Sweep  Features and SweepFeatureData Objects

To create a Sweep feature:

• See the ISweepFeatureData examples.

• Open a part in SOLIDWORKS and create a profile and a path along which to sweep the profile. Create guide curves, if using a sketch profile.

• In a macro:

  • Access the part.
     
  • Call IModelDocExtension::SelectByRay to select the:
     
    1. Profile:
        
       
       • If a sketch profile, use Mark = 1 to select a face, edge, or curve. For a swept-boss feature, the sketch profile must be closed. For a swept-surface feature, the sketch profile is open or closed.
         
       • If a circular profile, use Mark = 4 to select a sketch line, edge or curve. The circular profile is open or closed.
         
       • If a solid profile, use Mark = 1 to select the tool body to use to make the cut and use Mark = 2048 to select the solid body to cut. Solid profiles are used only in swept-cut features.
         
        
    2. Sweep path using Mark = 4:
        
       
       • Select a set of sketched curves contained in one sketch, a curve, or a set of model edges.
         
       • The sweep path is open or closed.
         
       • The starting point of the sweep path must lie on the plane of the profile for a 1-directional sweep. If the sweep path extends to both sides of the profile, you can create a bidirectional sweep.
         
       • Sweep paths are not used with circular profiles.
         
        
    3. Guide curves using Mark = 2:
        
       
       • Guide curves are used only with sketch profiles.
         
       • A guide curve must be coincident with the sketch profile or with a point on the profile sketch.
         
       • Guide curves are not used in bidirectional sweeps.
         
        
    4. Direction vector using Mark = 128:
        
       • Select a plane, face, line, axis, edge, cylinder, or a pair of vertices that define the direction.
          
  • To create a SweepFeatureData object and initialize it with default properties for a:
  
   
  • Swept-boss feature, call IFeatureManager::CreateDefinition(swFmSweep).
  • Swept-cut feature, call IFeatureManager::CreateDefinition(swFmSweepCut).
  • Swept-surface feature, call IFeatureManager::CreateDefinition(swFmRefSurface).
     
  • If you specified a direction vector in step 3.2.4 above, then before creating the sweep feature you must:
     
    • Set ISweepFeatureData::PathAlignmentType to swTangencyType_e.swTangencyDirectionVector.
    • Set ISweepFeatureData::TwistControlType to swTwistControlType_e.swTwistControlFollowPath.
       
  • Before creating a thin-walled swept-cut or swept-boss feature, you must:
     
    • Set ISweepFeatureData::ThinFeature to true.
    • Set ISweepFeatureData::ThinWallType.
    • Call ISweepFeatureData::SetWallThickness.
       
  • Modify other ISweepFeatureData properties that apply to the selected profile. For example for a sketch profile, if the sweep path extends to both sides of the profile, you can make the sweep bidirectional by setting ISweepFeatureData::Direction. See the SOLIDWORKS help and ISweepFeatureData for more information about sweep feature properties.
     
  • Create the sweep feature by calling IFeatureManager::CreateFeature(SweepFeatureData object).

To edit the sweep feature:

1. Call IFeature::GetDefinition to access the SweepFeatureData object.
2. Call ISweepFeatureData::AccessSelections.
3. Modify ISweepFeatureData object properties. Note that you cannot create a thin-walled sweep feature at this point.
4. Call IFeature::ModifyDefinition, if you modified the feature, or ISweepFeatureData::ReleaseSelectionAccess, if you did not modify the feature.