All Frameworks Class Hierarchy This Framework Indexes Previous Next

CATMecModUseItf Interface CATIMmiUseSetFactory

SystemTS.IUnknown

System.IDispatch

System.CATBaseUnknown

CATIMmiUseSetFactory

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

interface CATIMmiUseSetFactory

Interface to create mechanical bodies.
Role:This interface enables you to create MechanicalTool and GSMTool features, both are mechanical features included into a 3D Shape.

The MechanicalTool feature

It is a solid body which is always aggregated by the MechanicalPart feature (CATIPrtPart ). The "PartBody" and all the "Body" in the specification tree are MechanicalTool features. The two CreatePRTTool methods enable you to create a MechanicalTool feature.

The GSMTool feature

It is a surfacic body. Since V5R13, there are two types of GSMTool:

Geometrical Set, the previous Open_Body

Such a surfacic body can be aggregated by the MechanicalPart feature, a MechanicalTool feature, and a Geometrical Set feature. The CATIGSMTool.GetType method returns 0. The CreateGeometricalSet method enables you to create a Geometrical Set feature.

Ordered Geometrical Set, a V5R13 novelty

Such a surfacic body can be aggregated by the MechanicalPart feature, and only an Ordered Geometrical Set feature. The CATIGSMTool.GetType method returns 1. The CreateOrderedGeometricalSet method enables you to create an Ordered Geometrical Set feature.

Any method that tries to create a body disrespecting aggregation rules or the private status of the destination body will throw an exception. For example creating a MechanicalTool inside a MechanicalTool is not allowed. Likewise, creating a GSMTool inside a private GSMTool is not allowed. Refer to CATIGSMTool.SetPrivate or CATIGSMTool.IsPrivate methods.

This interface is implemented by the specification container of the 3D Shape that you retrieve with CATInit.GetRootContainer

Method Index

o CreateGeometricalSet(CATUnicodeString&,CATIMmiMechanicalFeature_var&,CATIMmiMechanicalFeature_var&,int): Creates a Geometrical Set.
o CreateOrderedGeometricalSet(CATUnicodeString&,CATIMmiMechanicalFeature_var&,CATIMmiMechanicalFeature_var&,int): Creates an Ordered Geometrical Set.
o CreatePRTTool(CATUnicodeString&,CATIMmiMechanicalFeature_var&,CATIMmiMechanicalFeature_var&,int): Creates a MechanicalTool at a given position.

Methods

o CreateGeometricalSet

public virtual HRESULT CreateGeometricalSet(	const CATUnicodeString&	`iUserName`,
	const CATIMmiMechanicalFeature_var&	`iDestination`,
	CATIMmiMechanicalFeature_var&	`oGeomSet`,
	int	`iPosition`	`=-1`) = 0

Creates a Geometrical Set.
Role:This method creates a Geometrical Set feature. It implements the CATIMmiNonOrderedGeometricalSet interface.

Parameters:

iUserName

The user name of the created Geometrical Set. If the string is empty, the name will be automatically computed. It is the concatenation of the NLS name of the Geometrical Set feature and a number.

iDestination

Depending on the iPosition value, iDestination can be either the feature aggregating the new Geometrical Set or the feature just before the new Geometrical Set.

If iDestination is an aggregating feature, it can be

The MechanicalPart feature. You retrieve this feature by using the

CATIMmiPrtContainer.GetMechanicalPart

A Geometrical Set feature

A MechanicalTool feature

If iDestination represents the feature just before the new Geometrical Set, it can be any Mechanical feature (except the MechanicalPart)

oGeomSet

The created Geometrical Set.

iPosition

The position of the new Geometrical Set into the aggregating feature.
Legal values:

iPosition = -1 (the default value)
- If iDestination is the MechanicalPart feature
- If iDestination is a Geometrical Set or a MechanicalTool feature
0 <= iPosition<= iDestination size

The new Geometrical Set is created into iDestination:

iPosition = 0: At the last position inside iDestination
Otherwise: At the iPosition+1 position inside iDestination

Otherwise: the Geometrical Set is not created

o CreateOrderedGeometricalSet

public virtual HRESULT CreateOrderedGeometricalSet(	const CATUnicodeString&	`iUserName`,
	const CATIMmiMechanicalFeature_var&	`iDestination`,
	CATIMmiMechanicalFeature_var&	`oOrderedGeomSet`,
	int	`iPosition`	`=-1`) = 0

Creates an Ordered Geometrical Set.
Role:This method creates an Ordered Geometrical Set feature. It implements the CATIMmiOrderedGeometricalSet interface.

Parameters:

iUserName

The user name of the created Ordered Geometrical Set. If the string is empty, the name will be automatically computed. It is the concatenation of the NLS name of the Ordered Geometrical Set feature and a number.

iDestination

Depending on the iPosition value, iDestination can be either the feature aggregating the new Ordered Geometrical Set or the feature just before the new Ordered Geometrical Set.

If iDestination is an aggregating feature, it can be

The MechanicalPart feature. You retrieve this feature by using the

CATIMmiPrtContainer.GetMechanicalPart

An Ordered Geometrical Set feature

If iDestination represents the feature just before the new Ordered Geometrical Set, it can be any Mechanical feature (except the MechanicalPart)

oOrderedGeomSet

The created Ordered Geometrical Set.

iPosition

The position of the new Ordered Geometrical Set into the aggregating feature.
Legal values:

iPosition = -1 (the default value)
- If iDestination is the MechanicalPart feature
- If iDestination is an Ordered Geometrical Set
0 <= iPosition<= iDestination size

The new Ordered Geometrical Set is created into iDestination:

iPosition = 0: At the last position inside iDestination
Otherwise: At the iPosition+1 position inside iDestination

Otherwise: the Ordered Geometrical Set is not created

o CreatePRTTool

public virtual HRESULT CreatePRTTool(	const CATUnicodeString&	`iUserName`,
	const CATIMmiMechanicalFeature_var&	`iDestination`,
	CATIMmiMechanicalFeature_var&	`oPRTTool`,
	int	`iPosition`	`= 0`) = 0

Creates a MechanicalTool at a given position.
Role:This method creates a MechanicalTool feature at the last position inside the MechanicalPart feature (iDestination).

Parameters:

iUserName

The user name of the MechanicalTool to be created. If the string is empty, the name will be automatically computed. It is the concatenation of the NLS name of the MechanicalTool feature and a number.

iDestination

The unique possibility is the MechanicalPart feature of the 3D Shape. You retrieve this feature by using the

iPosition

CATIMmiPrtContainer.GetMechanicalPart The position inside iDestination:
Legal values:

n = 0: the MechanicalTool is created at the last position
n > 0 or n <= iDestination size: the position of the MechanicalTool is equal to n+1
Otherwise: the MechanicalTool is not created

Returns:

E_FAIL if an error occured, S_OK otherwise.

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