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SketcherInterfaces Interface CATISketchPositioning

System.IUnknown
  |
  +---System.IDispatch
    |
    +---System.CATBaseUnknown
      |
      +---CATISketchPositioning
 

Usage: an implementation of this interface is supplied and you must use it as is. You should not reimplement it.


interface CATISketchPositioning

Interface to manage the positioning of a sketch.
Role: This interface is used to manage the attributes of a sketch from which the position will be computed.


Method Index


o EvalPosition(HRESULT&,HRESULT&,HRESULT&,int,int)
Compute, evaluate and analyze the new position of the sketch.
o GetDirectionCoordinates(CATListValCATISpecObject_var&)
Retrieves the direction coordinates for orientation.
o GetHDirectionSense(int&)
Retrieves the Horizontal direction.
o GetNormalSense(int&)
Retrieves the Normal direction.
o GetOrientationDirection(CATSktPosDirection&)
Retrieves the direction of the sketch axis which is oriented.
o GetOrientationMode(CATSktPosOrientationMode&)
Retrieves the orientation definition mode.
o GetOrientationReferences(CATListValCATISpecObject_var&)
Retrieves the orientation reference elements.
o GetOriginMode(CATSktPosOriginMode&)
Retrieves the origin definition mode.
o GetOriginReferences(CATListValCATISpecObject_var&)
Retrieves the origin reference elements.
o GetSupportMode(CATSktPosSupportMode&)
Retrieves the support definition mode.
o GetSupportReferences(CATListValCATISpecObject_var&)
Retrieves the support reference elements.
o GetVDirectionSense(int&)
Retrieves the Vertical direction.
o PositionAsReference()

Role: Puts the sketch ARWL (As Result With Link) at the same position as the original sketch, and set the type of the sketch on CATSktSupPositionedAsRef
o ReverseHDirection(void)
Reverses the Horizontal direction.
o ReverseVDirection(void)
Reverses the Vertical direction.
o SetOrientationDirection(CATSktPosDirection)
Sets the oriented direction of the sketch axis.
o SetOrientationMode(CATSktPosOrientationMode)
Sets the orientation definition mode.
o SetOrientationReferences(CATListValCATBaseUnknown_var&)
Sets the orientation reference elements.
o SetOriginMode(CATSktPosOriginMode)
Sets the origin definition mode.
o SetOriginReferences(CATListValCATBaseUnknown_var&)
Sets the origin reference elements and definition mode.
o SetSupportMode(CATSktPosSupportMode)
Sets the support definition mode.
o SetSupportReferences(CATListValCATBaseUnknown_var&)
Sets the support reference elements.
o SwapHVDirections(void)
Swaps the Horizontal and Vertical directions.

Methods


o EvalPosition
public virtual HRESULT EvalPosition(HRESULT& oSupportStatus,
HRESULT& oOriginStatus,
HRESULT& oOrientationStatus,
const int iEvaluationMode=1,
const int iMovingMode=1) = 0
Compute, evaluate and analyze the new position of the sketch.
Role: This method lets you know if the sketch is correctly positioned.
Parameters:
oSupportStatus
[out] Evaluation status of the sketch support positioning
oOriginStatus
[out] Evaluation status of the sketch origin positioning
oOrientationStatus
[out] Evaluation status of the sketch orientation positioning
iEvaluationMode
[in] Evaluation mode
Legal values: The evaluation mode value can be 1 for creation state or 2 for edition state.
iMovingMode
[in] Moving mode
Legal values: The moving mode value can be 1 to move the absolute axis and the sketch geometry or 0 to move the absolute axis only.
Returns:
HRESULT
o GetDirectionCoordinates
public virtual HRESULT GetDirectionCoordinates(CATListValCATISpecObject_var& oXYZ)= 0
Retrieves the direction coordinates for orientation.
Parameters:
oXYZ
[out] A list of 3 literal parameters for each coordinate.
Returns:
HRESULT
o GetHDirectionSense
public virtual HRESULT GetHDirectionSense(int& oDirection)= 0
Retrieves the Horizontal direction.
Parameters:
oDirection
[out] Direction coefficient.
+1
Same direction.
-1
Reverse direction.
Returns:
HRESULT
o GetNormalSense
public virtual HRESULT GetNormalSense(int& oDirection)= 0
Retrieves the Normal direction.
Parameters:
oDirection
[out] Direction coefficient.
+1
Same direction.
-1
Reverse direction.
Returns:
HRESULT
o GetOrientationDirection
public virtual HRESULT GetOrientationDirection(CATSktPosDirection& oDirection)= 0
Retrieves the direction of the sketch axis which is oriented.
Role: The orientation direction lets you specify whether the orientation references will be applied on axis H or V. Direction definitions are listed in the CATSktPosDirection definition.
Parameters:
oDirection
[out] Oriented direction.
Legal values: The oriented direction value can be CATSktDirHorizontal for the horizontal axis or CATSktDirVertical for the vertical axis.
Returns:
HRESULT
o GetOrientationMode
public virtual HRESULT GetOrientationMode(CATSktPosOrientationMode& oMode)= 0
Retrieves the orientation definition mode.
Role: The orientation definition mode lets you define the absolute axis orientation. Orientation definition modes are listed in the CATSktPosOrientationMode definition.
Parameters:
oMode
[out] Orientation definition mode.
e.g.: CATSktOrtThroughAPoint
Returns:
HRESULT
o GetOrientationReferences
public virtual HRESULT GetOrientationReferences(CATListValCATISpecObject_var& oReferences) = 0
Retrieves the orientation reference elements.
Parameters:
oReferences
[out] List of orientation reference elements.
Returns:
HRESULT
o GetOriginMode
public virtual HRESULT GetOriginMode(CATSktPosOriginMode& oMode)= 0
Retrieves the origin definition mode.
Role: The origin definition mode lets you define the sketch origin. Origin definition modes are listed in the CATSktPosOriginMode definition.
Parameters:
oMode
[out] Origin definition mode.
e.g.: CATSktOriPartOrigin
Returns:
HRESULT
o GetOriginReferences
public virtual HRESULT GetOriginReferences(CATListValCATISpecObject_var& oReferences) = 0
Retrieves the origin reference elements.
Parameters:
oReferences
[out] List of origin reference elements.
Returns:
HRESULT
o GetSupportMode
public virtual HRESULT GetSupportMode(CATSktPosSupportMode& oMode)= 0
Retrieves the support definition mode.
Role: The support definition mode lets you define the sketch support references. Support definition modes are listed in the CATSktPosSupportMode definition.
Parameters:
oMode
[out] Support definition mode.
e.g.: CATSktSupOnePlane
Returns:
HRESULT
o GetSupportReferences
public virtual HRESULT GetSupportReferences(CATListValCATISpecObject_var& oReferences) = 0
Retrieves the support reference elements.
Parameters:
oReferences
[out] List of support reference elements.
Returns:
HRESULT
o GetVDirectionSense
public virtual HRESULT GetVDirectionSense(int& oDirection)= 0
Retrieves the Vertical direction.
Parameters:
oDirection
[out] Direction coefficient.
+1
Same direction.
-1
Reverse direction.
Returns:
HRESULT
o PositionAsReference
public virtual HRESULT PositionAsReference()=0

Role: Puts the sketch ARWL (As Result With Link) at the same position as the original sketch, and set the type of the sketch on CATSktSupPositionedAsRef
Returns:
HRESULT - S_OK, if the sketch has been successfully positioned as its reference. - E_FAIL, otherwise.
o ReverseHDirection
public virtual HRESULT ReverseHDirection(void ) = 0
Reverses the Horizontal direction.
Returns:
HRESULT
o ReverseVDirection
public virtual HRESULT ReverseVDirection(void ) = 0
Reverses the Vertical direction.
Returns:
HRESULT
o SetOrientationDirection
public virtual HRESULT SetOrientationDirection( const CATSktPosDirection iDirection)= 0
Sets the oriented direction of the sketch axis.
Role: The orientation direction allows lets you specify whether the orientation references will be applied on axis H or V. Direction definitions are listed in the CATSktPosDirection definition.
Parameters:
iDirection
[in] Oriented direction.
Legal values: The oriented direction value can be CATSktDirHorizontal for the horizontal axis or CATSktDirVertical for the vertical axis.
Returns:
HRESULT
o SetOrientationMode
public virtual HRESULT SetOrientationMode( const CATSktPosOrientationMode iMode) = 0
Sets the orientation definition mode.
Role: The orientation definition mode lets you define the absolute axis orientation. Orientation definition modes are listed in the CATSktPosOrientationMode definition.
Parameters:
iMode
[in] Origin definition mode.
e.g.: CATSktOrtThroughAPoint
Returns:
HRESULT
o SetOrientationReferences
public virtual HRESULT SetOrientationReferences( const CATListValCATBaseUnknown_var& iReferences) = 0
Sets the orientation reference elements.
Parameters:
iReferences
[in] List of orientation reference elements.
Returns:
HRESULT
o SetOriginMode
public virtual HRESULT SetOriginMode( const CATSktPosOriginMode iMode) = 0
Sets the origin definition mode.
Role: The origin definition mode lets you define the sketch origin. Origin definition modes are listed in the CATSktPosOriginMode definition.
Parameters:
iMode
[in] Origin definition mode.
e.g.: CATSktOriPartOrigin
Returns:
HRESULT
o SetOriginReferences
public virtual HRESULT SetOriginReferences( const CATListValCATBaseUnknown_var& iReferences) = 0
Sets the origin reference elements and definition mode.
Parameters:
iReferences
[in] List of origin reference elements.
Returns:
HRESULT
o SetSupportMode
public virtual HRESULT SetSupportMode( const CATSktPosSupportMode iMode) = 0
Sets the support definition mode.
Role: The support definition mode lets you define the sketch support references. Support definition modes are listed in the CATSktPosSupportMode definition.
Parameters:
iMode
[in] Support definition mode.
e.g.: CATSktSupOnePlane
Returns:
HRESULT
o SetSupportReferences
public virtual HRESULT SetSupportReferences( const CATListValCATBaseUnknown_var& iReferences) = 0
Sets the support reference elements.
Parameters:
iReferences
[in] List of support reference elements.
Returns:
HRESULT
o SwapHVDirections
public virtual HRESULT SwapHVDirections(void ) = 0
Swaps the Horizontal and Vertical directions.
Returns:
HRESULT

This object is included in the file: CATISketchPositioning.h
If needed, your Imakefile.mk should include the module: CATSketcherInterfaces

Copyright © 2003, Dassault Systèmes. All rights reserved.