Pro/ENGINEER - Changing Features

In this mini-tutorial, we will look at various ways of changing features once they have been created. First, it is important to understand what constitutes a feature. The best way to understand a feature is to create them. Every piece of information you input becomes part of the feature specification. Roughly speaking, this specification can be divided into three parts:

• Specification of a sketch plane
• A 2-D section profile sketched and constrained on the sketch plane
• Specification of how the section expands (sweeps) off the plane to form a 3-D feature

There are important exceptions to these for some features. Some of the differences will be noted.

Modify

The simplest, and most common, way of changing a feature is to change the numeric values of constraining dimensions. This is done through the modify command on the part menu. The basic sequence of operations is:

• Choose modify | value
• Select one or more features, using options from the get select menu or choosing from the model tree window.
• Select the dimension to modify and enter a new value
• Regenerate to see results

You can also:

• Zoom, pan, rotate your view to get at dimensions
• Choose view | repaint to clear unneeded dimensions from the screen

Redefine

The redefine command on the feature menu is a very powerful command which lets you alter all of the specifications of a feature, including dimension values. It essentially lets you redo any of the steps you took in creating a feature. The basic sequence of operations is:

• Choose redefine
• Select a feature to redefine and then done on the select feature menu
• The feature dialog box comes up labeled with the type of feature selected (e.g., cut, protrusion):

• Select the element of the feature you want to redefine (the > pointer will move to where you pick) and then click on define (not OK)
• Go back through the sequence of menus, entries, etc. which defined that feature element
• When done, click on OK in the feature dialog

For cuts and protrusions, the feature elements contain the following information:

• Attributes - whether the feature sweeps from one or both sides of the sketch plane
• Section - change the sketching plane, redefine the section profile sketch, or just the dimensional constraint scheme
• Direction - (for Boolean subtraction operations) define whether the material inside or outside the section profile is removed
• Depth - the distance, either linear or angular, the section profile is swept

Holes have some other feature elements worth noting:

• Placement type - whether the hole is constrained with linear or radial dimensions
• Placement refs - the reference planes used to locate and constrain the hole

For rounds:

• Attributes - whether the round is of a constant radius or not

Another note, when redefining placement/reference planes, you will be sequenced through the planes:

• The placement plane will be highlighted in red and you will be given the menu options of using the same ref or choosing an alternate
• The reference planes will be highlighted in blue and you will be given the menu options of using the same ref or choosing an alternate

Reorder

The reorder command in the feature menu allows you to change the sequence in which the feature operations are performed on the part. You can see the current sequence of operations (from top to bottom) in the model tree dialog. The basic sequence is:

• Choose reorder
• Select a feature to redefine and then done on the select feature menu
• Choose whether you want to insert the feature before or after another feature. The allowable locations to insert the feature is listed on the command line. The numbers refer to the order (from top to bottom) in the model tree dialog.
• Click on the feature in the model tree dialog or in the modeling window to insert before/after

Reroute

The reroute command in the feature menu allows you to select a new sketch plane to place a section profile on. There are generally tight restrictions as to the new plane Pro/E will let you choose.

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