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DraftingInterfaces Interface CATIDftGenViewFactory

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

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


interface CATIDftGenViewFactory

This interface contains methods to create generative drafting views.
Role: This interface is implemented by sheet object.


Method Index


o CreateSectionView(double*,CATDftViewType,int,int,CATListPtrCATMathPoint2D,CATIDftView*,CATIDftView**)
Create a section view.
o CreateStandAloneSectionView(double*,CATDftViewType,CATMathDirection,int,CATISketch*,CATCell*,CATBody*,CATMathPoint[2],CATIProduct*,CATIDftView**)
Create a Standalone Section View.
o CreateViewFrom3D(double*,IUnknown*,CATIDftView**)
Create a view from 3D.

Methods


o CreateSectionView
public virtual HRESULT CreateSectionView(double* iptOrigin,
CATDftViewType iViewType,
int iViewProfile,
int iSideToDraw,
CATListPtrCATMathPoint2D iListOfPoints,
CATIDftView* ipiMotherView,
CATIDftView** opiSectionView) = 0
Create a section view. Role: Create a section view from a generative view called mother view. The section view will be defined by a cutting-profile defined in the mother view.
Parameters:
iPtOrigin[2]
Coordinates of anchor point of the section view created.
iViewType
Type of the View:
Legal values: DftSectionView, DftSectionCutView,
iViewProfile
Type of the profile:
Legal values: 0: Offset, 1: Aligned
iSideToDraw
The side of the section to draw. This side is defined according to the first segment of the section profile. This segment is oriented from its start point to its end point. When looking along this segment, from its start point towards its end point, setting iSideToDraw to 0 (clockwise) draws the section seen from the left of the segment. Setting iSideToDraw to 1 (counterclockwise)draws the section seen from the right of the segment.
Legal values: 0: Clockwise, 1: Counterclockwise
iListOfPoints
List of points defined the cutting profile (At least 2 points).
ipiMotherView
Pointer on the mother view.
opiSectionView
Pointer on the new section view.
Returns:
HRESULT
S_OK
if the section view was correctly added.
E_INVALIDARG
if the arguments are incorrect.
E_FAIL
if the operation failed.
o CreateStandAloneSectionView
public virtual HRESULT CreateStandAloneSectionView(double* iptOrigin,
CATDftViewType iViewType,
CATMathDirection iVecpro,
int iViewProfile,
CATISketch* ipi3DSketch,
CATCell* ipiCell,
CATBody* ipiBody,
CATMathPoint[2] iLimitPoints,
CATIProduct* ipiProduct,
CATIDftView** opiSectionView) = 0
Create a Standalone Section View. Role: Create a standalone section view with associative cutting profile to 3D element. The authorised 3D elements are either a sketch element or plannar face or a plan.
Parameters:
iPtOrigin[2]
Coordinates of anchor point of the section view created.
iViewType
Type of the View:
Legal values: DftSectionView,DftSectionCutView
iVecPro
The direction of projection of the view: This direction must be contained in the plane of the section and must be: Perpandicular to the first line of the Sketch for profile defined by a Sketch. Perpandicular to the line created by two limit points of the profile for profile defined by a Plane or a planar face.
iViewProfile
Type of the profile:
Legal values: 0: Offset, 1: Aligned
i3DSketch
The cutting profile is defined by a 3D sketch containing the geometry's description of the section profile
Legal values: if NULL, The profile must be defined by a plan or a plane face in the drawing
ipiCell
The cutting profile is defined by a plan or plane face.
Legal values: if NULL, The profile must be defined by a sketch
ipiBody
Associated body if the cutting profile is defined by a plan or plane face.
Legal values: NULL, if the profile is defined by a sketch.
iLimitPoints
2 points limits of the cutting profile, if the cutting profile is defined by a plan or a plane face.
iProduct
In the case of a 3D element is defined in CATProduct document, iProduct defines instance in the product containing i3DSketch or i3DElement
Legal values: NULL, if the profile is defined in CATPart
Returns:
S_OK
if the view section was correctly added.
E_INVALIDARG
if the arguments are incorrect.
E_FAIL
if the operation failed.
o CreateViewFrom3D
public virtual HRESULT CreateViewFrom3D(double* iptOrigin,
IUnknown* ipiTPSView,
CATIDftView** opiDftView) = 0
Create a view from 3D. Role: A View From 3D is extracted from a 3D part, document or process that is assigned 3D tolerance specifications and annotations.
Parameters:
iPtOrigin[2]
Coordinates of anchor point of the view created.
ipiTPSView
Pointer on TPSView: This pointer may be retrieved by using QueryInterface on CATITPSView pointer.
opiDftView
Pointer on the new view.
Returns:
HRESULT
S_OK
if the view was correctly added.
E_INVALIDARG
if the arguments are incorrect.
E_FAIL
if the operation failed.
See also:
CATITPSView

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

Copyright © 2003, Dassault Systèmes. All rights reserved.