Imagine that you’re working at a company which designs car interiors. You are responsible for designing the cupholders for next years model and the sales department have identified two customer segments where they want to be able to offer unique solutions tailored for these customers. One segment is the Swedish market where the customers want large cupholders which can fit a cup big enough to wake up the tired Swede on his way to work. The second customer segment is the Italian market where the customers want small cupholders for espresso cups.
When solving this problem, it would be neat if the cup would drive the design of the cup holder, so that depending on what cup you put in your CATIA model you would get at unique design of your cup holder. We can achieve this by using the Publish function in CATIA.
With the help of Publish, we can create a named reference for use in other parts for creating linked geometry. Without Publish the link to an external reference would look like in the picture below.
In this case we are referencing to a length in a sketch in a body in a part, this way helps us somewhat with understanding the model but can cause problem if we want to make changes. If you would replace Cup1 with Cup2, then the reference would point to `Cup2\PartBody\Sketch.3\Length.4`. In Cup2 the reference Length.3 in Sketch.3 could be something entirely different since the numbering depends on in which order the dimensions were created. It is implausible that a designer would remember to create the dimensions in the same order in two different parts and impossible for several designers to create them in the same order. If we instead publish the information that we want to have in common between parts, we get a more stable and functional model.
In the example of the cup holder I have chosen to have the bottom diameter of the different cups as the driver for size of the cup holder. After designing my cup, I want to publish the bottom diameter as my reference CupSize. This is done by opening Tools>Publication… and then choosing Parameter.
By choosing the feature in the specification tree which defines the bottom diameter, the dimensions appear on the screen and I can select the bottom diameter directly on the model.
We are then returned to the publication window and we can see that the bottom diameter is now in the list. It is now important to name the reference, it is this name that CATIA will search for when we want to reference the bottom diameter.
The publication is repeated for both cups and the reference gets THE SAME NAME in both cups, this is because our cupholder will be searching for the reference CupSize regardless of which cu we use.
Now it is time to set up the link between the cups and the cup holder, we create an assembly which contains the cupholder and one cup. When we want to change cup, and therefore the design of the cup holder, we will use the Replace command on the cup.
We now open the feature which defines the size of the bottom of the cup holder, in this case a sketch with a circle in it. On the dimension which defines the size of the circle we go in to Edit Formula… and choose CupSize in the specification tree. I have also added 2 mm to create some clearance between the cup and the walls.
Now the cup holder is linked to the published reference CupSize, this means that when we replace the cup, the size of the cup holder will change. If we use the Replace command to swap Cup1 for Cup2 a new window pops up, it tells us that not only will we impact the assembly constraints but also a design reference, the Contextual Design reference in the picture below.
Now we can control the design of the cup holder by simply changing which cup we want to use it with. By using Publish we have also made sure that we have a functional design reference. We could import any cup, save the bottom diameter with the Measure Item tool and publish the measure under the name CupSize and it would work straight away in creating a new design for the cup holder.
Technical Training Specialist
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