SolidWorks 2011 Parts Bible - Matt Lombard [47]
• Sometimes a 2D fillet simply cannot create the required 3D geometry.
Fillet features are the preferred method for creating rounds and fillets. The same can be said for chamfers. Still, sometimes you need to use tangent arcs in sketches. You will have to decide which way works best for you.
The Centerline tool follows the same methods as regular lines and is called a construction line in some cases. Other construction entities, such as construction circles, are not available directly, but you can create them by selecting the For Construction option in the PropertyManager for any entity.
The Spline tool draws a freeform curve. Splines may form either a single closed loop or an open loop. In either case, the spline is not allowed to cross itself. You can draw a spline by clicking each location where you want to add a control point. Figure 3.10 identifies the elements of a spline. The detail image shows the structure of a spline handle.
FIGURE 3.10
The structure of a spline and spline handles
Splines are used mainly for freeform complex shapes in 2D and 3D sketches, although you can also use them for anything in which you would use other sketch elements. If you need more information on splines and complex shape modeling, refer to the SolidWorks Surfacing and Complex Shape Modeling Bible (Wiley, 2008).
The Point tool creates a sketch point. Aside from limited cases of lofting to a point or using a point as a constraint sketch in a Fill feature, sketch points are usually used for reference or for the location of the centerpoint of Hole Wizard features.
You can also use the sketch point as a virtual sharp. If two sketch entities do not actually intersect because of a fillet or chamfer, selecting the two entities and clicking the Point tool creates a point at the location where they would intersect if they were extended. This is useful for dimensioning to the sharp. Virtual sharp display is controlled by a Document Property setting.
The 3D Sketch Plane tool creates a plane in a 3D Sketch. I discuss 3D Sketches in more detail in Chapter 6. By sketching on planes within a 3D sketch, you get most of the benefits and usage of 2D sketches, and you do not have to deal with history between sketches. Before committing too much work to this course, you should look into some of the shortcomings of 3D Planes. The planes are treated just like any other entity in the 3D sketch, which means you can assign sketch relations to them, but it also means that they can move around within the sketch like sketch entities.
The Add Relation tool displays a PropertyManager window that enables you to apply sketch relations. This interface appears to be obsolete because it is easier to simply select sketch items and apply relations via the context toolbar or in the PropertyManager window that appears automatically when you select them; however, there are some subtle workflow-related reasons for using this tool.
Two advantages exist to using the Add Relations dialog box over simply selecting sketch entities and adding relations. When the Add Relation PropertyManager is active, you do not need to use the Ctrl key to select multiple entities. You also do not need to clear a selection before making a new selection for the next relation. These two reasons sound minor, but if you have a large number of sketch relations to apply, the workflow goes much more smoothly using this tool than the default method.
The Display/Delete Relations tool enables you to look through the relations in a sketch and sort them according to several categories. From this window, you can delete or suppress relations and replace entities in relations.
The Quick Snaps flyout tool enables you to quickly filter types of entities that sketch elements will snap to when you move or create them. To access the tools, click the drop-down arrow to the right of the toolbar button.
The Mirror Entities tool mirrors selected sketch entities about a single selected centerline and applies