Tutorial Overview
A. Disclaimer
This document is provided as a free resource, to encourage Catia V5 users in the neverending
quest for new and better skills. It has been provided at the time and expense of
the author, with no monetary compensation. The author has no desire to control the enduse
of the knowledge received from this document; however, use of any portion of this
document for commercial training purposes is strictly forbidden. This tutorial is to
remain forever in the realm of free knowledge transfer. Please report any misuse or
violation of this free usage policy.
B. Software Requirements
The intended audience of this tutorial, is Dassault Systemes customers using Catia V5,
Release 14 or higher, with a minimum recommended P2 configuration, MD2 license, or
better. The author is using Catia V5 R14 SP09, and HD2 license.
C. About Parameters and Formulas
These topics are beyond basic Part Design. It is assumed that the reader has mastered
basic skills of creating parts in Catia V5. Therefore, no extra attention will be given to
the details of steps leading up to the subject matter. This is necessary for clarity and
brevity.
Having said that, the purpose of creating Parameters and Formulas, is to allow the user a
means to quickly and meaningfully design and edit a part, based on user-defined logic.
But what does that mean? Simply put - you, the reader, have the ability to set up
relationships that make editing the part easier, not only for yourself, but downstream
users! By using a little forethought and ingenuity, the designer (and/or other end-user)
can build a part that can be edited on the fly, without ever re-visiting a design function.
This tutorial will explore how to set up parameters and formulas in a methodical way, and
to try to steer the reader away from common and painful mistakes en route to the end
product. In future tutorials, we will explore ways to integrate the knowledge gained here,
into further automation of the design process.
Lets begin.
TIP: The screen shots included in this tutorial may be too small to view when
printing. This document is best viewed on the screen, with a zoom ratio of 200%.

Assigning Parameters
Now that the parameters have been created, what do they do? Right now, they are not
associated to anything, and in effect, do nothing. In this section, we will explore how to
assign parameters to designed part features, and modify parts using the associated
parameters.
The first step is to figure out where the newly defined parameters need to go. Parameters
are assigned using the Formula function. (used in previous steps) If you remember back
to the system generated parameter list in the formula dialog, there were several parameter
names, with a corresponding path. This is the realm we will be working in. Each of
these paths points back to something that we created sometime between the initial file
creation, down to the last fillet. We will locate the features that we wish to assign
parameters to, and use our parameters to override the design input values.
The formula dialog is a bit intimidating at first. With some experience, it becomes
relatively easy to decipher; however, there is a much quicker, and easier way to find a
feature, than wading through the list.
Lets go through the parameter list, in order, starting with the part number. Initialize the
Formula function. When the dialog appears, go to the field called Filter Name. Here,
we can filter data by any criteria. In our case, we have a value Part1 in the tree, which
is where we want to assign the PartNumber parameter. (default value - yours may
vary) By doing a wildcard search, (*Part1*) we return the following parameters:

These are created in the same fashion, but we have a distinct advantage with features of
size. Open the Formula function again. We will look for the Box_Length feature that
we wish to assign our parameter to.
We know that the length is contained in Sketch.1, as this was the footprint of the box.
We created lines at the vertices of this sketch. To find this parameter, it is as simple as
selecting Sketch.1. In sketch one, our 2 constraints will appear. Select the one you wish
to become the Box_Length parameter-controlled length. Next, simply press the Add
Formula button, and select the Box_Length parameter in the tree, and press OK.

Repeat the same steps for the width of the box, and change the Box_Width parameter to
verify the successful association.
Now, we will assign the Box_Height parameter to the 4 lines that we created from the
sketch vertices. Remember, these 4 lines are projected into the sketches used to create
the walls, and have parametric history - so they will update based on the current length
value of the lines.
Open the Formula function. Begin by selecting (in the tree) the first line you created.
You will need to select following parameter: (Notice the Value column C select the one
with the length that you originally defined)
Once this value is selected, we will once again use the Add Formula option, this time
inserting the Box_Height parameter. Press OK, and repeat this step for all 4 lines.