Create Trimmed Surface Feature Example (C#)
This example shows how to create a trimmed surface feature.
// ******************************************************************************
// Preconditions:
// 1. Specified part document template exists.
// 2. Run the macro.
//
// Postconditions:
// 1. Creates two intersecting surfaces.
// 2. Selects Surface-Extrude2 as the trim tool and sets the trimming options.
// 3. Trims Surface-Extrude1.
// ******************************************************************************
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System.Runtime.InteropServices;
using System;
namespace TrimSurfacesCSharp.csproj
{
public partial class SolidWorksMacro
{
public void Main()
{
ModelDoc2 swModel = default(ModelDoc2);
SketchManager swSketchMgr = default(SketchManager);
ModelDocExtension swModelDocExt = default(ModelDocExtension);
SketchSegment swSketchSegment = default(SketchSegment);
FeatureManager swFeatureMgr = default(FeatureManager);
SelectionMgr swSelMgr = default(SelectionMgr);
Feature swFeat = default(Feature);
bool status = false;
// Create new part document
swModel = (ModelDoc2)swApp.NewDocument("C:\\ProgramData\\SolidWorks\\SolidWorks 2013\\templates\\Part.prtdot", 0, 0, 0);
swSketchMgr = (SketchManager)swModel.SketchManager;
swModelDocExt = (ModelDocExtension)swModel.Extension;
swFeatureMgr = (FeatureManager)swModel.FeatureManager;
swSelMgr = (SelectionMgr)swModel.SelectionManager;
// Create two intersecting surfaces
status = swModelDocExt.SelectByID2("Right Plane", "Plane", 0, 0, 0, false, 0, null, 0);
swSketchMgr.InsertSketch(true);
swSketchSegment = (SketchSegment)swSketchMgr.CreateLine(-0.068922, 0.023964, 0.0, 0.042733, 0.005543, 0.0);
swModel.ClearSelection2(true);
status = swModelDocExt.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, false, 0, null, 0);
swFeatureMgr.FeatureExtruRefSurface2(true, false, false, 0, 0, 0.06604, 0.00254, false, false, false,
false, 0.0174532925199433, 0.0174532925199433, false, false, false, false, false, false, false,
false);
swSelMgr.EnableContourSelection = false;
status = swModelDocExt.SelectByID2("Front Plane", "PLANE", 0, 0, 0, false, 0, null, 0);
swSketchMgr.InsertSketch(true);
swSketchSegment = (SketchSegment)swSketchMgr.CreateLine(-0.041529, 0.023059, 0.0, -0.052625, -0.081662, 0.0);
swModel.ClearSelection2(true);
status = swModelDocExt.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, false, 0, null, 0);
swFeatureMgr.FeatureExtruRefSurface2(false, false, false, 0, 0, 0.0889, 0.06604, false, false, false,
false, 0.0174532925199433, 0.0174532925199433, false, false, false, false, false, false, false,
false);
swSelMgr.EnableContourSelection = false;
// Set the trimming options
status = swFeatureMgr.PreTrimSurface(false, true, false, false);
// Trim the surface
status = swModelDocExt.SelectByID2("", "SURFACEBODY", 0.0289416986472588, 0.00781827749557351, 0.0290635845400971, true, 0, null, 0);
swFeat = (Feature)swFeatureMgr.PostTrimSurface(true);
}
/// <summary>
/// The SldWorks swApp variable is pre-assigned for you.
/// </summary>
public SldWorks swApp;
}
}