DDi Tech Center

There’s always more than one way to create a feature in SolidWorks. Starting in SolidWorks 2008 the ability to sweep a solid body along a tangent path was introduced. This new feature is ideal for modeling geometry created by machining operations.

Requirements:
1.A sketch to serve as a sweep path.
2.A multi-body solid with one of the two bodies created on a sketch plane which is related to the sweep path. In short, you need to model the cutting body so that it can move along the tool path.

There are three applications on this example model:
1.A corner rounding end mill which needs to cut along part of an edge which creates a complex fillet.A second Revolved Cut feature would be required to create this geometry without a Solid Sweep.

2.Modeling a vent with a bull nose end mill for an injection mold parting line. Irregular paths or cutter depths are easily modeled in fewer features.

3.Modeling a runner with a tapered ball end mill for an injection mold. This also eliminates having to calculate the runner path length to accommodate for the secondary Revolved Cut feature which would be required at the end of the runner without a Solid Sweep.

Here’s the general process:
1.Create the tool path sketch; be sure to add a lead-in gap so the bodies don’t get merged in Step 3.
2.Create a Reference Plane on one end of the tool path.
3.Sketch the profile of the cutter & revolve using a Revolve feature. Be sure to disable ‘Merge Bodies’.
a.Creating a gap between the tool and the work piece on the tool path sketch makes this irrelevant but it’s a ‘good practice’.
4.Create a Cut-Sweep feature
5.Select the Solid Sweep option and select the appropriate entities for each entry box.

Limitations:
As of this writing the current limitation with Solid Sweeps is the path must be tangent (i.e. no sharp edges). Sketching a R.0005” fillet is technically enough to get around the limitation. This limitation is documented as being eliminated in SolidWorks 2009.