SolidWorks 2011 Parts Bible - Matt Lombard [316]
Draft can fail for a number of reasons, including tangent faces, small sliver faces, complex adjacent faces that cannot be extended, or faces with geometry errors. When modeling, it is best to minimize the number of breaks between faces. This is especially true if the faces will be drafted later. Generally, the faces you apply draft to are either flat faces or faces with single direction curvature. You can't expect SolidWorks to draft anything you throw at it; you should try to give it good, clean geometry.
When draft does fail for a reason that doesn't seem obvious to you, you should use the Check utility under the Tools menu and also try a forced rebuild (Ctrl+Q) with Verification on Rebuild turned on. The Check utility checks the model for geometry errors. Verification on Rebuild checks more rigorously for features intersecting the model incorrectly. Some features may fail with the option on that would not fail with it off. When this happens, there is something wrong with that feature that the simplified default error checking did not catch.
DraftXpert
DraftXpert is a tool used to create multiple Neutral Plane draft features quickly. You can also use it to edit multiple drafted faces without regard for which features go to which faces.
Using Indent
Indent is a feature that uses a solid body as a tool, and indents a thin-walled area in the target part around the tool. For example, if you are building a plastic housing around a small electric motor, then the Indent feature shapes the housing and creates a gap between the housing and the motor. Figure 24.13 shows the PropertyManager interface for the Indent feature, as well as the geometry created by Indent.
In this case, the small motor is placed where it needs to be, but there is a wall in the way. Indent is used to create an indentation in the wall by using the same wall thickness and placing a gap of .010 inch around the motor. The motor is brought into the wall part using the Insert⇒Part command. This is a multi-body technique. (Multi-bodies are examined in detail in Chapter 19.)
The workflow for Indent is as follows:
1. Open or create a thin-walled part (this can be plastic, sheet metal, machined, and so on) in which you want to create an indentation.
2. Create a new body that will be the positive shape of the negative indentation. You can use Insert⇒Part to insert an external pre-existing part if you want.
3. Start the Indent command by choosing Insert⇒Features⇒Indent.
4. Select the thin-walled part that you want to put the indentation into (as Target Body).
5. Click an area on the tool body and change the Keep or Remove option as necessary. Use Keep when you selected a location on the tool body where you want to create a thin-walled area, or Remove if you want the selected area to be free of material.
6. Set the Thickness for the material thickness, and the Clearance for free space between the tool body and the new thin-walled material.
FIGURE 24.13
Using the Indent feature
Indent is particularly effective if you have a part that is nearly finished with a lot of detail on it that might be lost by rolling back and making drastic changes to the feature history.
The “cut” option is good for non-thin features where you want an offset cut-with-body. It is just like the Combine (subtract) tool, only with the ability to add an offset.
Working with Shell
The Shell feature is a powerful yet sometimes tricky feature to work with in SolidWorks. Many users just expect it to work regardless of the condition of the geometry, but it requires that some simple conditions be met. In general, to allow the Shell feature to work, you have to have a model where the minimum outside curvature (convex) is greater than the shell thickness. Shell works in 3D much like the offset sketch works in 2D. If the curvature is too