SolidWorks 2011 Parts Bible - Matt Lombard [313]
Caution
The Rib feature is very sensitive to changes in the number of solid bodies in a part. If the number of bodies that exist at the point in the FeatureManager where the Rib feature exists changes either by increasing or by decreasing, the Rib will fail with the message, “Please select a body on which you want to create a rib feature.” You must edit the Rib feature to repair this condition.
Using Intersection Curves as reference
Ribs are features that typically go inside hollowed out parts. For that reason, they are often difficult to visualize, especially when they are on a plane that is deep down inside a part. You may find it useful to use some sort of a reference that shows where the current sketch plane intersects the wall of the part. For this I typically use Intersection Curves. This technique can be used in either Plan View or Skyline type ribs.
The Intersection Curve is on the Sketch toolbar. While in a 2D sketch, activate the tool and then select faces that intersect the current sketch plane. Deactivate the tool when you are done. You may want to select all the lines selected by the Intersection Curve tool and turn them into construction geometry. This provides a good reference for the rib sketch without interfering with the Rib feature.
Figure 24.7 shows an example of using an Intersection Curve as a reference for setting up a rib sketch. The construction lines at the ends and below the right end of the skyline rib sketch are Intersection Curves.
FIGURE 24.7
Using Intersection Curves as references
At the ends of the shell, the intersection curves serve to give the sketch a reference point to be fully defined. Under the right end of the rib sketch, the intersection curve gives you a reference to dimension the height of the rib in the shallower section of the part. The part shown in Figure 24.7 is on the DVD, with the filename Chapter 24 – skyline.sldprt.
Terminating ribs
The Rib feature automatically extends and trims ribs based on your rib sketch. This is a great ease-of-use function, but it tends to lead to sloppy sketching for Rib features. If you sketch a rib, and the sketch does not lead all the way to the wall of the part, SolidWorks extends it. If your sketch line goes past the wall, SolidWorks trims the rib so that it only goes up to the wall of the part. Figure 24.8 shows how the two straight ribs are extended from the existing sketches on a pair of plan view ribs.
FIGURE 24.8
Extending ribs
Sometimes you do not want a rib extended to the wall of the part. You may want to terminate a rib at a specific location in the middle of the part. The way to do this is to use a skyline rib and end the skyline sketch with a vertical (plus or minus draft) line that points to the base of the part. Figure 24.9 shows how to accomplish this. Notice that on the left end of the rib, it is extended straight down to the bottom of the part, and on the right side of the rib it is extended up to the next wall.
FIGURE 24.9
Terminating a skyline rib
A final termination situation I want to mention is one that can sometimes happen at curved edges. If the extension of the rib cannot be contained by the model, the rib will fail. This is not always as obvious a situation as you might think. When a non-horizontal rib intersects a curved edge, it usually forces you to fake something a little. Figure 24.10 shows an example of why this is.
FIGURE 24.10
The part wall does not terminate the rib.
The reason for the error shown in Figure 24.10 is that even though the rib sketch intersects the edge of the part, the width of the top of the rib would go past the edge