Mechanical Modeler

The GeometricalElement Features

A geometrical feature is a mechanical feature to which the update mechanism, through the CATIBuild [5] interface, associates a topological result. This section presents an overview of these features thanks to the Mechanical StartUps tree and explains how a classification in relationship with the topology of the feature can be done.

The Mechanical StartUps Tree

The geometrical features derive from the GeometricalElement StartUp [6]. The picture [Fig.1] below is an extract of the mechanical StartUps tree:

Fig.1: GeometricalElement Architecture

Classification by Topology

There are some interfaces, implemented (*) on the GeometricalElement3D StartUp, which enables you to classify a geometrical feature by its topological result [5]. These interfaces are useful to filter selections, it means that you can use them in agent of selection for example. 

• CATIMfPoint, CATTIMfLine and CATIMfPlane

The CATBody associated with the feature is a equivalent to a Point (CATPoint) , a Line (CATLine), a Plane (CATPlane) respectively.

• CATIMfInfiniteResult

All the domains (CATDomain) of the CATBody associated with the feature are infinite. (infinite line or plane)

• CATIMfZeroDimResult, CATIMfMonoDimResult, CATIMfBiDimResult and CATIMfTriDimResult 

All the domains (CATDomain) of the CATBody associated with the feature have the same dimension of  0,1, 2 or 3 respectively.

(*)The implementation is "conditional". It means that a QueryInterface call on these interfaces will be successful only if the feature requires the specificity of the interface. However, be aware that a feature may change of type during its life.

Solid versus Surfacic Feature

A solid feature is a feature only referencing 3D geometry whereas a surfacic feature is a feature referencing  0D, 1D, 2D or 3D geometry. 

• Points are surfacic features of zero dimension,
• Wires (including the sketches) are surfacic features of one dimension,
• Surfaces are surfacic features of two dimension,
• Volumes are surfacic features of three dimension. [13]

In the general case, a feature deriving from the MechanicalShapeFeature StartUp is a solid feature and a feature deriving from the GSMGeom or GeometricalElement3D StartUps is a surfacic feature [Fig.1]. But there are at least two exceptions. The EdgeFillet feature, deriving from the MechanicalContextualFeature StartUp, can be locally a surfacic feature if it is aggregated in a GSMTool. Inversely, the Loft feature, deriving from the GSMGeom StartUp, can be locally a solid feature if it is aggregated in an HybridBody. 

However, if this kind of behavior is possible for Dassault Systemes features, it is impossible for your features. A CAA geometrical feature deriving from MechanicalContextualFeature or MechanicalFormFeature is necessarily a solid feature, whereas a CAA feature deriving from GSMGeom or GeometricalElement3D is a surfacic feature [7].

The CATIMf3DBehavior interface enables you to know if a geometrical feature is solid or surfacic. These interface groups together methods which are exclusives:

• For a solid feature, the IsASolid method returns S_OK, and the other methods return E_FAIL,
• For a surfacic feature, the IsAShape method returns S_OK, and the other methods return E_FAIL.

For the volumes, the IsAShape method returns S_OK, since a volume is a surfacic feature, but also the IsAVolume method of the CATIMf3DBehavior2 interface.

A solid feature can be only included in a solid and surfacic features set, in other words a PartBody or a Body feature, as compared to a surfacic feature which can be included into any geometrical features set: a Geometrical Feature Set, an Ordered Geometrical Set, a PartBody, or a Body. 

Form versus Contextual Feature

A solid feature can either be a form or a contextual feature. 

Definition

A Pad, a Pocket, a Groove, are different features: some add matter, while some remove it. However, they share a common point: they have a Form and are therefore called Form features. What exactly are they ?

Take a Groove for instance. From its input parameters, a Curve and a closed Sketch, one can easily derive a shape (a Form) by sliding the Sketch along the Curve. The resulting solid has then to be operated with the Part's shape as it exists prior to the definition of the Groove, by removing matter (thanks to a boolean difference operation in this case). 

The fact that these features can be applied by first computing their form and then operating the form with the current shape of the geometrical features set defines the form feature. The form of such a feature is sometimes called its footprint.

In contrast to Form features, Contextual features, cannot be applied by first computing a standalone footprint, and then operating it with the current set. Fillets, Drafts, and generally all Dress up features fall into this category, because their shape is determined not only by their own input parameters, but also by the local topology of the target set. Contextual features do not have a footprint.

First Feature for a PartBody/Body

The first feature in a PartBody [3] cannot be a contextual feature because at this point there is no matter in the Part to operate upon. This constraint does not exist for the Body features. Since their ultimate goal is to be operated with the PartBody, the matter on which their first feature will operate will be provided by the PartBody. As a consequence, their first feature can be a contextual feature.

The Feature Polarity

It must be noted that the fact that some features add and others remove matter from the Part is not linked to the form/contextual classification. A Draft is a contextual feature that adds matter, while a Chamfer, also contextual, removes it. A Revolution and a Pocket are form features that create and remove matter respectively. 

Adding or removing matter defines the polarity of the solid feature. The CATIShapeFeatureProperties interface (MechanicalModeler) returns the polarity of the solid feature.

Note: The polarity of a Body/PartBody, which is the polarity of its first solid feature, is given by the same interface. 

Creation versus Modification Feature 

This distinction between a feature of creation and a feature of modification is meaningful for features inside an ordered set [8]. The interface specifying the classification is CATIInputDescription (InteractiveInterfaces). 

A feature of creation is a feature creating matter from its input specifications. For example, a line created from two points is a feature of creation. A feature of modification is a feature modifying one or several of its input specifications. For example, a split is a feature of modification. The GetFeatureType method of the CATIInputDescription enables you to specify the type of your feature. This type is not necessarily fixed, it can be dependant of the values of inputs.

A feature of modification is also named an absorbent feature for the following behaviors on its modified inputs also named absorbed features: 

• The absorbed feature are not drawn,
• They do not appear in the result of the surfacic body [9],
• They are not selectable.

Fig.2 Ordered Set

The right picture [Fig.2] shows the result of the split operation of Extrude.1 (a surface) by the plane Plane.1. Split.1 is the feature representing the result. If you see the left picture [Fig.2] which shows the model before the split operation, you can note on the right that Extrude.1 is not drawn. 

The absorbed features are returned by the GetListOfModifiedFeatures method of CATIInputDescription. It can be one or several features, but all are an input of the absorbent feature, and have the same dimension as it. 

One of these absorbed features is privileged. It is the feature returned by the GetMainInput method. This feature has two roles:

• It gives the graphic properties to the absorbent feature

The color of Feat3, a feature of modification which has two inputs, is given by its main input, here it is Input2. 

• In case of reorder of a feature of modification, the moved feature has for new input the main input of the previous feature

If Feat4, a feature of modification, is moved before Feat3, the input of Feat4 becomes Input2 (the main input).

If your feature is a feature of creation, the GetListOfModifiedFeatures and GetMainInput methods must return E_FAIL. 

Datum versus Specification Feature

Definition

One of the major strengths of the Feature modeler [6] is that it allows the construction of a feature from other features. The result of one feature can be the inputs of another feature so that one can reach a linked flow of features characterizing the design intent. The modification of one of the parameters of one feature in the chain does not break the design since the update allows just the recalculation of the final result. We, therefore, have a record of the construction.

For some applications, this record is useless. So we have introduced the notion of a mechanical feature without history. This is the datum. A datum is a feature without input geometrical specifications. 

A datum is not a specific feature: it is an existing feature with the "datum" status. It can be, for example, a GSMPoint, a GSMLine, a GSMPlane or a GeometricalElement3D feature. The CATIMf3DBehavior interface and its IsaDatum method returns the status of the feature. 

(*) GSMPoint, GSMLine and GSMPlane are StartUps deriving from GSMGeom but not representing on the given UML schema [Fig.1].

Creating a datum can be done for other reasons: 

• To hide the design,
• To keep the geometry without historical interest,
• To apply constraints more easily .

Creating Interactively a Datum

The way to create a datum depends on the current application:

• In the Generative Shape Design application, you can use the CreateDatum setting:

Fig.3 a: Datum in GSD

The Line.1 feature has been created with the Point.1 and Point.2 features. But before executing the Line command, the CreateDatum setting has been activated. Next, the Point.1 has been moved, but the line has not changed. (Points are represented by white crosses, and the line ends by two black dots).

• In the  Part Design application, you can use the sequence of the Copy  & Paste Special commands:

Fig.3 b: Datum in Part Design

The PartBody has been selected, and with the contextual menu, the Copy/Paste Special command with the "Paste As Result" option has been executed. The Solid.1 feature has been created.

Note: If the "Paste As Special With Link" is chosen, this means that a link to the original feature has been kept. A modification in the feature modifies the datum after an update.

Creating a Datum by Code

There are three ways to code the creation of a datum:

1. Using the CATIIsolate interface (MechanicalModeler) 

This interface enables the transformation of an existing feature to a feature without specifications. But this interface is only available for few features: Point, Line, Plane, Circle.

2. Using the CATIDatumFactory interface (MechanicalModeler) 

A feature is created using a CATBody. Based on this topological object, a surface, a plane, a point, a solid feature is created. 

There are two available methods:

• InstantiateDatum(CATBody* iBody,CATISpecObject* &oDatumFeature)

This method creates the scope [10] with an automatic naming. 

• InstantiateDatum(CATBody* iBody,CATLISTP(CATCell)* iGNUserCells,CATListOfCATUnicodeString* iUserKeys,CATISpecObject* &oDatumFeature)

This method enables driving yourself the naming of the following cells. The "Creating a Result Without Procedural Report" chapter of the article entitled "Integrating the New Mechanical Feature in the Update Mechanism" [5] gives the details to fill these lists.

The created features are the following:

1. if the CATBody contains one domain with only one vertex, it is a Point feature implementing the CATIGSMPoint interface.
2. if the CATBody contains one domain with one edge, it is a Line feature implementing the CATIGSMLine interface.
3. if the CATBody contains one domain with one CATPlane element, it is a Plane feature implementing the CATIGSMPlane interface.
4. if the CATBody contains one domain with one CATCircle element, it is a Circle feature implementing the CATIGSMCircle interface.
5. if the CATBody contains several domains with the same dimension 0, it is a GSMZeroDim feature implementing the CATIMfZeroDimResult interface
6. if the CATBody contains several domains with the same dimension 1,it is a GSMMonoDim feature implementing the CATIMfMonoDimResult interface
7. if the CATBody contains several domains with the same dimension 2, it is a GSMBiDim feature implementing the CATIMfBiDimResult interface
8. if the CATBody contains several domains with the same dimension 3, it is a Solid feature implementing the CATIMfTriDimResult interface
9. otherwise the feature is a GeometricalElement3D

Caution: With the second InstantiateDatum method, with the list of cells and the list of keys, a GeometricalElement3D is created instead a basic feature (Point, Line, Plane, Circle).

3. By creating your own feature

In certain cases, the topology is not fixed, it must be generated at each update. In this case, you should create a new geometrical feature which will derive from the GeometricalElement3D [Fig.1] StartUp.  The "Creating a New StartUp Deriving from a Mechanical StartUp" article [7] gives all the steps to create it. This feature must necessarily implement the following interfaces:

• CATIBuild

Refer to the "Creating a Result Without Procedural Report" section of the "Integrating the New Geometrical Feature in the Update Mechanism" article [5]

• CATIMf3DBehavior

The new feature is a surfacic feature and a datum feature:

• IsASolid should returns E_FAIL
• IsAShape should returns S_OK
• IsADatum  should returns S_OK

For the other behaviors, refer to the article entitled "Integrating a New Mechanical Feature in V5" [11].

Existing Features

Dassault Systemes provides Mechanical features through applications such as Part Design or Generative Shape Design.  This section lists them, as well as the related interfaces that manage them.

The Part Design Features

They are not represented on the GeometricalElement Architecture UML Schema [Fig.1], most of them derive from the Solid feature. 

• The solid features: you can create them with the CATIPrtFactory (PartInterfaces) interface:
• Contextual feature:
  • Fillet
  • Chamfer
  • Split
  • ...
• Form feature
  • Pad
  • Pocket
  • Groove
  • Shaft
  • ...
• The volumes also with the  CATIPrtFactory (PartInterfaces) interface:
  • Draft , 
  • Seewing , 
  • Shell,
  • ...
• The surfacic operations [3]: also with the  CATIPrtFactory (PartInterfaces) interface:
• Split,
• Close Surface
• ...
• The boolean operations [3]: With the CATIPrtBooleanFactory interface (PartInterfaces) 
  • Add
  • Remove
  • Intersect
  • Assemble

The Generative Shape Design Features. 

These features derive from the GSMGeom feature. [Fig.1]. You can create them with the CATIGSMFactory (GSMInterfaces) interface:

• Element 0D, 1D, 2D
  • Point
  • Line
  • Plane
  • Extrude 
• Transformation feature
  • Translation
  • Rotation
  • ... 
• Dress-up 

Inserting a Geometrical Feature inside a Geometrical Features Set

The geometrical features sets are the PartBody feature, the Body features, the Ordered Geometrical Set features, and the Geometrical Set features [3]. 

Before going further, let us review the vocabulary

• Aggregate a feature into a set is the operation consisting in to add the feature into the set
• Insert a feature into a set is first an aggregation, and then a operation to manage the order into the set.

This insertion is depending on three things:

1. The factory creating the feature

The features created by the CATIGSMFactory interface (The Generative Shape Design Features section) are to be aggregated after their creation, whereas the features created by the CATIPrtFactory/CATIPrtBooleanFactory interfaces (The Part Design Features section) are automatically included in the current set. 

Consequently, for features created by the CATIGSMFactory interface, and for your CAA features (surfacic or not), read the How to aggregate a geometrical feature into a geometrical features set section for explanations about the aggregation. 

2. The type of the feature.

To aggregate a solid feature, the used interface is not the same as for a surfacic feature. The methodology is explained in the How to aggregate a geometrical feature into a geometrical features set section.

3. The type of the geometrical features set.

Whatever the factory, and whatever the type of the feature, if the set is ordered, the aggregation is not sufficient. After the aggregation and after the update of the feature, you must invoke the Insert method of the CATMmrLinearBodyServices class. This method manages the re-root of the features into the ordered set. [8].

How to aggregate a geometrical feature into a geometrical features set?

To aggregate a solid feature inside a PartBody or a Body, the InsertInProceduralView method of the CATIPrtProceduralView  interface must necessarily be used.  Refer to the "A Chain of Features" section of the "Specification/Result Mechanism Applied to Mechanical Feature" article [8].

For any surfacic feature you can use the CATIDescendant interface. But, if the surfacic feature derives from GSMGeom, it is recommended to use the InsertInProceduralView method of the CATIGSMProceduralView. 

If the set is ordered, the new feature must be located just after the current feature, if the current feature is into the set, otherwise located at the end of the set. The both InsertInProceduralView methods manage the right location. If you use the CATIDescendant, here it is a piece of code to manage the good location:

...
int pos = 0 ;
CATISpecObject_var CurrentElt = GetCurrentFeature() ;
if ( NULL_var != CurrentElt)
{
   pos = pIDescendantsOnGSMTool->GetPosition(CurrentElt);                   
}

if ( 0 == pos )
{
   pIDescendantsOnGSMTool->Append(piSpecOnCombinedCurve);
}else
{
                 
   pIDescendantsOnGSMTool->AddChild(piSpecOnCombinedCurve,pos+1);
}
...

It is an extract of the combined curve use case [12] where:

• GetCurrentFeature is a method of the command where is extract this code
• pIDescendantsOnGSMTool, is a CATIDescendant interface pointer on the set
• piSpecOnCombinedCurve is a CATISpecObject interface pointer on the feature to aggregate
• If the current feature is not inside the set, the value of pos is zero. The new combined curve is aggregated at the end of the set thanks to the Append method.
• If the current feature is inside the set, the value of pos is not nul. The new combined curve is aggregated just after the current feature thanks to the Addchild method.

There is another advantage to use the CATIGSMProceduralView instead of the CATIDescendants interface for a surfacic feature. The first interface creates a Geometrical Set, if the current set is not a surfacic set. It is possible if the PartBody or the Body features have been instantiated from the MechanicalTool StartUp. It means that your Part document was created before the R14. 

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In Short

The specification container is one of the containers of the Part document. It groups together the mechanical features. Among these are the geometrical features which hold a topological result. There are two kinds of geometrical features:

• The solid feature

In most cases, this is the feature deriving from the MechanicalShapeFeature StartUp. It is aggregated either by the PartBody, or a Body. Both are solid and surfacic features sets. There are the form features having a footprint and the contextual features which need an initial form to be computed with it. 

• The surfacic feature:

In most cases, this is the feature deriving either from the GSMGeom StartUp or the GeometricalElement3D StartUp. It is aggregated either by Ordered Geometrical Set, or a Geometrical Set. Both are surfacic features sets. 

A solid feature or a surfacic feature can be a datum. A datum is a feature without specifications, it contains only the result, a CATBody.

To insert a geometrical feature into a set: 

• Use the appropriate interface according to the type of the feature:
  • CATIPrtProceduralView for a solid feature
  • CATIDescendants for a surfacic feature
  • CATIGSMProceduralView for a surfacic feature derving from the GSMTool StartUp
• After the update, Invoke the Insert method of the CATMmrLinearBodyService if the set is ordered.

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References

History

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