SolidWorks 2011 Parts Bible - Matt Lombard [65]
• Up to Surface. Up to Surface could probably be better named Up to Face, because the end does not necessarily have to be an actual surface feature. This end condition may display a warning if the projection of the sketch onto the selected face extends beyond the boundary of the face. In that case, it is advisable to knit several faces together into a surface body and to use the Up to Body end condition.
• Offset from Surface. By default, Offset from Surface extrudes until it reaches a specified distance from a selected surface. There are two methods for determining the type of offset and one to determine direction.
• The default offset method behaves as if the selected surface were offset radially, so that a surface with a 4-inch radius and a 1-inch offset would give a curvature on the end of the extrude of a 3-inch radius.
• The second method, called Translate Surface, behaves as if the surface were moved by the offset distance.
• Reverse Offset refers to when the offset stops short of the selected face or when it goes past it.
• Up to Body. The Up to Body end condition is very useful in many situations, especially when receiving the error message, “The end face cannot terminate the extrusion,” from the Up to Surface end condition.
• Mid Plane. The Mid Plane end condition eliminates the Direction 2 options and divides the extrude distance equally in both directions; for example, if you specify a 1.00-inch Mid Plane, SolidWorks extrudes .50 inches in one direction and .50 inches in the other direction.
• Through All. The Through All end condition is available only when there is already solid geometry existing in the part. When used for an extruded boss (which adds material), it extrudes to the distance of the farthest point of the solid model in a direction perpendicular to the sketch plane. When used for a cut, it simply cuts through everything.
Offset from surface using the default and Translate Surface options
The Reverse Offset option
• Up to Next. Up to Next extrudes the feature until it runs into a solid face that completely intercepts the entire sketch profile. If a portion of the sketch hangs over the edge of the face, the extrude feature will keep going until it runs into a condition that matches that description, which may be the outer face of the part in the direction of the extrusion.
The Up to Next end condition used with a Cut extrude
By default, the Direction of Extrusion is normal to the sketch plane, but you can also select a linear entity such as an edge or axis as the direction. All the end-condition options are still available when you manually define the Direction of Extrusion as something other than the default.
You can also assign a draft option to an extrusion as it is created, and you can control the draft separately for Direction 1 and Direction 2.
Best Practice
When dealing with molded or cast parts, certain types of features, such as draft, fillets, and shells, are often the targets of users trying to assign best practices. This is partially because using draft, fillets, and shells is very much like playing Rock, Paper, Scissors; the only way to win this game is by luck. Arranging the features in the correct order so that the model is efficient and achieves the desired results is challenging. It is usually best to apply draft as a separate feature rather than using it in the definition of the Extrude feature. It is also best to apply draft after most of the modeling is done, but before you apply the cosmetic fillets and before you use the shell feature.
Using the Thin Feature Panel
The Thin Feature panel is activated by default when you try to extrude an open loop sketch (a sketch that does not fully enclose an area). The end-condition options remain the same. What changes is the feature applies a thickness to the sketch elements in the manner of a sheet metal part, thin-walled plastic part, or a rib. The Thin Feature panel of the Extrude PropertyManager,