SOLIDWORKS Sweeps FAQ

Article by GoEngineer on Dec 08, 2014

In this SOLIDWORKS FAQ, we answer ten questions about SOLIDWORKS sweeps. 

Question: How can I improve the quality in the Sweep Cut feature with a solid body as a tool? 

Answer: The result is influenced by geometries, continuity, and their complexity.

  • Create an Extrude solid as a Tool Body, it is better than a Revolved solid. 
  • If you use a Cylinder as a workpiece, it is preferred not to have the Tool body extend past the cut path of the part it is cutting, to avoid auto-intersection. 
  • If you use the “Wrap” command, it is better to trace a spline over arcs and lines; this will improve the internal continuity of projected curves. 
  • When possible, Insert – Curve – Split Line command permits to have a better internal continuity with a generic sketch. 
  • Duplicate a face on the target body (Offset Surface to 0.0 mm) and use it to project the sketch with Wrap or Split Line commands. 

Question: What are some of the functions of the Selection Manager? 

Answer: The Selection Manager has some of the following features (loft, sweep, surface boundary) and it can do the following functions:

  • Allows the selection of edge and sketch entities 
  • Allows the selection of entities from multiple sketches, in combination with model edges 
  • Replaces contour and smart selection 

Some of the options in the Selection Manager are the following: 

  • Select Close loop 
  • Select Open loop 
  • Select Region 
  • Select Group 
  • Standard Selection 

Question: Is it required to create individual sketches for each guide curve for sweeps or lofts? 

Answer: No, multiple guide curves can exist in a single sketch for a sweep or a loft command. 

Question: A swept-cut using a solid body does not follow the path. Why? 

Answer: To have a solid body follow a sketched path, please ensure that the path is continuous without any sharp corners. The path must be tangent within itself and begin at a point on or within the tool body profile. 

Question: How a solid sweep is created using a non-tangent path (right angles)? 

Answer: To create a solid sweep with a non-tangent path change the Options- >” Orientation/twist” section to either “Keep Normal Constant” or “Follow Path: All Faces 

Question: After creating a sweep section, sweep path, guide curves, and a pierce relation between the sketches, why does the sweep path fail with a "no pierce relation" error message? 

Answer: The maximum number of turns/twists that a sweep profile can make is 100. 

Question: What are the requirements for the tool body used in the solid sweep feature? 

Answer: The tool body must be convex, revolved, or extrude with the main body, not merged; otherwise the results will be unexpected with possible errors. 

Question: What is a possible reason for the option "align with end faces” not working in a sweep feature? 

Answer: If the sweep starts and ends at the same face (e.g. a u-shape), then "align with end faces” will not work.

  • A workaround is to split the start/end face into two faces. The sweep should then work as expected.

Question: How can surfaces left over by a sweep be made smooth?

Answer: Sweeps are non-analytic geometry, thus the sweeps have some leeway when they are created. 

  • This allows the sweep to be a great tool, but this same latitude can cause some sweeps to drift if they aren’t properly constrained. 
  • The problem can be corrected by using a path and guide curve as documented in the SOLIDWORKS Help guide.

Question: Can options in PropertyManagers be permanently set, for example, to always use a face fillet or certain loft tangency conditions? 

Answer: Unfortunately, these options cannot be permanently set, even by manual registry edits, as they are hardcoded.

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About GoEngineer

GoEngineer delivers software, technology and expertise that enable companies to unlock design innovation and deliver better products faster. With more than 35 years' experience and tens of thousands of customers in high tech, medical, machine design, energy and other industries, GoEngineer provides best-in-class design solutions from SOLIDWORKS CAD, Stratasys 3D printing, Creaform & Artec 3D scanning, CAMWorks, PLM, Altair, and more

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