If you have a new or exisiting drawing it is likely that you want to add views of the 3D object into the sheet. Here is a commented
code fragment which shows you to do it (error checking removed). Note also that we open the assembly invisibly so the user does not have to wait for the display of the assembly.
// Choose the IDW drawing template file
CComBSTR strTemplateFilename;
strTemplateFilename = L"C:\\Users\\Public\\Documents\\Autodesk\\Inventor 2014\\Templates\\Ransen.idw" ;
// Get the list of documents so we can add a new one to it (an IDW)
CComPtr<Documents> pDocuments;
pInvApp->get_Documents (&pDocuments) ;
// create a new IDW drawing from the selected template
CComPtr<Document> pDocument ;
HRESULT hRes = pDocuments->Add(kDrawingDocumentObject,
strTemplateFilename,
VARIANT_TRUE, // true = create the document visible
&pDocument);
// Convert from the "general document" type into the "drawing document" type...
CComQIPtr<DrawingDocument> pDrawingDoc ;
pDrawingDoc = pDocument ;
// Get the sheets in the drawing document. Since this IDW has only just been
// created there will be a single sheet
CComPtr<Sheets> pSheets ;
hRes = pDrawingDoc->get_Sheets(&pSheets) ;
// Get the single sheet inside the IDW. Remember the first object
// in a COM list had index 1...
CComPtr<Sheet> pSheet ;
hRes = pSheets->get_Item (CComVariant(1),&pSheet) ;
// Just for fun, get some data about the sheet...
double SheetHeight,SheetWidth ;
CComBSTR bstrSheetName ;
pSheet->get_Name (&bstrSheetName) ;
pSheet->get_Width(&SheetWidth) ;
pSheet->get_Height(&SheetHeight) ;
TRACE (L"The first sheet is called <%s> and is %.1f %.1f\n",
bstrSheetName,SheetWidth,SheetHeight) ;
// Now, we are going to add 2 views to the sheet, so get the list of views
// Since this is a new drawing there will be no views yet, but we need
// the list to add a view...
CComPtr<DrawingViews> pViews ;
hRes = pSheet->get_DrawingViews (&pViews) ;
// Create two points (using the transient geometry machine) which will
// position the views in the sheet...
CComPtr<TransientGeometry> pTrGeom = GetTransGeomPtr();
CComPtr<Point2d> pPt1;
CComPtr<Point2d> pPt2;
pTrGeom->CreatePoint2d(10.0,10.0,&pPt1);
pTrGeom->CreatePoint2d(10.0,30.0,&pPt2);
// Set the view scales that we need.
const double kViewScale1 = 0.25 ;
const double kViewScale2 = 0.125 ;
// Now get hold of the assembly which we want to show in the view
// (We'll open it invisibly)
CComBSTR strAssemblyFilename ;
strAssemblyFilename = L"C:\\CollMakeV2\\Coll_IPT_IAM\\new test.iam" ;
CComPtr<Document> pDoc ;
hRes = pDocuments->Open (strAssemblyFilename, // what to open
VARIANT_FALSE, // open it invisible
&pDoc) ; // result
// The 6th parameter of AddBaseView requires a proper BSTR type object
// else you'll get out of memory errors
CComBSTR bstrModelViewName1 = CString (L"PLUTO") ;
CComBSTR bstrModelViewName2 = CString (L"NEPTUNE") ;
// Now create our two views, first the base view on which all the others are based...
CComVariant varEmpty ;
CComPtr<DrawingView> pBaseView1 ;
pViews->AddBaseView (pDoc, // what to show
pPt1, // center of view
kViewScale1, // size, scale, of view
kBottomViewOrientation, // from where to view the doc
kHiddenLineDrawingViewStyle, // DrawingViewStyleEnum
bstrModel, // must be a BSTR
varEmpty,varEmpty, // unused in this case
&pBaseView1) ; // the created view
CComPtr<DrawingView> pBaseView2 ;
pViews->AddBaseView (pDoc,
pPt2,
kViewScale2,
kRightViewOrientation,
kShadedDrawingViewStyle, // DrawingViewStyleEnum
bstrModelViewName2,
varEmpty,varEmpty,
&pBaseView2) ;
pDoc->Close (VARIANT_TRUE) ; // VARIANT_TRUE = close skipping save, obviously
As far as the "where are we looking from" option, these are the most common:
kBottomViewOrientation
kBackViewOrientation
kCurrentViewOrientation
kFrontViewOrientation
kLeftViewOrientation
kRightViewOrientation
kTopViewOrientation
These correspond in the user interface, to the view cube:
