There are times when a part has to be robust enough to handle several variations of design features and/or iterations. This would be the case when you build start parts or master models that give the designer a starting point for a complex design. A master model is critical if the parts you design always have the same basic features, but the details of those features vary. The most obvious case would be a plate that has variable length, width and height, as well as possibly having a few holes whose locations or sizes might 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 feature but 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 the use of these geometric parameters to solve this problem.
Note: In order to recreate this exercise your CATIA package will need to have the Knowledgeware Advisor (KWA) workbench. It will also be an assumption that you know how to easily create geometric sets, parameters, formulas and rules.
The example described is a simple flat head screw which will have different head types or tool slots. It exemplifies a Flat, Phillips, Hex, Star and a random swirl shape to show the extreme variations that can be created.
To start with, it is assumed you already have an existing part created, but do not have the ability to add much variation to that part without a considerable amount of design time or manipulation. The first thing you will need to add is a variable to trigger the change you want to create. In the example, a String parameter called “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 populate the curve parameter, but let’s not get too far ahead of ourselves!
The next parameter that needs to be created is a CURVE parameter. This parameter can be found near the end of the parameter list and is surrounded by the 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 of a specific unit. Typically, a parameter is not very useful until it has a value specified. In the case of a geometric parameter, the value or unit is a form of geometry; therefore a curve parameter’s value can be a sketch, spline, polyline or any other form of wireform geometry.
Now that the trigger and the placeholder have been created, the values of the curve parameter need to be created. These values will be sketches in the screw example, but can be anything that can be described as a curve. Five sketches were created and each named according to the profile being created – Straight, Cross, Hexagon, Star and Swirl. The naming is done to make it easier to identify the profiles and I would highly recommend naming them logically, but is not necessary as each sketch has its own proprietary name by default.
Once the values are created, the curve parameter needs to be populated with the values (Sketches) you created. You will need to switch to the Knowledgeware Advisor (KWA) workbench and create a rule. In the rule, 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
Else if variable == different value
This can be built upon with additional nested conditions, but for simplicity we will only use one condition and one result. In the example, the rule reads as follows:
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 “is equal to.” “<>” can also be used if you are determining whether something “is NOT equal.”
- “Flat” is one of the five multiple values of “PROFILE” that was 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 geometrical set that holds all the geometry, so the name is ProfilesShape.
- “Straight” is the name of the sketch that corresponds with the “Flat” screw head type. It is also in the “Profiles” geometrical set, so the name is ProfilesStraight.
Now that the curve parameter is populated, you will notice the icon changed to that of a formula and is ready to be used to build geometry. In the screw example, it was used as the sketch profile of a pad which was trimmed with a groove feature and those features were inserted into a separate part body, with that body being subtracted out of 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 many ways a valuated curve parameter can be utilized.
Using this method, your designs will be more robust as you will be able to create varying control points, different Sketch planes, splitting surfaces, sketch profiles, directional lines or axes or just about any type of control geometry to initiate complex design changes. Take the information here and build on it to reduce your design and manipulation time, increase productivity and make your designs more robust and powerful.