SolidWorks 2011 Parts Bible - Matt Lombard [180]
Figure 12.25 shows a portion of a feature tree of a part from which a feature in the middle of the tree was deleted. Unless you are very careful about how you set up your part, a deletion of this kind will result in a lot of errors.
Notice the tool tip balloon in Figure 12.25. Many users get in the habit of clicking out of any sort of warning or error message. You shouldn't be afraid of errors. Once you know how to deal with them, you will think of errors as a tool to help you investigate your model. The first thing you should do with an error message is read it. Eventually, you will be able to recognize error messages and their meanings very quickly.
FIGURE 12.25
Deleting a feature in the middle of a tree can cause a lot of errors.
This error message says, “The intended cut does not intersect the model. Please check the sketch and direction.” This means that you have a cut that is cutting air. This is because the feature it was cutting was deleted. You may know the cause of errors or you may not. If you had inherited this part from someone else who did not explain the state of the model to you, you might have to figure it out yourself. Most of the time, it is not difficult to figure out what is going on.
When you inherit a model with errors, the first thing you should do is look for the error that is highest in the tree. When you make a change that causes errors, these errors are almost always lower in the tree than the change. Special situations can arise where a change causes an error up the tree, but they are rare.
Here are some common error messages and what they are really trying to tell you:
• Some Items are no longer in the model. You can reselect the items using the Edit Definition in the FeatureManager design tree. The first thing to know here is that Edit Definition has been gone for several releases now. Edit Feature is the name of the command you will be looking for. You can get this message when an edge or a face for a selected feature no longer exists. A number of things can cause it, but the culprit is usually changes to the model upstream. As a result, if you roll back the model, and make changes (especially if you delete something, but adding features can also cause errors of this sort), you can expect some problems when you unroll the model.
• Operation failed due to geometric condition. This is one that frustrates a lot of users, because “geometric condition” is vague and could mean just about anything related to geometry. It can sometimes mean that a selection set is incomplete — the feature requires another face or another edge to be selected in order to work, or a fillet cannot work because an edge flips convexity, or a sketch line does not cut all the way across a solid body. There are too many possibilities to list, but it is a clue that you need to check either the selections for the feature or the body on which the feature is operating. In more complex cases, it might mean that the part has some geometrical errors that you need to figure out by using the Check tool or Verification on Rebuild.
• Warning: This sketch contains dimensions or relations to model geometry which no longer exists… This is one of the better messages that SolidWorks provides. It is fairly self-explanatory and goes on to give you a couple of useful suggestions as to how you might fix the problem.
• Some filleted items are no longer in the model. Edit the feature to reselect the items. When all of the edges selected in a fillet feature are suddenly not there, the entire fillet feature fails because there is nothing to do. This warning displays the red circle with the X in it. Some edges may remain selected, and the fillet feature can still work. In these cases, you will get the next message, which is just a warning rather than an error.
• Warning: Edge for fillet/chamfer does not exist. In this case, you see the yellow triangle warning, and the fillet still creates