[C# SolidWorks API] ロフトを使ったモデリング

2015/4/28 2015/5/8 Computer, SolidWorks

スケッチした形状を断面形状としてロフト機能を利用すると，さまざまな形状をモデリングすることができます．試しに，”SolidWorks Loft”でGoogle検索するとこのような形状を見つけることができました．そんな重要かつ便利なロフト機能をAPIから使ってみましょう．

下面と上面の断面形状をスケッチして，ロフト機能で3次元形状を作ってみます．今回は簡単のため，断面形状は大きさの異なる四角形としましょう．

ロフト機能で3次元形状を作る手順は次の通りです．

1．下面の断面形状をスケッチする
2．上面をスケッチするための参照面を作成する
3．参照面に上面の断面形状をスケッチする
4．下面と上面をつなぐガイドカーブを作成する
5．ロフト機能で下面と上面をつなぐ

1と3の断面形状のスケッチは[C# SolidWorks API] 四角形をスケッチするを参考にしてください．

コーディングでは，次の3つのメソッドを定義します．

1．基準となるoriginePlaneから距離distanceだけ離れた位置に参照面を作成するメソッド
　createReferencePlane(string originPlane, double distance)

2．上下面の名前bottomSketchName，topSketchNameと断面寸法からガイドカーブを作成するメソッド
　string sketchGuideCurve(string bottomSketchName, string topSketchName,
　　　double bWidth, double bHeight, double tWidth, double tHeight, double height)

3．上下面とガイドカーブの名前からロフトを実行するメソッド
　loft(string bottomSketchName, string topSketchName,
　　　string guideCurveSketchName)

上下面とガイドカーブの寸法，位置関係については，下の図を参照してください．

実行例

下面: bWidth = 0.2 m, bHeight = 0.2 m
上面: tWidth = 0.4 m, tHeight = 0.1 m
Height = 1.0 [m]
として，3次元形状を作成した様子です．基準面には”平面”を指定しています．

コード

全体のプログラムは次のようになります．

using System;
using System.Collections.Generic;
using System.Linq;
using System.Text;
using System.Threading.Tasks;

// for SolidWorks API
using SolidWorks.Interop.cosworks;
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;

// for Debuging
using System.Diagnostics;

namespace swLoft
{
    class Program
    {
        SldWorks.ISldWorks swApp = null;
        IModelDoc2 modelDoc = default(ModelDoc2);

        void startSW()
        {
            swApp = new SldWorks.SldWorks();
            Debug.Assert(swApp != null);
            swApp.Visible = true;
        }


        void createNewPartDocument()
        {
            string partTemplate = swApp.GetUserPreferenceStringValue((int)swUserPreferenceStringValue_e.swDefaultTemplatePart);
            if ((partTemplate != null) && (partTemplate != ""))
            {
                modelDoc = (IModelDoc2)swApp.NewDocument(partTemplate, (int)swDwgPaperSizes_e.swDwgPaperA2size, 0.0, 0.0);

            }
        }


        string sketchRectangle(string planeName, double width, double height)
        {
            string sketchName = null;

            IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;
            bool isSelected = dExt.SelectByID2(planeName, "PLANE", 0, 0, 0, false, 0, null, 0);
            
            if (isSelected) {
                ISketchManager sketchMgr = modelDoc.SketchManager;
                
                double halfWidth = width / 2.0;
                double halfHeight = height / 2.0;

                sketchMgr.InsertSketch(true); 
                sketchMgr.CreateCornerRectangle(-halfWidth, halfHeight, 0, halfWidth, -halfHeight, 0);
                sketchMgr.InsertSketch(true); 
                sketchName = getItemName("SKETCH", -halfWidth, 0, halfHeight);
            }

            return sketchName;

        }


        string sketchGuideCurve(string bottomSketchName, string topSketchName, double bWidth, double bHeight, double tWidth, double tHeight, double height)
        {
            string sketchName = null;
            IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

            bool isSelected = dExt.SelectByID2("Point1@" + bottomSketchName, "EXTSKETCHPOINT", 0, 0, 0, false, 1, null, 0);
            Debug.Assert(isSelected);
            isSelected = dExt.SelectByID2("Point1@" + topSketchName, "EXTSKETCHPOINT", 0, 0, 0, true, 1, null, 0);
            Debug.Assert(isSelected);
            modelDoc.Insert3DSplineCurve(false);

            double bottomW = bWidth / 2.0;
            double bottomH = bHeight / 2.0;
            double topW = tWidth / 2.0;
            double topH = tHeight / 2.0;
            sketchName = getItemName("EDGE", -(topW + bottomW) / 2.0, height / 2.0, -(topH + bottomH) / 2.0);

            return sketchName;

        }


        string createReferencePlane(string originPlaneName, double distance)
        {
            string refPlaneName = null;

            IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

            // Create Reference Plane
            bool isSelected = dExt.SelectByID2(originPlaneName, "PLANE", 0, 0, 0, false, 0, null, 0);
            if (isSelected) {
                IFeatureManager featureMgr = (IFeatureManager)modelDoc.FeatureManager;
                IRefPlane rPlane = (IRefPlane)featureMgr.InsertRefPlane((int)swRefPlaneReferenceConstraints_e.swRefPlaneReferenceConstraint_Distance, distance,
                                                                         0, 0, 0, 0);
                refPlaneName = getItemName("PLANE", 0, distance, 0);
            }

            return refPlaneName;

        }
        

        void loft(string bottomSketchName, string topSketchName, string guideCurveSketchName)
        {
            IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

            bool isSelected = dExt.SelectByID2(bottomSketchName, "SKETCH", 0, 0, 0, false, 1, null, 0);
            Debug.Assert(isSelected);
            
            isSelected = dExt.SelectByID2(topSketchName, "SKETCH", 0, 0, 0, true, 1, null, 0);
            Debug.Assert(isSelected);
            
            isSelected = dExt.SelectByID2(guideCurveSketchName, "REFERENCECURVES", 0, 0, 0, true, 2, null, 0);
            Debug.Assert(isSelected);
            
            IFeatureManager featureMgr = (IFeatureManager)modelDoc.FeatureManager;
            featureMgr.InsertProtrusionBlend2(false, true, false, 1, 0, 0, 1, 1, true, true, false, 0, 0, 0, true, true, true,
                                       (int)swGuideCurveInfluence_e.swGuideCurveInfluenceNextGlobal);
        }


        void createShape(double bWidth, double bHeight, double tWidth, double tHeight, double height)
        {
            // Sketch Bottom
            string bottomSketchName = sketchRectangle("平面", bWidth, bHeight);

            // Sketch Top
            string refPlaneName = createReferencePlane("平面", height);
            string topSketchName = sketchRectangle(refPlaneName, tWidth, tHeight);

            // Sketch Guide Curve
            string guideCurveSketchName = sketchGuideCurve(bottomSketchName, topSketchName, bWidth, bHeight, tWidth, tHeight, height);

            // Loft
            loft(bottomSketchName, topSketchName, guideCurveSketchName);
        }


        string getItemName(string type, double x, double y, double z)
        {
            string featureName = null;

            IModelDocExtension dExt = modelDoc.Extension;

            // まず，選択する
            bool status = dExt.SelectByID2("", type, x, y, z, true, 0, null, 0);
            if (status)
            {
                // 対象を取得する
                IFeature feature = (IFeature)(modelDoc.SelectionManager).getSelectedObject6(1, -1);
                // 選択を解除する
                modelDoc.ClearSelection2(true);
                Debug.Assert(feature != null);
                string fType = null;
                featureName = feature.GetNameForSelection(out fType);
                Debug.Print(fType + ": " + featureName);
            }

            return featureName;
        }

        void setView(int viewType)
        {
            modelDoc.ShowNamedView2("", viewType);
            modelDoc.ViewZoomtofit2();
        }

        static void Main(string[] args)
        {
            Program p = new Program();

            p.startSW();

            p.createNewPartDocument();

            Console.WriteLine("Creating Shape");
            double bWidth = 0.2;
            double bHeight = 0.2;
            double tWidth = 0.4;
            double tHeight = 0.1;
            double height = 1.0;
            p.createShape(bWidth, bHeight, tWidth, tHeight, height);

            p.setView((int)swStandardViews_e.swIsometricView);
        }
    }
}

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using System;

using System.Collections.Generic;

using System.Linq;

using System.Text;

using System.Threading.Tasks;

// for SolidWorks API

using SolidWorks.Interop.cosworks;

using SolidWorks.Interop.sldworks;

using SolidWorks.Interop.swconst;

// for Debuging

using System.Diagnostics;

namespace swLoft

{

class Program

{

SldWorks.ISldWorks swApp = null;

IModelDoc2 modelDoc = default(ModelDoc2);

void startSW()

{

swApp = new SldWorks.SldWorks();

Debug.Assert(swApp != null);

swApp.Visible = true;

}

void createNewPartDocument()

{

string partTemplate = swApp.GetUserPreferenceStringValue((int)swUserPreferenceStringValue_e.swDefaultTemplatePart);

if ((partTemplate != null) && (partTemplate != ""))

{

modelDoc = (IModelDoc2)swApp.NewDocument(partTemplate, (int)swDwgPaperSizes_e.swDwgPaperA2size, 0.0, 0.0);

}

string sketchRectangle(string planeName, double width, double height)

{

string sketchName = null;

IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

bool isSelected = dExt.SelectByID2(planeName, "PLANE", 0, 0, 0, false, 0, null, 0);

if (isSelected) {

ISketchManager sketchMgr = modelDoc.SketchManager;

double halfWidth = width / 2.0;

double halfHeight = height / 2.0;

sketchMgr.InsertSketch(true);

sketchMgr.CreateCornerRectangle(-halfWidth, halfHeight, 0, halfWidth, -halfHeight, 0);

sketchMgr.InsertSketch(true);

sketchName = getItemName("SKETCH", -halfWidth, 0, halfHeight);

}

return sketchName;

}

string sketchGuideCurve(string bottomSketchName, string topSketchName, double bWidth, double bHeight, double tWidth, double tHeight, double height)

{

string sketchName = null;

IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

bool isSelected = dExt.SelectByID2("Point1@" + bottomSketchName, "EXTSKETCHPOINT", 0, 0, 0, false, 1, null, 0);

Debug.Assert(isSelected);

isSelected = dExt.SelectByID2("Point1@" + topSketchName, "EXTSKETCHPOINT", 0, 0, 0, true, 1, null, 0);

Debug.Assert(isSelected);

modelDoc.Insert3DSplineCurve(false);

double bottomW = bWidth / 2.0;

double bottomH = bHeight / 2.0;

double topW = tWidth / 2.0;

double topH = tHeight / 2.0;

sketchName = getItemName("EDGE", -(topW + bottomW) / 2.0, height / 2.0, -(topH + bottomH) / 2.0);

return sketchName;

}

string createReferencePlane(string originPlaneName, double distance)

{

string refPlaneName = null;

IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

// Create Reference Plane

bool isSelected = dExt.SelectByID2(originPlaneName, "PLANE", 0, 0, 0, false, 0, null, 0);

if (isSelected) {

IFeatureManager featureMgr = (IFeatureManager)modelDoc.FeatureManager;

IRefPlane rPlane = (IRefPlane)featureMgr.InsertRefPlane((int)swRefPlaneReferenceConstraints_e.swRefPlaneReferenceConstraint_Distance, distance,

0, 0, 0, 0);

refPlaneName = getItemName("PLANE", 0, distance, 0);

}

return refPlaneName;

}

void loft(string bottomSketchName, string topSketchName, string guideCurveSketchName)

{

IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

bool isSelected = dExt.SelectByID2(bottomSketchName, "SKETCH", 0, 0, 0, false, 1, null, 0);

Debug.Assert(isSelected);

isSelected = dExt.SelectByID2(topSketchName, "SKETCH", 0, 0, 0, true, 1, null, 0);

Debug.Assert(isSelected);

isSelected = dExt.SelectByID2(guideCurveSketchName, "REFERENCECURVES", 0, 0, 0, true, 2, null, 0);

Debug.Assert(isSelected);

IFeatureManager featureMgr = (IFeatureManager)modelDoc.FeatureManager;

featureMgr.InsertProtrusionBlend2(false, true, false, 1, 0, 0, 1, 1, true, true, false, 0, 0, 0, true, true, true,

(int)swGuideCurveInfluence_e.swGuideCurveInfluenceNextGlobal);

}

void createShape(double bWidth, double bHeight, double tWidth, double tHeight, double height)

{

// Sketch Bottom

string bottomSketchName = sketchRectangle("平面", bWidth, bHeight);

// Sketch Top

string refPlaneName = createReferencePlane("平面", height);

string topSketchName = sketchRectangle(refPlaneName, tWidth, tHeight);

// Sketch Guide Curve

string guideCurveSketchName = sketchGuideCurve(bottomSketchName, topSketchName, bWidth, bHeight, tWidth, tHeight, height);

// Loft

loft(bottomSketchName, topSketchName, guideCurveSketchName);

}

string getItemName(string type, double x, double y, double z)

{

string featureName = null;

IModelDocExtension dExt = modelDoc.Extension;

// まず，選択する

bool status = dExt.SelectByID2("", type, x, y, z, true, 0, null, 0);

if (status)

{

// 対象を取得する

IFeature feature = (IFeature)(modelDoc.SelectionManager).getSelectedObject6(1, -1);

// 選択を解除する

modelDoc.ClearSelection2(true);

Debug.Assert(feature != null);

string fType = null;

featureName = feature.GetNameForSelection(out fType);

Debug.Print(fType + ": " + featureName);

}

return featureName;

}

void setView(int viewType)

{

modelDoc.ShowNamedView2("", viewType);

modelDoc.ViewZoomtofit2();

}

static void Main(string[] args)

{

Program p = new Program();

p.startSW();

p.createNewPartDocument();

Console.WriteLine("Creating Shape");

double bWidth = 0.2;

double bHeight = 0.2;

double tWidth = 0.4;

double tHeight = 0.1;

double height = 1.0;

p.createShape(bWidth, bHeight, tWidth, tHeight, height);

p.setView((int)swStandardViews_e.swIsometricView);

}

解説

コードを詳しく見ていきましょう．

2．上面をスケッチするための参照面を作成する
createRefencePlaneは，基準となる面の名前originPlaneNameと距離distanceを指定して，参照面を作成するメソッドです．戻り値は，新しく作成した面の名前です．

string createReferencePlane(string originPlaneName, double distance)
{
    string refPlaneName = null;
    IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

    // Create Reference Plane
    bool isSelected = dExt.SelectByID2(originPlaneName, "PLANE", 0, 0, 0, false, 0, null, 0);
    if (isSelected) {
        IFeatureManager featureMgr = (IFeatureManager)modelDoc.FeatureManager;
        IRefPlane rPlane = (IRefPlane)featureMgr.InsertRefPlane((int)swRefPlaneReferenceConstraints_e.swRefPlaneReferenceConstraint_Distance, distance,
                                                                         0, 0, 0, 0);
                
        refPlaneName = getItemName("PLANE", 0, distance, 0);
    }

    return refPlaneName;
}

string createReferencePlane(string originPlaneName, double distance)

{

string refPlaneName = null;

IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

// Create Reference Plane

bool isSelected = dExt.SelectByID2(originPlaneName, "PLANE", 0, 0, 0, false, 0, null, 0);

if (isSelected) {

IFeatureManager featureMgr = (IFeatureManager)modelDoc.FeatureManager;

IRefPlane rPlane = (IRefPlane)featureMgr.InsertRefPlane((int)swRefPlaneReferenceConstraints_e.swRefPlaneReferenceConstraint_Distance, distance,

0, 0, 0, 0);

refPlaneName = getItemName("PLANE", 0, distance, 0);

}

return refPlaneName;

}

7行目：基準面を取得しています．

9行目：フィーチャマネージャを取得しています．

10行目：フィーチャマネージャのInsertRefPlaneメソッドを使って，参照面を作成しています．
第1引数で，条件として距離を設定しています．swRefPlaneReferenceConstraints_e.swRefPlaneReferenceConstraint_Distance
第2引数で，距離の値を指定しています．

13行目：参照面の名前を取得しています（平面１など）．

4．下面と上面をつなぐガイドカーブを作成する
sketchGuideCurveは，上下面の名前と断面寸法からガイドカーブを作成するメソッドです．戻り値は，新しくガイドカーブの名前です．

string sketchGuideCurve(string bottomSketchName, string topSketchName, double     bWidth, double bHeight, double tWidth, double tHeight, double height)
{
    string sketchName = null;
    IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

    bool isSelected = dExt.SelectByID2("Point1@" + bottomSketchName, "EXTSKETCHPOINT", 0, 0, 0, false, 1, null, 0);
    Debug.Assert(isSelected);
            
    isSelected = dExt.SelectByID2("Point1@" + topSketchName, "EXTSKETCHPOINT",  0, 0, 0, true, 1, null, 0);
    Debug.Assert(isSelected);
    
    modelDoc.Insert3DSplineCurve(false);

    double bottomW = bWidth / 2.0;
    double bottomH = bHeight / 2.0;
    double topW = tWidth / 2.0;
    double topH = tHeight / 2.0;
    sketchName = getItemName("EDGE", -(topW + bottomW) / 2.0, height / 2.0, -(topH + bottomH) / 2.0);

    return sketchName;
}

string sketchGuideCurve(string bottomSketchName, string topSketchName, double bWidth, double bHeight, double tWidth, double tHeight, double height)

{

string sketchName = null;

IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

bool isSelected = dExt.SelectByID2("Point1@" + bottomSketchName, "EXTSKETCHPOINT", 0, 0, 0, false, 1, null, 0);

Debug.Assert(isSelected);

isSelected = dExt.SelectByID2("Point1@" + topSketchName, "EXTSKETCHPOINT", 0, 0, 0, true, 1, null, 0);

Debug.Assert(isSelected);

modelDoc.Insert3DSplineCurve(false);

double bottomW = bWidth / 2.0;

double bottomH = bHeight / 2.0;

double topW = tWidth / 2.0;

double topH = tHeight / 2.0;

sketchName = getItemName("EDGE", -(topW + bottomW) / 2.0, height / 2.0, -(topH + bottomH) / 2.0);

return sketchName;

}

6行目：上面（topSketchName）の点（Point1）を選択リストに追加しています．SelectByID2の第1引数が名前，第2引数が種類です．第6引数がfalseであることにも注意してください．一度選択リストを空にしてから追加しています．

9行目：下面（bottomSketchName）の点（Point1）を選択リストに追加しています．SelectByID2の第6引数がtrueであることに注意してください．現状のリストに選択した対象を追加しています．

12行目：Insert3DSplineCurveでカーブを作成しています．引数がfalseなので，カーブは閉じていません．

5．ロフト機能で下面と上面をつなぐ
loftは，上下面とガイドカーブの名前を指定して，ロフトを実行するメソッドです．戻り値はありませんが，スケッチやカーブ同様名前を返すようにしておくと便利だと思います．

void loft(string bottomSketchName, string topSketchName, string guideCurveSketchName)
{
    IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

    bool isSelected = dExt.SelectByID2(bottomSketchName, "SKETCH", 0, 0, 0, false, 1, null, 0);
    Debug.Assert(isSelected);
            
    isSelected = dExt.SelectByID2(topSketchName, "SKETCH", 0, 0, 0, true, 1, null, 0);
    Debug.Assert(isSelected);
            
    isSelected = dExt.SelectByID2(guideCurveSketchName, "REFERENCECURVES", 0, 0, 0, true, 2, null, 0);
    Debug.Assert(isSelected);
            
    IFeatureManager featureMgr = (IFeatureManager)modelDoc.FeatureManager;
    featureMgr.InsertProtrusionBlend2(false, true, false, 1, 0, 0, 1, 1, true, true, false, 0, 0, 0, true, true, true,
                                       (int)swGuideCurveInfluence_e.swGuideCurveInfluenceNextGlobal);
}

void loft(string bottomSketchName, string topSketchName, string guideCurveSketchName)

{

IModelDocExtension dExt = (IModelDocExtension)modelDoc.Extension;

bool isSelected = dExt.SelectByID2(bottomSketchName, "SKETCH", 0, 0, 0, false, 1, null, 0);

Debug.Assert(isSelected);

isSelected = dExt.SelectByID2(topSketchName, "SKETCH", 0, 0, 0, true, 1, null, 0);

Debug.Assert(isSelected);

isSelected = dExt.SelectByID2(guideCurveSketchName, "REFERENCECURVES", 0, 0, 0, true, 2, null, 0);

Debug.Assert(isSelected);

IFeatureManager featureMgr = (IFeatureManager)modelDoc.FeatureManager;

featureMgr.InsertProtrusionBlend2(false, true, false, 1, 0, 0, 1, 1, true, true, false, 0, 0, 0, true, true, true,

(int)swGuideCurveInfluence_e.swGuideCurveInfluenceNextGlobal);

}

5，8，11行目：選択する対象の名前と種類を指定して，下面，上面，ガイドカーブを選択しています．SelectByID2の第6引数が上からtrue，false，falseとなっている点にも注意してください．

15行目：InsertProtrusionBlend2で，ロフトを実行しています．各引数の意味は，APIのヘルプに加えて，ロフトPropertyManagerを参考にすると理解しやすいと思います．