Using Multiple-Value Parameters to control CATIA dimensions

In this post, I will explain how to control a CATIA dimension using a multiple-value parameter. As an example, I will use a sheet metal part shown below, in which the raw sheet material can only come in standard thicknesses, for instance, 1mm, 1.2mm, 1.5mm, and 2mm.

First, we will create a user parameter with multiple values. In the Knowledge toolbar, select the Formula icon. In the New Parameter of type pull-down lists, select Length and Multiple Values, then click the New Parameter of type button.

In the Value list dialog box, enter the standard thickness values, and click OK to return to the Formulas dialog box.

Rename the created parameter from Length.1 to a meaningful name, such as Thickness. Do not close the Formulas dialog box yet.

Next, we will link the sheet metal thickness to the created parameter.

Select the Sheet Metal Parameter.1 object in the tree. This puts the parameter view filter on the selected object, so now the list in the Formulas dialog box only displays the parameters for the selected object. Highlight the `Sheet Metal Parameter.1\Thickness’ parameter in the list and click the Add Formula button.

While in the Formula Editor dialog box, click the Thickness parameter in the tree, so it populates the right-hand side in the formula. This formula now equates the sheet thickness to the user parameter Thickness. Click OK to close the Formula Editor dialog box, then close the Formulas dialog box.

Double-click the Thickness parameter in the tree. Note than only standard thickness values are available for selection in the pull-down list.

Test the result by selecting different thickness values in the list and updating the part.

The list of standard thicknesses can be updated later, if necessary. To do that, double-click the parameter in the tree, then right-click in the value field, and select Multiple Values > Update Values in the contextual menu.

In the Value list dialog box that opens, edit the list as desired. In the example below, we’ve added standard thickness 1.8mm in between the 1.5mm and 2mm values.

The use of parameters and formulas in CATIA is covered in the following Rand 3D classes:

CATIA Introduction to Modeling
CATIA Advanced Part Design
CATIA Knowledge Advisor and Expert

About the Author

Senior Technical Training Engineer<br><br>As a senior member of the Rand 3D team with a doctorate degree in Finite Element Analysis (FEA) and over 35 years of experience, Iouri provides design, consulting, and training services to those in the aerospace, automotive, electronics, and consumer goods industries. Iouri is a seasoned pro in 3D parametric design and prototyping using knowledge-based engineering methods, and has worked on a wide range of projects including BOM automation, CMM points generation, automated 3D annotation creation, and die tooling automation design. He is also a sought-after instructor and holds the designations of both CATIA Certified Professional (Expert level) and CATIA Certified Instructor.

Follow on Linkedin Visit Website More Content by Iouri Apanovitch