NX二次开发-UFUN创建扫掠UF_MODL_create_sweep

这个函数挺复杂的，我也是参考别人去做的。但是我还是没有做出来多段引导线的。

我们在做钻头螺旋槽的时候，一般都是拿一个封闭截面，三条引导线去做扫掠。

后来我是录制NXOPEN去做的

参考资料 https://www.ugapi.com/thread-10038.html

NX9+VS2012

#include <uf_object_types.h>
#include <NXOpen/ListingWindow.hxx>
#include <NXOpen/NXMessageBox.hxx>
#include <NXOpen/UI.hxx>
#include <NXOpen/Annotations.hxx>
#include <NXOpen/Assemblies_Component.hxx>
#include <NXOpen/Assemblies_ComponentAssembly.hxx>
#include <NXOpen/Body.hxx>
#include <NXOpen/BodyCollection.hxx>
#include <NXOpen/Face.hxx>
#include <NXOpen/Line.hxx>
#include <NXOpen/NXException.hxx>
#include <NXOpen/NXObject.hxx>
#include <NXOpen/Part.hxx>
#include <NXOpen/PartCollection.hxx>
#include <NXOpen/CartesianCoordinateSystem.hxx>
#include <NXOpen/CoordinateSystemCollection.hxx>
#include <NXOpen/Features_FeatureCollection.hxx>
#include <NXOpen/Features_HelixBuilder.hxx>
#include <NXOpen/XformCollection.hxx>
#include <uf.h>
#include <uf_modl.h>
#include <uf_curve.h>
#include <uf_vec.h>



tag_t CreateHelical(string strVal[5], double origin[3], double xDirection[3], double yDirection[3])
{
    Session *theSession = Session::GetSession();
    Part *workPart(theSession->Parts()->Work());
    Part *displayPart(theSession->Parts()->Display());

    Features::Helix *nullFeatures_Helix(NULL);

    Features::HelixBuilder *helixBuilder1;
    helixBuilder1 = workPart->Features()->CreateHelixBuilder(nullFeatures_Helix);

    helixBuilder1->SetOrientationOption(Features::HelixBuilder::OrientationOptionsSpecified);

    helixBuilder1->StartAngle()->SetRightHandSide(strVal[0].c_str()); //角度
    helixBuilder1->SizeLaw()->Value()->SetRightHandSide(strVal[1].c_str()); //直径
    helixBuilder1->PitchLaw()->Value()->SetRightHandSide(strVal[2].c_str());//螺距
    helixBuilder1->StartLimit()->Expression()->SetRightHandSide(strVal[3].c_str());//起始
    helixBuilder1->EndLimit()->Expression()->SetRightHandSide(strVal[4].c_str());//终止

    Point3d originCoord(origin[0], origin[1], origin[2]);
    Vector3d xDirection1(xDirection[0], xDirection[1], xDirection[2]);
    Vector3d yDirection1(yDirection[0], yDirection[1], yDirection[2]);

    Xform *xform1;
    xform1 = workPart->Xforms()->CreateXform(originCoord, xDirection1, yDirection1, SmartObject::UpdateOptionWithinModeling, 1.0);

    CartesianCoordinateSystem *cartesianCoordinateSystem1;
    cartesianCoordinateSystem1 = workPart->CoordinateSystems()->CreateCoordinateSystem(xform1, SmartObject::UpdateOptionWithinModeling);

    helixBuilder1->SetCoordinateSystem(cartesianCoordinateSystem1);

    NXObject *nXObject1;
    nXObject1 = helixBuilder1->Commit();
    helixBuilder1->Destroy();

    return nXObject1->Tag();
}



void MyClass::do_it()
{

    // TODO: add your code here
    
    UF_initialize();

    //设置螺旋线参数
    string strVal[5] = { "0", "8.5", "56", "0", "285" };
    double origin[3] = { 0.0, 0.0, 0.0 };
    double xd[3] = { 1.0, 1.0, 0.0 };
    double yd[3] = { 0.0, 1.0, 0.0 };
    //创建螺旋线
    tag_t helicalTag = CreateHelical(strVal, origin, xd, yd);

    //创建三点整圆
    double first_point1[3] = { -2.0, 0.0, 0.0 };
    double second_point1[3] = { 0.0, 2.0, 0.0 };
    double third_point1[3] = { 2.0, 0.0, 0.0 };
    tag_t arc_tag1 = NULL_TAG;
    UF_CURVE_create_arc_thru_3pts(2, first_point1, second_point1, third_point1, &arc_tag1);

    //定义引导线
    UF_STRING_t s_guide;
    UF_MODL_init_string_list(&s_guide);
    UF_MODL_create_string_list(1, 1, &s_guide);//第二个参数为引导线数量
    s_guide.num = 1;
    s_guide.string[0] = 1;//引导线数量
    s_guide.dir[0] = 1;
    s_guide.id[0] = helicalTag; //将前面创建的螺旋线tag作为引导线

    //定义截面线
    UF_STRING_t    s_section;
    UF_MODL_init_string_list(&s_section);
    UF_MODL_create_string_list(1, 1, &s_section);//第二个参数为截面线数量
    s_section.num = 1;
    s_section.string[0] = 1;//截面线数量
    s_section.dir[0] = 1;
    s_section.id[0] = arc_tag1;//输入截面线tag

    //定义脊线
    UF_STRING_t s_spine;
    UF_MODL_init_string_list(&s_spine);

    //设置定位方法
    UF_METHOD_t orientation;
    orientation.method = 4;//定位方法(方向)4是固定
    orientation.value[0] = 0;
    orientation.value[1] = 1;
    orientation.value[2] = 0;
    orientation.id = 0;
    orientation.inter = 0;

    //设置缩放方法
    UF_METHOD_t scaling;
    scaling.method = 1;
    scaling.value[0] = 1;
    scaling.value[1] = 0;
    scaling.value[2] = 0;
    scaling.id = 0;
    scaling.inter = 0;

    int alignment = 1;//调整方法,参数还是弧长
    int inter = 1;//插值方法,线性还是立方
    int body_type = 1;//设置扫掠片体还是实体
    double tol[3] = { 0, 0, 0 };//指定公差(全为0就是勾选保留形状)
    tag_t body_id = NULL_TAG;
    //创建扫掠
    UF_MODL_create_sweep(&s_guide, &s_section, &s_spine, &orientation, &scaling, &alignment, &inter, &body_type, UF_NULLSIGN, tol, &body_id);

    //释放
    UF_MODL_free_string_list(&s_guide);
    UF_MODL_free_string_list(&s_section);
    UF_MODL_free_string_list(&s_spine);


    UF_terminate();

}


Caesar卢尚宇
2020年8月8日