There are times when a part has to be robust enough to handle multiple variations of design features and / or iterations. This would be the case when you build starter pieces or master models that give the designer a starting point for a complex design. A master cast is critical if the parts you design always have the same basic characteristics, but the details of those characteristics vary. The most obvious case would be a plate that has variable length, width and height, plus possibly has some holes whose locations or sizes could change where each of the values ​​can be driven by global parameters. What happens when you need to change the geometry of a body or function, but you don’t want to have repetitive design features or you want to avoid a complex tree structure? You use a geometric parameter, of course! This article will walk you through using these geometric parameters to solve this problem.

Note: To recreate this exercise, your CATIA package must have the Knowledgeware Advisor (KWA) workbench. It will also assume that you know how to easily create geometric sets, parameters, formulas, and rules.

The example described is a simple flat head screw that will have different types of heads or tool slots. It exemplifies a flat, Phillips, hexagonal, star shape, and a random swirl to show the extreme variations that can be created.

To begin with, it is assumed that you have already created an existing part, but you do not have the ability to add much variation to that part without a considerable amount of design or manipulation time. The first thing you’ll need to add is a variable to trigger the change you want to create. In the example, a string parameter named “PROFILE” was created with multiple values ​​(Flat, Phillips, Hex, Torx, and Swirl-E-Bob). The different values ​​of this parameter will determine which sketch is used to complete the curve parameter, but let’s not get too far ahead!

The next parameter to create is a CURVE parameter. This parameter can be found near the end of the parameter list and is surrounded by other geometric parameters, including Surface, Plane, Circle, Line, and Point. A geometric parameter is like any other parameter and can be thought of as an empty placeholder for a specific unit. Typically, a parameter is not very useful until it has a specified value. In the case of a geometric parameter, the value or unit is a form of geometry; therefore, the value of a curve parameter can be a sketch, spline, polyline, or any other form of wireframe geometry.

Now that the trigger and placeholder have been created, you need to create the curve parameter values. These values ​​will be sketches in the bolt example, but can be anything that can be described as a curve. Five sketches were created and each was named according to the profile being created: straight, cross, hexagonal, star, and spiral. The name is made to facilitate the identification of the profiles and I highly recommend naming them logically, but it is not necessary as each sketch has its own default property name.

After the values ​​are created, the curve parameter must be populated with the values ​​(sketches) that you created. You will need to switch to the Knowledgeware Advisor (KWA) workbench and create a rule. In the ruler, you will need to create a conditional statement that will drive the curve parameter. The syntax of a conditional statement in KWA is as follows:

If variable == value

{action}

Otherwise if variable == different value

{other action}

This can be built with additional nested conditions, but for simplicity we will only use one condition and one result. In the example, the rule says the following:

IF PROFILE == “Flat”

{

ProfilesShape = ProfilesStraight

}

ELSE IF PROFILE == “Phillips”

{

ProfilesShape = ProfilesCross

}

ELSE IF PROFILE == “Hex”

{

ProfilesShape = ProfilesHexagon

}

ELSE IF PROFILE == “Torx”

{

ProfilesShape = ProfilesStar

}

ELSE IF PROFILE == “Swirl-E-Bob”

{

ProfilesShape = ProfilesSwirl

}

To break this down, we will look at each line of the first condition.

• “PROFILE” is the name of the string parameter that was created for the trigger.
• “==” means “equals”. “<>” can also be used if you are determining if something is “NOT equal”.
• “Plane” is one of five multiple “PROFILE” values ​​that were assigned to determine which sketch would be used to evaluate the curve parameter. Shape “is the name of the curve parameter and” Profiles “is the name of the geometric set that contains all the geometry, so the name is ProfilesShape.
• “Straight” is the sketch name that corresponds to the “Flat” screw head type. It is also found in the “Profiles” geometric set, so the name is ProfilesStraight.

Now that the curve parameter has been completed, you will notice that the icon has changed to that of a formula and is ready to use to build geometry. In the screw example, it was used as the sketch profile of a pad that was cut out with a slot feature and those features were inserted into a separate part body, and that body was subtracted from the main screw part body. Sounds complicated, right? You can simply use your curve parameter as the profile of a pad, pocket, or any number of part or surface features you need to create. This is just one of the many ways that a valued curve parameter can be used.

With this method, your designs will be more robust as you can create different control points, different sketch planes, split surfaces, sketch profiles, directional lines or axes, or almost any type of control geometry to initiate complex design changes. Take the information here and build on it to reduce your design and handling time, increase productivity, and make your designs more robust and powerful.