit Sub
else
Set BiDimFeature = PartDocument.Selection.Item2(1).Value
BiDimFeatureType = TypeName(BiDimFeature)
if ((BiDimFeatureType=”Plane”) Or (BiDimFeatureType=”PlanarFace”))
then
BiDimFeature.GetFirstAxis V1
BiDimFeature.GetSecondAxis V2
else
Exit Sub
end if
‘ We create a view called “Front View” in the current sheet, using Plane
as projection plane, and whose origin
‘ coordinates are 300,150
Set DrawingFrontView = DrawingSheet.Views.Add(“Front View”)
Set DrawingViewGenerativeBehavior = DrawingFrontView.GenerativeBehavior
DrawingViewGenerativeBehavior.Document = PartDocument
DrawingViewGenerativeBehavior.DefineFrontView V1(0), V1(1), V1(2),
V2(0), V2(1), V2(2)
DrawingFrontView.x = 300
DrawingFrontView.y = 150
DrawingViewGenerativeBehavior.Update
‘ We clear the PartDocument Selection object
PartDocument.Selection.Clear
end if
Parameters:

  • i_filter_type (tuple) –

  • i_active_document_message (str) –

  • i_non_active_document_message (str) –

  • i_tooltip (bool) –

  • o_document (Document) –

Return type:

str

property vis_properties: VisPropertySet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384)
o Property VisProperties() As VisPropertySet (Read Only)

Manages graphic properties on current selection.
Role: Gives a VisPropertySet automation object so that graphic properties
of the selected objects can be read or modified.
Note: After the execution of the VisProperties methods which update graphic
properties of the features, selected features which are not exposed to
automation will be updated. After the execution of the VisProperties methods
which consult the selection to give the graphic properties, selected features
which are not exposed to automation will be consulted.

Example:
This example sets in no show all elements of the current
selection:

Dim Selection,VisPropertySet
Set Selection = CATIA.ActiveDocument.Selection
Set VisPropertySet = Selection.VisProperties
VisPropertySet.SetShow catVisPropertiesNoShowAttr
Return type:

VisPropertySet