Mechanical Design

Drafting

Creating a Section View from a 3D Sketch

How to create a section view with the cutting profile associative to a 3D Sketch
Use Case

Abstract

This article discusses the CAADrwCreateSectionFrom3DSketch use case. This use case explains how to create a generative section view defined by a cutting profile associative to a 3D Sketch. Thus, if the 3D Sketch is modified, the section view will modified after update.

What You Will Learn With This Use Case

This use case is intended to show you how to create a Drawing generative section view from a 3D Sketch.

Fig 1: The part document containing the sketch "SketchForSection"

The SketchForSection sketch allows you to manage the cutting profile of the Drawing Section View from the 3D document.

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The CAADrwCreateSectionFrom3DSketch Use Case

CAADrwCreateSectionFrom3DSketch is a use case of the CAADraftingInterfaces.edu framework that illustrates DraftingInterfaces framework capabilities.

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What Does CAADrwCreateSectionFrom3DSketch Do?

 

Fig. 2: Drawing Document with the new Section view

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How to Launch CAADrwCreateSectionFrom3DSketch

To launch CAADrwCreateSectionFrom3DSketch, you will need to set up the build time environment, then compile CAADrwCreateSectionFrom3DSketch 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\PartWithPlaneAndSketchForSectionView.CATPart.

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Where to Find the CAADrwCreateSectionFrom3DSketch Code

The CAADrwCreateSectionFrom3DSketch use case is made of a single source file named CAADrwCreateSectionFrom3DSketch.cpp located in the CAADrwCreateSectionFrom3DSketch.m module of the CAADraftingInterfaces.edu framework:

Windows InstallRootDirectory\CAADraftingInterfaces.edu\CAADrwCreateSectionFrom3DSketch.m\
Unix InstallRootDirectory/CAADraftingInterfaces.edu/CAADrwCreateSectionFrom3DSketch.m/

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

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Step-by-Step

There are six steps in CAADrwCreatViewFrom3D:

  1. Creating and Initializing the Document
  2. Creating the Drawing in the Document
  3. Retrieving the Part document and the "SketchForSection" Sketch
  4. Creating the Section View from the "SketchForSection" Sketch
  5. 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 "SketchForSection" Sketch

...
 // READ THE PART DOCUMENT AND GET THE APPROPRIATE SKETCH
 // =====================================================
 CATDocument *pDocPart = NULL;
 if( SUCCEEDED(CATDocumentServices::OpenDocument(pfileNamePart, pDocPart)) && pDocPart)
 {
   CATInit_var spInitOnDoc(pDocPart);
   if(NULL_var != spInitOnDoc)
   {
     // Retrieves the root container
     CATIPrtContainer * piPrtCont = (CATIPrtContainer*) spInitOnDoc->GetRootContainer("CATIPrtContainer"); 
     if (piPrtCont)
     {
       // Get the part feature of the container.
       CATIPrtPart_var spPart = piPrtCont->GetPart();

       // Get the appropriate sketch 
       CATIDescendants *piDescPart=NULL;
       if (SUCCEEDED(spPart->QueryInterface(IID_CATIDescendants,(void**)&piDescPart)))
       {
         CATListValCATISpecObject_var listFeatures;

         piDescPart->GetAllChildren ("CATISketch",listFeatures) ;

         int nbChilds = listFeatures.Size();
         CATISketch* piSketch = NULL;
         CATISpecObject_var spFeat;
         for (int i = 1; i <= nbChilds; i++)
         {
           spFeat = listFeatures[i]; 
           if (NULL_var != spFeat)
           {
             if (SUCCEEDED(spFeat->QueryInterface(IID_CATISketch, (void**)&piSketch)))
             {
               CATIAlias *piSketchAlias = NULL;
               if (SUCCEEDED(piSketch->QueryInterface(IID_CATIAlias, (void**)&piSketchAlias)))
               {
                 CATUnicodeString SketchName = piSketchAlias->GetAlias();
		 const CATUnicodeString SketchSection_UC = "SketchForSection";
		 if (SketchName == SketchSection_UC)
		 hr = CreateSectionViewFromSketchInDrawingDoc(pNewDoc, piSketch);

...

All the sketches in the Part document are retrieved by using the GetAllChildren method of the CATIDescendants interface. The appropriate sketch is extracted from the list thanks to the GetAlias method of the CATIAlias interface.

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Creating the Section View from the "SketchForSection" Sketch

...
// ---------------------------------------------------------------
// Sub program to create a Drawing Generative View from a 3D Sketch.
// ---------------------------------------------------------------
HRESULT CreateSectionViewFromSketchInDrawingDoc(CATDocument *ipNewDoc, CATISketch *ipi3DSketch)
{
  HRESULT hr = E_FAIL;

  if (ipNewDoc && ipi3DSketch)
  {
    // 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 (ie. the list of .CATDrwSTD files in the reffiles directory)
              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 ISO standard in the document
                      piStdmgr->ImportStandard (wstd);
                      break;
                    }
                    delete[] wstd; wstd = NULL;
                  }
                }
                piListstd->Release(); piListstd=NULL; 
              }
              piStdmgr->Release (); piStdmgr=NULL;
            }
          }

          // Creation of new generative section view from a 3D Sketch in the active sheet of the Drawing Document
          CATIDftView *piDftSectionViewFrom3D = NULL;
          CATIDftSheet *piDftSheet = NULL;
          piDftDrawing->GetActiveSheet(&piDftSheet);

          // View anchor point definition
          double ptOrigin[2] = {150.0,150.0};
           CATMathVector normalSketch;
          CATI2DLine_var spFirstLine;
          double pOrthoDirection[2];
 
          CATIDftGenViewFactory *piDftGenViewFact = NULL;
          if (piDftSheet && SUCCEEDED(piDftSheet->QueryInterface(IID_CATIDftGenViewFactory,(void **)&piDftGenViewFact))) 
          {
            // vecPro argument compute:
            // VecPro must be a direction perpandicular to the first line in the sketch defining the section profile.
            // The Vecpro orientation informs the system which part will be drawn in the section view.
            CATLISTV (CATI2DWFGeometry_var ) GeomList;
            if (SUCCEEDED(ipi3DSketch->GetComponents(CATI2DWFGeometry::ClassName(),GeomList)))
            {
              if (GeomList.Size() > 1)
              {
                int indice=1;
                while (indice < GeomList.Size())
                {
                  spFirstLine = GeomList[indice];
                  if (NULL_var != spFirstLine)
                  {
                    double pOrigin[2],pDirection[2];
                    spFirstLine->GetLineData(pOrigin, pDirection);
                    pOrthoDirection[0] = pDirection[1];
                    pOrthoDirection[1] = -pDirection[0]; 
                    break;
                  }
                  indice++;
                }
              }
            }
            CATISpecObject_var spPlanarSupport;
            if (SUCCEEDED(ipi3DSketch->GetPlanarSupport(spPlanarSupport )))
            {
              CATPlane_var spPlane= spPlanarSupport;
              if(NULL_var != spPlane)
              {
                CATMathPlane mathPlaneSk;
                spPlane->GetAxis(mathPlaneSk);
                CATMathPoint ThePoint;
                mathPlaneSk.EvalPoint(pOrthoDirection[0],pOrthoDirection[1],ThePoint); 
                double XCoord = ThePoint.GetX();
                double YCoord = ThePoint.GetY();
                double ZCoord = ThePoint.GetZ(); 

                CATMathDirection vecPro;
                vecPro.SetCoord(XCoord,YCoord,ZCoord);

                // Offset Profile
                int viewProfile = 0;

                // Section View defined by a Sketch
                CATCell *piPlaneElem = NULL;
                CATBody *piBody= NULL;
                CATMathPoint iLimitPoints[2];

                // Sketch defined in Part Document
                CATIProduct *piProduct= NULL;

                // Creation of the section view associative to a 3D Sketch
                hr = piDftGenViewFact->CreateStandAloneSectionView(ptOrigin, DftSectionView, vecPro, viewProfile, ipi3DSketch,piPlaneElem,piBody,iLimitPoints,piProduct,
                &piDftSectionViewFrom3D);
                piDftGenViewFact->Release();piDftGenViewFact=NULL;
              }
            }
          }
          piDrawingSO->Release();
          piDrawingSO=NULL;
        }
       piDftDrawing->Release(); 
       piDftDrawing = NULL;
     }
   }
  } 
  return hr;
}
...

The sub program CreateSectionViewFromSketchInDrawingDoc create a Section View from a 3D Sketch by using the method CreateStandAloneSectionView of the CATIDftGenViewFactory interface. This interface is implemented by the Sheet. The Drawing Standard has to be initialized before the Drawing View creation

Main arguments to initialize are:

The other arguments are of no use in this sample.

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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:

  1. Open a Part document
  2. Retrieve the appropriate sketch in the Part document.
  3. Create a Drawing document, and initialize the sStandard
  4. Create a section view from a 3D Sketch by using CreateStandAloneSectionView method defined in the CATIDftGenViewFactory interface
  5. Save the Drawing document

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References

[1] Building and Launching a CAA Use Case
[2] Loading a Document
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History

Version: 1 [Jan 2005] Document created
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Copyright © 2005, Dassault Systèmes. All rights reserved.