Mechanical Design

Drafting

Creating a View from 3D

How to create a view from 3D with annotations created by the Functional and Tolerancing and Annotation workbench

Use Case

Abstract

This article discusses the CAADrwCreateViewFrom3D use case. This use case explains how to create a view from 3D with annotations created by Functional and Tolerancing and Annotation workbench.

What You Will Learn With This Use Case
The CAADrwCreateViewFrom3D Use Case

What Does CAADrwCreateViewFrom3D Do
How to Launch CAADrwCreateViewFrom3D
Where to Find the CAADrwCreateViewFrom3D Code

Step-by-Step
In Short
References

What You Will Learn With This Use Case

This use case is intended to show you how to create a Drawing generative view from a TPS view. A TPS view is defined in a 3D part, product or process that is assigned 3D tolerance specifications and annotations. The Drawing generative View will be associated to the part document and the TPS view. All the modifications applied in the TPS view will be propagated in the Drawing generative view by update.

Fig 1: The part document containing a TPS View (Front View.1)

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The CAADrwCreateViewFrom3D Use Case

CAADrwCreateViewFrom3D is a use case of the CAADraftingInterfaces.edu framework that illustrates DraftingInterfaces framework capabilities.

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What Does CAADrwCreateViewFrom3D Do?


Fig. 2: Drawing Document with the view from 3D

Fig. 2 represents the Drawing document in which a front view has been created from the active TPS view of Annotation Set in the Part document. Note: A red cross is created to inform the end user that the text leader is associative to hidden geometry in the view.

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How to Launch CAADrwCreateViewFrom3D

To launch CAADrwCreateViewFrom3D, you will need to set up the build time environment, then compile CAADrwCreateViewFrom3D along with its prerequisites, set up the run time environment, and then execute the use case [1].

When you launch the use case, pass the full pathname of the Drawing file as argument. A Part file is delivery in the following path: CAADraftingInterfaces.edu\CNext\resources\graphic\PadWith3DAnnotations.CATPart.

With Windows

e:> mkrun -c cmd
CAADrwCreateViewFrom3D c:\...\PadWith3DAnnotations.CATPart c:\DrawingTestOutput.CATDrawing

With UNIX

$ mkrun -c cmd
CAADrwCreateViewFrom3D /u/users/.../PadWith3DAnnotations.CATPart /u/users/DrawingTestOutput.CATDrawing

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Where to Find the CAADrwCreateViewFrom3D Code

The CAADrwCreateViewFrom3D use case is made of a single source file named CAADrwCreateViewFrom3D .cpp located in the CAADrwCreateViewFrom3D.m module of the CAADraftingInterfaces.edu framework:

Windows	`InstallRootDirectory\CAADraftingInterfaces.edu\CAADrwCreateViewFrom3D.m\`
Unix	`InstallRootDirectory/CAADraftingInterfaces.edu/CAADrwCreateViewFrom3D.m/`

where InstallRootDirectory is the directory where the CAA CD-ROM is installed.

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Step-by-Step

There are five steps in CAADrwCreatViewFrom3D:

Creating and Initializing the Document
Creating the Drawing in the Document
Retrieving the Part Document and the Active TPS View
Creating the View from 3D
Saving the Document and Exiting

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Creating and Initializing the Document

int main(int iArgc, // Number of arguments (2) 
char** iArgv) // Path to the new *.CATDrawing document
{
// Check arguments
if(3 != iArgc) return 1;
const char *pfileNamePart = iArgv[1];
const char *pfileNameOut = iArgv[2];
int code_err = 1;


// CREATE THE SESSION
// ==================
CATSession *pSampleSession = NULL;
HRESULT hr = ::Create_Session("SampleSession",pSampleSession);
if (FAILED(hr)) return 1;

...

This section represents the usual sequence for loading a CATIA document [2].

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Creating the Drawing in the Document

...
   // DRAWING DOCUMENT CREATION
   // ===============================
   CATDocument* pNewDoc = NULL;
   CATDocumentServices::New("CATDrawing", pNewDoc); 
...

The other steps to fully initialize the Drawing document are included in the specific sub program, CreateViewFrom3DInDrawingDoc.

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Retrieving the Part Document and the Active View of the TPS Annotation Set

...
// READ THE PART DOCUMENT AND GET ACTIVE TPS VIEW
// ====================================================
  CATDocument *pDocPart = NULL;
  if( SUCCEEDED(CATDocumentServices::OpenDocument(pfileNamePart, pDocPart)) )
  {
    CATInit *piDocAsInit = 0;
    if( SUCCEEDED(pDocPart->QueryInterface(IID_CATInit, (void**)&piDocAsInit)) )
    {
      CATITPSDocument *piTPSDoc= NULL;
      if (SUCCEEDED(piDocAsInit->QueryInterface(IID_CATITPSDocument,(void **)&piTPSDoc)))
      {
        CATITPSList *piTPSList = NULL;
        if (SUCCEEDED(piTPSDoc->GetSets(&piTPSList)))
        {
          unsigned int nbSet;
          piTPSList->Count(&nbSet);
          if (nbSet > 0)
          {
            CATITPSComponent *piTPSCmp = NULL;
            if (SUCCEEDED(piTPSList->Item(0,&piTPSCmp)))
            {
              if (piTPSCmp)
              {
                CATITPSSet *piTPSSet = NULL;
                if (SUCCEEDED(piTPSCmp->QueryInterface(IID_CATITPSSet,(void **)&piTPSSet)))
                {
                  CATITPSView *piTPSActiveView = NULL;
                  if (SUCCEEDED(piTPSSet->GetActiveView (&piTPSActiveView)) && piTPSActiveView)
                  {
                    IUnknown *pTPSViewUk = NULL;
                    if (SUCCEEDED(piTPSActiveView->QueryInterface(IID_IUnknown,(void **)&pTPSViewUk)))
                    {
                      // Call a Sub Program to Create a Drawing View from TPS View in a Drawing Document
                      // =========================================================================
                      hr = CreateViewFrom3DInDrawingDoc(pNewDoc,piTPSActiveView);

...

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Creating the View from 3D

...
// Sub program to create a Drawing Generative View from TPS View.
// =========================================================
HRESULT CreateViewFrom3DInDrawingDoc(CATDocument *ipNewDoc, CATITPSView *ipiTPSActiveView)
{
  HRESULT hr = E_FAIL;

  if (ipNewDoc && ipiTPSActiveView)
  {
  // DRAWING STANDARD CREATION
  // ===============================

  // Gets the drawing feature using the CATIDftDocumentServices interface
  CATIDftDrawing *piDftDrawing = NULL;
  CATIDftDocumentServices *piDftDocServices = NULL;
  CATIContainer_var spDrwCont;
  if (SUCCEEDED(ipNewDoc->QueryInterface(IID_CATIDftDocumentServices, (void **)&piDftDocServices)))
  {
    piDftDocServices->GetDrawing(IID_CATIDftDrawing, (void **)&piDftDrawing);
    piDftDocServices->Release(); 
    piDftDocServices = NULL;
    if (piDftDrawing)
    {
      CATISpecObject *piDrawingSO=NULL;
      if (SUCCEEDED(piDftDrawing->QueryInterface(IID_CATISpecObject,(void **)&piDrawingSO)))
      {
        spDrwCont = piDrawingSO->GetFeatContainer();
        if (NULL_var != spDrwCont)
        {
          CATIDftStandardManager *piStdmgr = NULL;
          hr = spDrwCont->QueryInterface(IID_CATIDftStandardManager,(void**)&piStdmgr);
          if (SUCCEEDED(hr))
          {
            // Find a standard in the list of allowed standards
            CATIStringList *piListstd = NULL;
            if ( SUCCEEDED(piStdmgr->GetAvailableStandards(&piListstd)) && piListstd )
            {
              unsigned int nbrstd = 0;
              piListstd->Count(&nbrstd);
              for (unsigned int indice = 0; indice < nbrstd; indice ++)
              {
                wchar_t *wstd = NULL;
                if ( SUCCEEDED ( piListstd->Item ( indice, &wstd ) ) && wstd )
                {
		  CATUnicodeString stdname;
		  const CATUnicodeString ISO_UncS = "ISO";
		  stdname.BuildFromWChar(wstd);
		  if ( stdname == ISO_UncS ) 
                  {
                    // Import the ANSI standard in the document
                    piStdmgr->ImportStandard (wstd);
                    break;
                  }
                  delete[] wstd; wstd = NULL;
                }
              }
              piListstd->Release(); piListstd=NULL; 
            }
            piStdmgr->Release (); piStdmgr=NULL;
          }
        }

        // Creation of new generative view from TPS view in the active sheet of the Drawing Document
        CATIDftView *piDftViewFrom3D = NULL;
        CATIDftSheet *piDftSheet = NULL;
        piDftDrawing->GetActiveSheet(&piDftSheet);

        // View anchor point definition
        double ptOrigin[2] = {150.0,150.0};
        IUnknown *pTPSViewUk = NULL;
        if (SUCCEEDED(ipiTPSActiveView->QueryInterface(IID_IUnknown,(void **)&pTPSViewUk)))
        {
          CATIDftGenViewFactory *piDftGenViewFact = NULL;
          if (piDftSheet && SUCCEEDED(piDftSheet->QueryInterface(IID_CATIDftGenViewFactory,(void **)&piDftGenViewFact))) 
          {
            hr = piDftGenViewFact->CreateViewFrom3D(ptOrigin, pTPSViewUk, &piDftViewFrom3D);
            piDftGenViewFact->Release();piDftGenViewFact=NULL;
          }
          pTPSViewUk->Release();
          pTPSViewUk=NULL;
        }
        piDrawingSO->Release();
        piDrawingSO=NULL;
      }
      piDftDrawing->Release(); 
      piDftDrawing = NULL;
    }
   }
   } 
  return hr;
}

...

The sub program CreateViewFrom3DInDrawingDoc creates a View from 3D by using the method CreateViewFrom3D of the CATIDftGenViewFactory interface. This interface is implemented by the Sheet.

Note: Before the creation of the Drawing View, the Drawing Standard has to be correctly initialized. It must be identical to the Standard used by the Annotation Set aggregating the TPS View in the 3D document [3].

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Saving the Document and Exiting

...
// SAVE THE RESULT
// =================
if (pNewDoc)
{
  CATDocumentServices::SaveAs(*pNewDoc, (char *)pfileNameOut);
  CATDocumentServices::Remove (*pNewDoc);
}

//ENDS SESSION AND DROPS DOCUMENT
//===================================== 
if (pDocPart)
  CATDocumentServices::Remove (*pDocPart);

::Delete_Session("SampleSession");

This section represents the usual sequence for saving a newly created CATIA document.

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In Short

This use case shows the way to:

Open a Part document
Retrieve the active TPS view in the Annotation Set
Create a Drawing document, and initialize the standard
Create a view from 3D by using the CreateViewFrom3D method defined in CATIDftGenViewFactory
Save the Drawing document.

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References

[1]	Building and Launching a CAA Use Case
[2]	Loading a Document
[3]	Technological Product Specification Overview
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History

Version: 1 [Jan 2005]	Document created
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