Pro Engineer/Regeneration Failures

< Pro Engineer

A regeneration failure is an error Pro/Engineer encounters in the generation of a model that forces it to halt until the problem is corrected by the user. Such failures are avoidable by careful, systematic use of the software but are unavoidable in dealing with designs handed down by less careful users.

Causes of Failures

Parent/Child Relationships

To determine whether a feature in the Model Tree is dependent on another feature, right click on it and select Info > Parent/Child. This will open a window describing what features this one depends on (its parents), and which features depend on it (its children).

When a feature of a part or assembly is a parent of other features, any changes to this parent are meant to be reflected in its children. This is enabled by careful consideration to Design Intent. For example, if a hole's diameter is intended to be the same as another hole, they should not be individually sized, but rather the child should be set equal in size to its parent so that any changes to the parent will result in robust reactionary behavior throughout the model and assembly.

The model tree, when managed carelessly, can become more of a web than a tree. Careless suppression of features is usually the root cause of regeneration failures.

Suppressing Features

To suppress a feature, select it in the viewing area or in the Model Tree and in the right-click context menu select Suppress.

Suppressing a feature is similar to hiding it from view but also causes Pro/Engineer to stop considering it in the part or assembly generation. Suppressing a feature makes the model behave as if the feature were deleted, whereas hiding makes a feature invisible. Because the feature behaves as if it were deleted, any unsuppressed children of the feature will suffer regeneration failures.

Suppression is useful in engineering applications when certain aspects of the model need to be ignored in computation. For example, in creating a mesh of a solid for finite element analysis, certain features of a model may be irrelevant to the results and may offer nothing to the model besides an increase in processing time. The solution is to create a copy of the model, and in this copy suppress the unnecessary features. This is called defeaturing. The defeatured copy of the model should then be carefully kept off limits for feature modification, because changes that happen to conflict with suppressed features are very easy to create and go unnoticed. While this careful use of the suppress function is fairly harmless, the following uses in a collaborative design environment are more dangerous:

Over-Referencing

References are necessary to create robust models that intelligently update themselves in all necessary places to reflect design intent when any single change is made. Overuse of references creates a web of dependency that later becomes difficult to untangle and not only increases the likelihood of failures occurring but exacerbates the problem of mitigating the failures that do occur.

Features are often defined by sketches. Extrusions and revolutions are common examples. Before sketching begins, Pro/Engineer asks for enough references to place the sketch on the model. Often, more references are necessary for robust design. However, to minimize future frustration, only as many features as absolutely necessary should be referenced, and only very basic features that are least likely to be removed should be referenced. Absolute datum references are very effective for this purpose.

When regeneration failures occur, and references need to be reassigned, the care taken in the choice of references will repay itself many times over in ease of mitigation.

Resolve Mode

When Pro/Engineer comes to a regeneration failure, it falls into Resolve Mode which utilizes an older interface consisting of menus that generally appear along the right side of the screen. In this mode, most functions of the program are disabled, including saving and quitting. The Undo feature is limited to one attempt and is not always successful. For these reasons, Resolve Mode can be difficult to maneuver out of, and is a source of frustration for many new users.

Failures often occur upon the Resume of a features that have been suppressed in the past, and have since been neglected and lost some of their parent references. One way to get out of this situation is to resuppress the feature: Quick Fix > Suppress > Confirm > Suppress All. This usually gets the model back to where it was before Resuming the feature. A more productive approach is to fix the reference problem by reassigning appropriate new references to whatever feature is missing them. Fix Model > Feature > Confirm > Redefine > Failed Feature gets this process started. Often this brings the user to the Edit Defintion of a feature defined by a sketch, and often it is the sketch that is missing references. In the toolbar: Placement > Edit > Sketch will open up the problem sketch. In the menu, Sketch > References will open up the References dialog and with any luck this will display the problems. These broken references sometimes need to be deleted and replaced, and sometimes need to be reassigned to reflect changes. This tool can not be closed normally until issue is not resolved. Extremely not user friendly and time consuming tool.

Resolve Options

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