AddByPlaneAndOffset used in an assembly

[oransen]

The Inventor 15 API says that AddByPlaneAndOffset is not supported in assemblies. Will that change/has that changed in later releases. It would be very useful, and can be done "manually" so why not programatically...?

TIA!

[oransen · Accepted solution]

I'm replying because I've found an alternative which might help others. I needed a function which, in an assembly, created a sketch offset from one of the standard planes. Here's the full C++ function:

bool CreateSketchOffsetFromXYPlaneInAsm (CComPtr<AssemblyComponentDefinition>& pAsmCompDef,  // where the sketch will be added
                                         CComPtr<PlanarSketch>& pNewSketch,     // The sketch created, an output
                                         const double kOffsetMm,
                                         const wchar_t* const pszSketchName)    // Name of the newly created sketch
{
    // Get PlanarSketches, the list of sketches
    CComPtr<PlanarSketches> pSketches = nullptr ;
    HRESULT hRes = pAsmCompDef->get_Sketches(&pSketches);
    if (FAILED(hRes) || (pSketches == nullptr)) {
        ShowCOMError (hRes,L"CXYPOSIA, get_Sketches failed") ;
        return false ;
    }

    // Get standard default WorkPlanes, probably 3 only initially in the list
    CComPtr<WorkPlanes> pWorkPlanes = nullptr ;
    hRes = pAsmCompDef->get_WorkPlanes(&pWorkPlanes);
    if (FAILED(hRes) || (pWorkPlanes == nullptr)) {
        ShowCOMError (hRes,L"CXYPOSIA, get_WorkPlanes failed") ;
        return false ;
    }

    // Get hold of one of the WorkPlanes. Valid indices are 1L 2L 3L for standard workplanes
    CComPtr<WorkPlane> pXYWorkPlane = nullptr ;
    hRes = pWorkPlanes->get_Item(_variant_t(3L, VT_I4),&pXYWorkPlane);
    if (FAILED(hRes) || (pXYWorkPlane == nullptr)) {
        ShowCOMError (hRes,L"CXYPOSIA, get_Item (workplane) failed") ;
        return false ;
    }

    CComPtr<TransientGeometry> pTransGeom = theApp.GetTransGeomPtr () ;    
    CComPtr<Point> pOrigin = nullptr ;
    hRes = pTransGeom->CreatePoint (0,0,0,&pOrigin);

    CComPtr<UnitVector> UnitXVector ;
    pTransGeom->CreateUnitVector (1.0,0,0,&UnitXVector) ;

    CComPtr<UnitVector> UnitYVector ;
    pTransGeom->CreateUnitVector (0.0,1.0,0,&UnitYVector) ;

    // Internally Inventor always uses cm, so convert...
    const double kOffsetInCm = kOffsetMm/10.0 ;
    pOrigin->PutZ (kOffsetInCm) ;
    CComPtr<WorkPlane> pOffsetWorkPlane ;
    hRes = pWorkPlanes->AddFixed(pOrigin,UnitXVector,UnitYVector,VARIANT_FALSE,&pOffsetWorkPlane) ;
    if (pOffsetWorkPlane == nullptr) { 
        gLogger.Printf (ekErrMsg,L"CXYPOSIA, Could not AddFixed") ;
        return false ;
    }

    // Now actually create a sketch and get a pointer to it in one go...    
    hRes = pSketches->Add (_variant_t((IDispatch *)pOffsetWorkPlane),
                           VARIANT_FALSE,
                           &pNewSketch);
    if (FAILED(hRes)) {
        ShowCOMError (hRes,L"CXYPOSIA, AddSketch failed") ;
        return false ;
    }

    pNewSketch->put_Name (BSTR(pszSketchName)) ;

    return true ;
}