Tips for Improving V5 Knowledge-Based Designs

By Joe Konecny, MSC.Software Corporation

It all starts with the geometry…

Anyone who has worked with Knowledge Advisor rules has most likely seen an update error pop up when a rule-driven parametric part morphs from one configuration to another. There are many reasons for update errors, but most of them can be linked back to how the geometry was originally created.

These types of errors can be minimized if some simple design rules are followed up-front during the creation of the part. One of the main causes of update errors is that BREP elements (like faces, edges, or vertices) were used during the design of the part instead of "real" geometry (such as planes, lines, and points). Take the following example of a lifter gib from the Mold Industry:

In this example, the parameter Gib Angle (Figure 1) varies from design to design causing the blue faces to move. The indicated holes (Figure 1) are to remain normal to the blue surfaces as the angle is modified. This model can be easily constructed using the blue faces of the part as the hole direction when creating the holes. However, as the angle goes to zero, the blue faces will disappear as they are joined with the bottom surface of the part. This leads to the following update error:

As one can see by the error message, the problem is that the blue faces no longer exist in this configuration. When the Gib Angle goes to zero, there is only one face on the bottom of the part. Because the holes were referenced to the blue faces, CATIA cannot update them when the Gib Angle equals zero because one of their parent elements no longer exists.

To remedy this situation, we must add the extra step of creating a plane that is driven by our Gib Angle parameter and which can be used as the hole direction reference:

This plane exists whether Gib Angle is zero or some other value. So, by choosing this "real" geometry (i.e. the plane) instead of the BREP geometry (i.e. the face), the angle can vary to zero without the previous update error:

This is one example of a good design methodology when working with Knowledge Advisor and parametric parts: Whenever possible, use real geometry instead of BREP geometry when creating parametric parts. This small amount of extra work up-front can save hours of debugging a knowledge based part later on.

How can I tell BREP geometry from "real" geometry?

This then leads to the question: How do I know when I'm selecting a BREP as opposed to "real" geometry? There are a couple of very simple ways to determine what is being selected. The first method is to try and select the elements from the tree rather than from the graphical area of the screen. By selecting elements from the tree, it is impossible to get a BREP (Figure 4). The second is to look at the message at the bottom left of the CATIA window before making a selection (Figure 4). If the message says "Face/...", "Edge/…", or "Vertex/…" then you are about to select a BREP.

By knowing what type of geometry you are selecting when you create a part it is much easier to make sure that you are using "real" geometry as opposed to BREP.

These are just two of several tips that can be used to make your knowledge based designs more robust. To learn about more tips and methodologies to improve your V5 knowledge based designs, visit http://www.mscsoftware.com/ads/?COENews040504.

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