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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:
       
    • Before creating a thin-walled swept-cut or swept-boss feature, you must:
       
    • 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.

 

 

 



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