【初级教程九】拉伸建模

leven50

本帖最后由天工开发者团队于 2024-10-28 17:15 编辑

一、扫描拉伸
概念：使用单一路径和横截面或多个路径和横截面创建扫描特征。

6.7.png

API：

ModelPtr AddSweptProtrusion(
long NumCurves,//指定在构建扫描凸出特征时使用的曲线对象的数量。
const _variant_t& TraceCurves,//包含轮廓和/或边缘对象。数组的大小等于NumCurves的值。
const _variant_t& TraceCurveTypes,//数组的大小等于NumCurves的值。包含FeaturePropertyConstants常量集合(igProfileBasedCrossSection, igEdgeBasedCrossSection)的成员，它们指定TraceCurves数组的相应成员是Profile对象还是Edge对象。
long NumSections,//指定在构造扫描凸出特征时使用的Section对象的数量。
const _variant_t& CrossSections,//包含轮廓和/或边缘对象。数组的大小等于NumSections的值
const _variant_t& CrossSectionTypes,//数组的大小等于NumSections的值。
const _variant_t& Origins,//包含定义相应截面的起始点的点。每个点表示为两个Double数组(例如，Dim dblOrigin(2) as Double;Dim Origins()作为Variant)。对于与周期性横截面(圆和椭圆)对应的此数组的成员，指定值为0，而不是指定表示点的数组。
const _variant_t& SegmentMaps,
enum FeaturePropertyConstants MaterialSide,
enum FeaturePropertyConstants StartExtentType,
double StartExtentDistance,
IDispatch* StartSurfaceOrRefPlane,
enum FeaturePropertyConstants EndExtentType,
double EndExtentDistance,
IDispatch* EndSurfaceOrRefPlane);

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示例代码：

template<typename T>
_variant_t CreateVariant(T* t, VARENUM em)
{
// 暂时支持数量为一的一维数组
SAFEARRAYBOUND bound = { 1, 0 };
SAFEARRAY* pSafeArry = SafeArrayCreate(em, 1, &bound);
SafeArrayPutElement(pSafeArry, &bound.lLbound, t);
VARIANT var;
VariantInit(&var);
var.vt = VT_ARRAY | em;
var.parray = pSafeArry;
return _variant_t(var);
}

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void AddSweptProtrusion()
{
Application* application = TGAddinApp::GetTGApp()->GetApplication();
TGPart::PartDocumentPtr pDoc = application->GetActiveDocument();
// 新建草图
TGPart::SketchPtr pSketch = pDoc->Sketches->Add();
//参考平面
TGPart::RefPlanePtr pRefplane = pDoc->GetRefPlanes()->Item(1);
// 轮廓
TGPart::ProfilePtr pProfile = pSketch->GetProfiles()->Add(pRefplane);
// 创建一个中线点为(0.0,0.0),长度为0.1，宽度为0.08的矩形
TGFrameworkSupport::Lines2dPtr pLines2d = pProfile->GetLines2d();
double cenX = 0.0, cenY = 0.0, width = 0.08, len = 0.1;
std::array<TGFrameworkSupport::Line2dPtr, 4> lines;
lines[0] = pLines2d->AddBy2Points(cenX - len / 2, cenY - width / 2, cenX + len / 2, cenY - width / 2);// 底边
lines[1] = pLines2d->AddBy2Points(cenX + len / 2, cenY - width / 2, cenX + len / 2, cenY + width / 2); // 右边
lines[2] = pLines2d->AddBy2Points(cenX + len / 2, cenY + width / 2, cenX - len / 2, cenY + width / 2); // 上边
lines[3] = pLines2d->AddBy2Points(cenX - len / 2, cenY + width / 2, cenX - len / 2, cenY - width / 2); // 左边
TGFrameworkSupport::Relations2dPtr pRelations2d = pProfile->GetRelations2d();
for (int i = 0; i < 4; i++)
{
TGFrameworkSupport::Line2dPtr pLine = lines[i];
TGFrameworkSupport::Line2dPtr pNextLine = lines[(i + 1) % 4];
pRelations2d->AddKeypoint(
pLine,
(int)TGConstants::KeypointIndexConstants::igLineEnd,
pNextLine,
(int)TGConstants::KeypointIndexConstants::igLineStart,
true);
}
pProfile->End(ProfileValidationType::igProfileClosed);
// 将该矩形设置为路径曲线
IDispatchPtr pTempTrace = static_cast<IDispatch*>(pProfile);
_variant_t TraceCurves = CreateVariant<IDispatch>(pTempTrace, VT_DISPATCH);
int TraceCurveType
= TGConstants::FeaturePropertyConstants::igProfileBasedCrossSection;
_variant_t TraceCurveTypes = CreateVariant<int>(&TraceCurveType, VT_INT);
// 绘制截面轮廓
_variant_t OrientationPlaneOrPivot(static_cast<IDispatch*>(pDoc->RefPlanes->Item(1)));
_variant_t ParentCurve(static_cast<IDispatch*>(pProfile));
pRefplane = pDoc->GetRefPlanes()->AddNormalToCurve(lines[0],
ReferenceElementConstants::igCurveStart, OrientationPlaneOrPivot,
ReferenceElementConstants::igPivotEnd, true, ParentCurve);
pSketch = pDoc->Sketches->Add();
ProfilePtr pProfileCross = pSketch->GetProfiles()->Add(pRefplane);
// 绘制一个圆心为新平面（0.0，0.0），半径为0.001的圆
pProfileCross->GetCircles2d()->AddByCenterRadius(0, 0.0, 0.01);
auto status = pProfileCross->End(ProfileValidationType::igProfileClosed);
// 将该圆设置为截面
IDispatchPtr pTempCross = static_cast<IDispatch*>(pProfileCross);
_variant_t CrossSections = CreateVariant<IDispatch>(pTempCross, VT_DISPATCH);
int CrossSectionType
= TGConstants::FeaturePropertyConstants::igProfileBasedCrossSection;
_variant_t CrossSectionTypes = CreateVariant<int>(&CrossSectionType, VT_INT);
// 截面原点，若截面为圆，此处为零
int t = 0;
_variant_t Origins = CreateVariant<int>(&t, VT_INT);
// 以圆为截面，矩形为路径的扫掠添料的操作
pDoc->Models->AddSweptProtrusion(
1,
TraceCurves,
TraceCurveTypes,
1,
CrossSections,
CrossSectionTypes,
Origins,
0, //从此往下的参数都是预备参数，无需考虑
FeaturePropertyConstants::igLeft,
FeaturePropertyConstants::igNone,
0.0,
NULL,
FeaturePropertyConstants::igNone,
0.0,
NULL
);
}

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示例效果：

二、螺旋拉伸
使用Models接口下的AddFiniteBaseHelix可创建螺旋特征:

ModelPtr Models::AddFiniteBaseHelix(struct RefAxis* HelixAxis, enum FeaturePropertyConstants AxisStart,
long NumCrossSections, SAFEARRAY** CrossSectionArray, enum FeaturePropertyConstants ProfileSide,
double Height, double Pitch, double NumberOfTurns, enum FeaturePropertyConstants HelixDir,
const _variant_t& TaperAngle = vtMissing, const _variant_t& TaperSide = vtMissing,
const _variant_t& EndPitch = vtMissing, const _variant_t& DeltaPitch = vtMissing,
const _variant_t& TaperStartRadius = vtMissing, const _variant_t& TaperEndRadius = vtMissing,
const _variant_t& FromFaceOrRefPlane = vtMissing, const _variant_t& ToFaceOrRefPlane = vtMissing);

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void AddHelixProtrusion()
{
namespace pt = TGPart;
namespace fwp = TGFrameworkSupport;
pt::PartDocumentPtr pPartDoc = SEAPP->GetActiveDocument();
pt::RefPlanePtr pRefPlaen = pPartDoc->GetRefPlanes()->Item(2l);
pt::ProfilePtr pProfile = pPartDoc->GetProfileSets()->Add()->GetProfiles()->Add(pRefPlaen);
fwp::Line2dPtr pLine = pProfile->GetLines2d()->AddBy2Points(0, -0.05, 0, 0.05);
pt::RefAxisPtr pRefAxis = pProfile->SetAxisOfRevolution(pLine);
fwp::Circle2dPtr pCrossSection = pProfile->GetCircles2d()->AddByCenterRadius(0.05, -0.05, 0.01);
ATL::CComSafeArray<IDispatch*> crossSectionArray(1);
crossSectionArray[0] = pProfile;
pPartDoc->GetModels()->AddFiniteBaseHelix(pRefAxis, // 螺旋轴
pt::igStart, // pt::igStart表示从轴定义的线段起点向终点向螺旋，pt::igEnd表示从轴定义的线段终点向起点螺旋
1, crossSectionArray.GetSafeArrayPtr(), // 传入横截面
pt::igRight, // 为未来开放路径预留，暂时无用，pt::igRight和pt::igLeft为有效值
0.1, // 螺高，暂时无用
0.05, // 螺距
2, // 螺数
pt::igRight // pt::igRight右旋，pt::igLeft左旋
);
}

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上述代码演示了创建螺旋拉伸的一般过程，运行效果如下。
6.2.png

三、法向拉伸
概念:法向拉伸通过拉伸位于零件面上的封闭曲线构造垂直于该面的拉伸,适用于使用文本轮廓或其他草图元素在非平整面构建特征时。与普通拉伸不同，法向拉伸命令并不基于轮廓。要构造法向拉伸特征，有几个前提:
一、已有一个设计模型
二、已将一个草图或草图中的某些轮廓投影至设计模型中。
使用下述Api可以创建一个法向拉伸特征。

NormalToFaceProtrusions::Add(
long NumberOfInputCurves,// 传入的edges个数
const _variant_t& InputCurvesSetArray, // edges
enum FeaturePropertyConstants LongestCurveSide, // pt::igLeft 向外拉伸(加料) pt::igRight 向内拉伸(除料)
double offsetDistance, // 拉伸厚度
enum FeaturePropertyConstants FaceContainment// pt::igFacesTouchingCurvesOnly 仅修改与曲线接触的面
// pt::igAllFaces 修改曲线图内的所有面
);

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下述代码演示了创建一个法向拉伸特征的完整过程：

void AddNormalProtrusion()
{
namespace pt = TGPart;
namespace gm = TGGeometry;
pt::PartDocumentPtr pPartDoc = SEAPP->GetActiveDocument();
assert(pPartDoc);
// 首先创建一个圆柱
pt::RefPlanePtr pYOZPlane = pPartDoc->GetRefPlanes()->Item(2l);
pt::ProfilePtr pProfile = pPartDoc->GetSketches()->AddByPlane(pYOZPlane)->GetProfile();
pProfile->GetCircles2d()->AddByCenterRadius(0.0, 0.0, 0.2);
ATL::CComSafeArray<IDispatch*> aProfiles(1);
aProfiles.SetAt(0, pProfile);
pt::ModelPtr pCylinderModel = pPartDoc->GetModels()->AddFiniteExtrudedProtrusion(1, aProfiles.GetSafeArrayPtr(),
pt::igSymmetric, 0.6);
// 在一个新的草图上创建一个圆
pt::RefPlanePtr pXOYPlane = pPartDoc->GetRefPlanes()->Item(1l);
pt::SketchPtr pSketch = pPartDoc->GetSketches()->AddByPlane(pXOYPlane);
pt::ProfilePtr pProfileScd = pSketch->GetProfile();
pProfileScd->GetCircles2d()->AddByCenterRadius(0.0, 0.0, 0.05);
// 投影圆所在草图到圆柱面上
gm::BodyPtr pBody = pCylinderModel->GetBody();
gm::FacesPtr pFaces = pBody->GetFaces(gm::igQueryCylinder);
assert(pFaces->GetCount() > 0);
gm::FacePtr pFace = pFaces->Item(1l);
long faceCnt = pFaces->GetCount();
pt::ProjectCurvesPtr pProjCvs = pPartDoc->GetConstructions()->GetProjectCurves();
pt::RefPlanePtr pDestPlane = pPartDoc->GetRefPlanes()->AddParallelByDistance(pXOYPlane, 0.2, pt::igNormalSide);
pt::ProjectCurvePtr pProjCv = pProjCvs->Add(pSketch, pFace, pDestPlane, pt::igRight, pt::igProjectOptionProject);
// 法向拉伸
gm::EdgesPtr pProjEdges = pProjCv->GetEdges(gm::igQueryAll);
long projEdgeCnt = pProjEdges->GetCount();
ATL::CComSafeArray<IDispatch*> aEdges(projEdgeCnt);
for (long i = 0; i < projEdgeCnt; i++)
{
aEdges.SetAt(i, pProjEdges->Item(i + 1));
}
_variant_t varEdges;
varEdges.parray = aEdges.Detach();
varEdges.vt = VT_ARRAY | VT_DISPATCH;
pCylinderModel->GetNormalToFaceProtrusions()->Add(projEdgeCnt, // 传入的edges个数
varEdges, // edges
pt::igLeft, // pt::igLeft 向外拉伸(加料) pt::igRight 向内拉伸(除料)
0.01, // 拉伸厚度
pt::igFacesTouchingCurvesOnly // pt::igFacesTouchingCurvesOnly 仅修改与曲线接触的面
// pt::igAllFaces 修改曲线图内的所有面
);
}

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总体思路为在创建一个圆柱体，并将一个圆投影至圆柱面后，调用NormalToFaceProtrusions::Add方法，运行效果如下。

四、加厚
加厚命令通过偏移一个或多个面来加厚零件,SDK中使用Thickens::Add方法用于加厚。
其原型为：

ThickenPtr Add(
enum FeaturePropertyConstants Side, //加厚方法
double offsetDistance, // 加厚厚度
long NumberOfFaces, // 要加厚的面的个数
SAFEARRAY** Faces // 要加厚的面集
)

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下述代码演示了添加加厚特征的一般过程：

// 添加加厚特征
void AddThickenFeature()
{
namespace pt = TGPart;
namespace gm = TGGeometry;
pt::PartDocumentPtr pPartDoc = SEAPP->GetActiveDocument();
assert(pPartDoc);
// 使用对称拉伸，创建一个圆柱，圆柱顶底面法向分别为左、右视图
// 圆柱底面半径0.1,圆柱高0.6
pt::RefPlanePtr pYOZPlane = pPartDoc->GetRefPlanes()->Item(2l);
pt::ProfilePtr pProfile = pPartDoc->GetSketches()->AddByPlane(pYOZPlane)->GetProfile();
pProfile->GetCircles2d()->AddByCenterRadius(0.0, 0.0, 0.1);
ATL::CComSafeArray<IDispatch*> aProfiles(1);
aProfiles.SetAt(0, pProfile);
pt::ModelPtr pCylinderModel = pPartDoc->GetModels()->AddFiniteExtrudedProtrusion(1, aProfiles.GetSafeArrayPtr(),
pt::igSymmetric, 0.6);
// 加厚顶、底面其中之一，使不对称
gm::BodyPtr pBody = pCylinderModel->GetBody();
gm::FacesPtr pFaces = pBody->GetFaces(gm::igQueryPlane);
assert(pFaces->GetCount() == 2);
ATL::CComSafeArray<IDispatch*> aFaces(1);
aFaces.SetAt(0, pFaces->Item(1l));
// 朝外侧加厚0.2
pCylinderModel->GetThickens()->Add(pt::igRight, // 加厚方向一般为igRight(外侧),
// 对于单个的曲面特征可以往两侧加厚，则可为igLeft 或 igBoth(未验证)
0.2, // 加厚厚度
1l, aFaces.GetSafeArrayPtr() // 模型中要加厚的面
);
}

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运行效果如下：

五、实体拉伸
使用SolidSweptProtrusions::Add方法可以基于已知实体和扫掠路径添加实体扫掠特征，这个方法的原型为：

SolidSweptProtrusionPtr Add(IDispatch* pTargetBody, //目标实体要求为gm::Body
IDispatch* pToolBody, // 原始实体要求为gm::Body 可与pTargetBody相等
IDispatch* pPath, // 扫掠路径，要求为pt::Profile
IDispatch* pRotationAxis, // 原始实体的旋转轴,对于圆柱、圆锥体，可传nullptr
IDispatch* pLockDirection,
VARIANT_BOOL bToolOnPath, // true时，在路径上旋转工具体;false时，垂直于曲面放置工具
VARIANT_BOOL bProtrusion // true时，拉伸;false时，除料
);

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void AddSolidSweptExtruProtrusion()
{
namespace pt = TGPart;
namespace fwp = TGFrameworkSupport;
namespace gm = TGGeometry;
pt::PartDocumentPtr pPartDoc = SEAPP->GetActiveDocument();
assert(pPartDoc);
// 创建一个圆柱体用于演示
pt::ProfilePtr pProfile = pPartDoc->GetSketches()->AddByPlane(pPartDoc->GetRefPlanes()->Item(1l))->GetProfile();
pProfile->GetCircles2d()->AddByCenterRadius(0, 0, 0.1); // 中心位于原点，半径0.1
ATL::CComSafeArray<IDispatch*> aProfiles(1);
aProfiles.SetAt(0, pProfile);
pt::ModelPtr pModelFst = pPartDoc->GetModels()->AddFiniteExtrudedProtrusion(aProfiles.GetCount(), aProfiles.GetSafeArrayPtr(), pt::igRight, 1.0);
// 创建扫掠路径(一条直线)
pt::RefPlanePtr pXOYPlane = pPartDoc->GetRefPlanes()->Item(1l);
pt::ProfilePtr pXOYProfile = pPartDoc->GetSketches()->AddByPlane(pPartDoc->GetRefPlanes()->Item(1l))->GetProfile();
fwp::Line2dPtr pLine2d = pXOYProfile->GetLines2d()->AddBy2Points(0, 0, 0.5, 0);
// 进行实体扫掠
pt::SolidSweptProtrusionsPtr pSweptProtrusions = pModelFst->GetSolidSweptProtrusions();
assert(pModelFst->GetExtrudedProtrusions()->GetCount() > 0);
pt::ExtrudedProtrusionPtr pCylinder = pModelFst->GetExtrudedProtrusions()->Item(1l);
gm::BodyPtr pToolBody = pModelFst->GetBody();
gm::BodyPtr pTargetBody = pToolBody;
pt::SolidSweptProtrusionPtr pBodySwept = pSweptProtrusions->Add(pTargetBody, pToolBody,
pXOYProfile, nullptr, nullptr, VARIANT_TRUE, VARIANT_TRUE);
}

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上述代码演示了使用这个方法的一般过程,运行效果如下。
6.5.png

六、放样拉伸
放样拉伸操作通过连接一系列闭合截面形成三维模型，可以使用Models::AddLoftedProtrusion方法进行放样拉伸。

template<typename T>
ATL::CComSafeArray<T> ToComSafeArray(std::initializer_list<T> const& initial_list)
{
ATL::CComSafeArray<T> comArray((ULONG)initial_list.size());
long i = 0;
for (auto it = initial_list.begin(); it != initial_list.end(); ++it)
{
comArray.SetAt(i, *it);
i++;
}
return comArray;
}
template<typename T>
_variant_t ToArrayVar(std::initializer_list<T> const& initial_list)
{
VARENUM varEnum;
if (std::is_same_v<T, double>)
{
varEnum = VT_R8;
}
else if (std::is_same_v<T, int>)
{
varEnum = VT_I4;
} else if (std::is_same_v<T, float>)
{
varEnum = VT_R4;
}
else if (std::is_same_v<T, IDispatch*>)
{
varEnum = VT_DISPATCH;
}
else if (std::is_same_v<T, long>)
{
varEnum = VT_I8;
}
else
{
static_assert("未定义的类型");
}
ATL::CComSafeArray<T> comArray = ToComSafeArray(initial_list);
_variant_t var;
var.vt = VT_ARRAY| varEnum;
var.parray = comArray.Detach();
return var;
}
_variant_t ToEmbedVar(std::initializer_list<_variant_t> const& initial_list)
{
SAFEARRAYBOUND arrBound{ initial_list.size(),0};
SAFEARRAY* psa = SafeArrayCreate(VT_VARIANT, 1, &arrBound);
long i = 0;
for (auto it = initial_list.begin(); it != initial_list.end(); ++it,++i)
{
SafeArrayPutElement(psa, &i, (void*)(&(*it)));
}
_variant_t var;
var.vt = VT_ARRAY | VT_VARIANT;
var.parray = psa;
return var;
}
void CreateRectange(TGPart::ProfilePtr pProfile, double cenX, double cenY, double len, double width)
{
namespace fwp = TGFrameworkSupport;
// 矩形在天工CAD中由四条首尾相连的直线组成
fwp::Lines2dPtr pLines2d = pProfile->GetLines2d();
std::array<fwp::Line2dPtr, 4> lines;
lines[0] = pLines2d->AddBy2Points(cenX - len / 2, cenY - width / 2, cenX + len / 2, cenY - width / 2);// 底边
lines[1] = pLines2d->AddBy2Points(cenX + len / 2, cenY - width / 2, cenX + len / 2, cenY + width / 2); // 右边
lines[2] = pLines2d->AddBy2Points(cenX + len / 2, cenY + width / 2, cenX - len / 2, cenY + width / 2); // 上边
lines[3] = pLines2d->AddBy2Points(cenX - len / 2, cenY + width / 2, cenX - len / 2, cenY - width / 2); // 左边
fwp::Relations2dPtr pRelations2d = pProfile->GetRelations2d();
for (int i = 0; i < 3; i++)
{
fwp::Line2dPtr pLine = lines[i];
fwp::Line2dPtr pNextLine = lines[(i + 1) % 4];
pRelations2d->AddKeypoint(
pLine,
(int)TGConstants::KeypointIndexConstants::igLineEnd,
pNextLine,
(int)TGConstants::KeypointIndexConstants::igLineStart,
true);
}
pProfile->End(TGPart::ProfileValidationType::igProfileClosed);
}
void AddLoftProtrusion()
{
namespace pt = TGPart;
namespace fwp = TGFrameworkSupport;
pt::PartDocumentPtr pPartDoc = SEAPP->GetActiveDocument();
pt::RefPlanePtr pSidePlane = pPartDoc->GetRefPlanes()->Item(2l); // 侧平面
// 左剖面，画一个矩形
pt::RefPlanePtr pFstPlane = pPartDoc->GetRefPlanes()->AddParallelByDistance(pSidePlane, 0.5, pt::igReverseNormalSide);
pt::ProfilePtr pFstProfile = pPartDoc->GetSketches()->AddByPlane(pFstPlane)->GetProfile();
CreateRectange(pFstProfile, 0, 0, 0.6, 0.5);
// 中间剖面，画一个圆
pt::ProfilePtr pScdProfile = pPartDoc->GetSketches()->AddByPlane(pSidePlane)->GetProfile();
pScdProfile->GetCircles2d()->AddByCenterRadius(0, 0, 0.2);
// 右剖面，画一个矩形
pt::RefPlanePtr pTrdPlane = pPartDoc->GetRefPlanes()->AddParallelByDistance(pSidePlane, 0.5, pt::igNormalSide);
pt::SketchsPtr pSketchs = pPartDoc->GetSketches();
pt::SketchPtr pSketch = pPartDoc->GetSketches()->AddByPlane(pTrdPlane);
pt::ProfilePtr pTrdProfile = pSketch->GetProfile();
CreateRectange(pTrdProfile, 0, 0, 0.6, 0.5);
// 创建放样拉伸特征
_variant_t sectionArr = ToArrayVar({
(IDispatch*)pFstProfile.GetInterfacePtr(),(IDispatch*)pScdProfile.GetInterfacePtr(),
(IDispatch*)pTrdProfile.GetInterfacePtr(),});
_variant_t sectTypeArr = ToArrayVar({
(int)pt::igProfileBasedCrossSection,
(int)pt::igProfileBasedCrossSection,
(int)pt::igProfileBasedCrossSection});
_variant_t sectionFstStPoints = ToArrayVar({ -0.3,-0.25 });
_variant_t sectionTrdStPoints = ToArrayVar({ -0.3,-0.25 });
_variant_t orginArr = ToEmbedVar({ sectionFstStPoints,_variant_t(0),sectionTrdStPoints });
pt::ModelsPtr pModels = pPartDoc->GetModels();
pModels->AddLoftedProtrusion(3, sectionArr, sectTypeArr, orginArr, 0, pt::igLeft,
pt::igNone, 0.0, nullptr, pt::igNone, 0.0, nullptr, pt::igNone, 0.0, pt::igNone, 0.0);
}

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上述代码演示了使用这个方法的一般过程，运行效果如下。
6.6.png

AddLoftedProtrusion的原型为：

ModelPtr AddLoftedProtrusion (
long NumSections,const _variant_t & CrossSections,const _variant_t & CrossSectionTypes,
const _variant_t & Origins,const _variant_t & SegmentMaps,enum FeaturePropertyConstants MaterialSide,
enum FeaturePropertyConstants StartExtentType,double StartExtentDistance,IDispatch * StartSurfaceOrRefPlane,
enum FeaturePropertyConstants EndExtentType,double EndExtentDistance,IDispatch * EndSurfaceOrRefPlane,
enum FeaturePropertyConstants StartTangentType,double StartTangentMagnitude,enum FeaturePropertyConstants EndTangentType,
double EndTangentMagnitude,const _variant_t & NumGuideCurves = vtMissing,
const _variant_t & GuideCurves = vtMissing );

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      虽然它看起来参数众多，但是一般只需要关注前四个参数，后面的参数要么是预留的，要么暂时是固定项。
      NumSections 截面个数
      CrossSections 用于传入截面，VT_ARRAY|VT_DISPATCH类型的变体，要求其内Dispatch个数和截面个数相同
      CrossSectionTypes 用于传入截面类型，VT_ARRAY|VT_I4型的变体，要求数组元素个数与截面个数相同，每个都用于描述CrossSections对应的截面类型
      Origins 用于描述每个截面的起始点，这些起始点集影响拉伸效果。VT_ARRAY|VT_VARIANT类型的变体，要求数组元素个数与截面个数相同。如果是周期性的截面(如圆、椭圆)，作为元素的变体可以只传0。否则作为元素的变体是VT_ARRAY|VT_R8类型的数组，元素个数为2。

【初级教程九】拉伸建模

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