Mechanical Modeler Novelties- Impacts

Mechanical Modeler		Mechanical Modeler Novelties- Impacts V5R13 & V5R14 novelties
Technical Article

Abstract

Since V5R13, Mechanical Modeler has introduced novelties which can imply modifications in your existing code, or can have consequences on the way to lead up your new developments.

The article has been cut in two parts, the first one presents the novelties [1], and the current one exposes the consequences in term of code for each kind of CAA applications.

This article requires Mechanical Modeler knowledge. However to help the reader, along the paragraphs, technical articles explaining Mechanical Modeler concepts are referenced.

Read Part Contents
Geometrical Feature Instantiation
- Surfacic Feature Instantiation
- Solid Feature Instantiation
Geometrical Feature Usage
User Feature and Power Copy Instantiation and Usage
CAA Geometrical Feature Creation
In Short
References

Read Part Contents

You are an application consulting the contents of a Part document in order to perform analysis or to do data transfers. You should know how to retrieve the geometrical features of a set [2], and their topological result [3].

To retrieve the contents of a set in order to retrieve its result, do not more use the CATIDescendants interface, but use the CATIBodyRequest interface. There are, at least, two reasons:

The CATIBodyRequest interface returns the relevant features of the set by excluding the absorbed features [4]. These features are not drawn, and even if they have a geometrical result, you must not take them into account.
The CATIBodyRequest interface directly retrieves the Solid feature which is the feature holding the result of a Body feature. Since the Body feature [2] can also contain surfacic features, its result is not more the last feature of the set, easily retrieval by CATIDescendants, but it is the last solid feature of the set.

Read the referenced article [3] for more information about the behavior and usage of the CATIBodyRequest interface.

Nevertheless, if you need all the aggregated geometrical features of a set, you can always use the GetDirectChildren method of CATIDescendants with the CATIGeometricalElement3D interface as filter.

Geometrical Feature Instantiation

You are an application instantiating Dassault Systemes (DS) or CAA geometrical features. The first question to solve is: where will be inserted the new feature? Answering this question enables you to know the valid geometrical features sets to insert your feature. Then, you could know the impacts in your existing code. This section is divided in two parts:

For surfacic features, refer to the Surfacic Feature Instantiation section.
For solid features, refer to the Solid Feature Instantiation section.

Surfacic Feature Instantiation

You are an application instantiating Dassault Systemes (DS) or CAA surfacic features. You can have three strategies to choose the valid geometric features set:

You do not care of the geometrical features set

It means that the surfacic feature can be inserted equally into a Body, into an Ordered Geometrical set, or into a Geometrical Set. Using this solution, you are DS compliant.

You do not want an insertion into a solid and surfacic features set

It means that the surfacic feature can be only inserted into a surfacic features set: either into an Ordered Geometrical set, or into a Geometrical Set, but not into a Body feature.

You only want an insertion into a Geometrical Set

It means that the surfacic feature will be always inserted into a non ordered surfacic features set. You may choose this solution if do you not want to disturb your clients, or your end users. They will have the same interactive behavior as before V5R13.

Now, for each strategy, the following table [Tab.1] summarizes the checks to do in your existing code.

Tab.1 Surfacic Feature Instantiation Impacts
Strategic choice	CATIGSMProceduralView use	Interface to filter a valid set	Insert the feature into the set	Migration between V5R13 and V5R14
You do not care of the geometrical features set	possible	CATIGSMTool	impact	no
You do not want an insertion into a solid and surfacic features set	no more possible	CATIMmiGeometricalSet	impact	R14 only
You only want an insertion into a Geometrical Set	no more possible	CATIMmiNonOrderedGeometricalSet	no impact	no

The first column describes your strategy
If your code use the CATIGSMProceduralView interface, and its InsertInProceduralView method, the second column shows if you can always use it. If you cannot use it, you should modify your code to do yourself the two steps which are described in the next point. Nevertheless, if you can always use it, do not forget to see the second step of the next point.
-> The CATIGSMProceduralView interface is not always possible because this interface allows the integration in any kind of geometrical features set.
The elementary steps to insert a new feature in a geometrical features set are:

Retrieve or create a valid geometrical features set

The third column names the interface which enables you to filter the valid geometrical features set. If the current set, retrieval by the GetCurrentTool method of the CATIPrtPart interface, does not implement the given interface, the DS strategy is to create a new Geometrical Set. Check in your existing code the filtering interface.

Insert the new surfacic feature into the set

The forth column shows if you have an impact in this step.

For those which did not use CATIGSMProceduralView, or cannot use it now, the following code shows, in bold, the lines to add in your existing code:

  ...
  CATIGSMTool *pIGSMToolOnMyTool = .... ;
  
  int TypeOrderedSet = -1 ;
  piGSMTool->GetType(TypeOrderedSet);
  if (TypeOrderedSet == 1 ) 
  {
      aggregates the new surfacic feature in pIGSMToolOnMyTool. 
      
  }else
  {// your previous code
  }
  
  Update the feature
  
  ...

The way to aggregate the feature into the set is detailed in the "How Insert a Geometrical Feature into a Geometrical Features Set" section of the referenced article [1].

For every body, after the aggregation, you must call the Insert method of the CATMmrLinearBodyServices class [4].

  ...
  
  if (TypeOrderedSet == 1) 
  {
      CATMmrLinearBodyServices::Insert(pointerOnNewFeature);  
  }
  ...

The fifth column shows if you have an impact in R14, if you have already done a migration in R13 to take the Ordered Geometrical Set into account.

Whatever the choice, you must check that the feature to insert implement CATIInputDescription. It is mandatory for any surfacic features. For DS surfacic features, the implementation has been done. You have only to check your CAA surfacic features.

You can refer to the Combined Curve use case [5], where the three choices have been implemented.

Solid Feature Instantiation

You are an application instantiating Dassault Systemes (DS) or CAA solid features. There are two cases to consider:

DS solid features

Factories creating DS solid features, automatically integrate the solid feature in the current Body.

CAA solid features

Your code to insert the feature into a set is based on the CATIMechanicalTool interface. So the insertion will be now either into a MechanicalTool, or an HybridBody.

To aggregate the solid feature into the set there is no impact. But, after the update of your feature, you must call the Insert method of the CATMmrLinearBodyServices class if the set is a solid and surfacic features set. In bold, the new lines to add in your existing code:

  ...
  Update the feature
  CATIMechanicalTool *pIMechToolOnMyTool = .... ;
  CATIGSMTool *pIGSMOnMyTool= NULL ;
  rc = pIMechToolOnMyTool->QueryInterface(IID_CATIGSMTool,(void)**&pIGSMOnMyTool);
  if (SUCCEEDED(rc) ) 
  {
      CATMmrLinearBodyServices::Insert(pointerOnNewFeature);  
  }
  ...

Geometrical Feature Usage

You are an application handling geometrical features, in other words your application modifies the contents of a set, modifies inputs of a feature, or delete a feature. The following table [Tab.2] summarizes the prohibited operations, and the new line of code to write depending on the type of the set where the operation is done.

Tab.2 Impact Depending on the Type of Set
Operation Types		OGS	Body	GS
Moving surfacic features coming from a GS	to	impossible	impossible	no impact
Moving surfacic features coming from an OGS/Body	to	impossible	impossible	impossible
Reordering features	into	impossible	impossible	no impact
Modifying feature inputs	into	After the update of the feature, add an `Insert` call	no impact	no impact
Deleting features	into	impossible	impossible	no impact

Some explanations:

No impact means that your existing code does not need any modification
It is the Insert method of the CATMmrLinearBodyServices
It is impossible to reorder a feature inside an ordered set (OGS/Body) - Do not use CATIPrtProceduralView and its reorder method.
It is impossible to move a feature to an ordered set, or coming from an ordered set.

Consequently, in your existing code, you must check the type of the set, and then execute the code depending on its type such as described just above [Tab.2].

User Feature and Power Copy Instantiation and Usage

If you have an application instantiating Power Copy or User feature [6] you have nothing to do since the software of instantiation automatically manages the insertion into a set whatever its type.

For a User feature, solid or surfacic, you do not have to implement the CATIInputDescription interface. It is automatically managed by the User Feature software.

If you have implemented the CATIEdit interface on your "typed" surfacic User Feature, the only one impact is to manage the current feature in the edition command. You should set as current the edited instance, and restore the old current feature once the edition is ended. Otherwise (for a solid User Feature), you have no impact, because the current feature must be already managed by your command.

The following table [Tab.3] summarizes these purposes:

Tab.3 User Feature and Power Copy Impacts
Operation	*CATIInputDescription* implementation	Edition
Power Copy	no implementation	always impossible
Surfacic User Feature	no implementation	manage the current feature such as described below
Solid User Feature	no implementation	no impact

For a surfacic User Feature, you can refer to the CAAMcaUdfEdition use case [7], for a detailed implementation. This use case highlights the added lines in the existing command.

If you have already done the migration in R13, your code is still valid for the R14.

CAA Geometrical Feature Creation

If you have an application creating CAA geometrical feature [8], the following table [Tab.4] summarizes the impacts in your existing code.

Tab.4 CAA Geometrical Feature Creation Impacts
	*CATIInputDescription* implementation	Creation Command	Edition Command (CATIEdit implementation)
Solid feature	NO	* Manage the valid set - see the Solid feature Instantiation section * Add an `Insert` call after the update of the feature	no impact
Surfacic feature	YES	* Manage the valid set - see the Surfacic Feature Instantiation section. * If creation into an OGS/Body : - Manage the current feature (1) - Add an `Insert` call after the update of the feature	If feature is into OGS/Body : - Manage the current feature (2) - Add an `Insert` call after the update of the feature Otherwise no modification

Some explanations:

The CATIInputDescription implementation is not necessary for a solid feature, since the first solid feature of a Body is always a feature of creation, and the others are always a feature of modification. For a surfacic feature it is mandatory.
All your creation command must manage the valid geometrical features set depending on your strategic choice. It is explained in the Geometrical Feature Instantiation section.
About the current feature management
- For a solid feature, there is no need to add the management of the current feature in your existing code, because it already does it.
- For a surfacic feature
  - In the command of creation, the feature newly created must be set the current one during the command (if the feature is created at the beginning of the command), and stay (or become) the current one leaving the command. (1)
  - In a command of edition, the edited feature must be set the current one during the time of the command. The previous current feature must be restored at the end of the command. (2)
It is the Insert method of the CATMmrLinearBodyServices class
In your commands of creation and edition, check that you use the CATFeatureImportAgent class to select the input of your features.

You can refer to the Combined Curve use case for the implementation of the CATIInputDescription interface [9], and a sample of existing command of creation and edition, updated to integrate the R13 and R14 novelties[10].

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In Short

V5R13 and V5R14 have introduced novelties which can involved your existing code. The main code impacts are:

Use CATIBodyRequest in place of CATIDescendants to retrieve the topological result of the set
Use the Insert method of the CATMmrLinearBodyServices if the feature is integrated in an ordered set.
Use the CATFeatureImportAgent class in your edition/creation command
Eventually manage the current feature in your edition/creation command
Implement CATIInputDescription on your CAA surfacic feature

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References

[1]	Mechanical Modeler Novelties - Presentation
[2]	The Contents of the Specification Container- Geometrical Features Sets
[3]	Specification/Result Mechanism Applied to Mechanical Features
[4]	Order and Absorption Concepts
[5]	Instantiating Combined Curves
[6]	An Overview of Power Copies and User Features
[7]	Creating a Command to Edit a User Feature
[8]	Creating a New StartUp Deriving from a Mechanical StartUp
[9]	Integrating Combined Curves inside Ordered Sets
[10]	Editing Combined Curves
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History

Version: 1 [Mar 2004]	Document created
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