Creating a Simplified Representation

This task explains how you can create a simplified representation of a section.


Sections used in this application do not display any 'thickness'. Display of thicknesses is not necessary at this design stage and displaying sections in this manner improves performance. (However, thickness information can be stored with the section for use in downstream processes.) In order to use sections for use with this application you need to create a simplified representation, which is explained here.






1. Open the section for which you want a simplified representation in the Sketcher application. Make sure that the option Construction/Standard Element is not set - this is controlled through a button in the Sketch Tools toolbar.

Sections whose webs will be welded to the plate - L, T, FL and Bulb sections - need an additional step, explained here. Rename the left, center and right points of the web section as shown below. This allows the section to locate correctly when placed on a plate. Rename:
  • Left - catStrWebSideLeft
  • Center - catStrWebCenter
  • Right - catStrWebSideRight
  2. Using a Sketcher tool (for more information on using the tools see Sketcher documentation) draw two lines that represent the simplified version of the section. The lines can be drawn anywhere you want in the section, but note that the section will be placed according to the placement of your lines. In the image below the lines (displayed thicker than the rest of the section) have been drawn along the center, and bottom, of the section, which is usually appropriate for this type of section.

NOTE: If you are creating a new anchor point - meaning creating an anchor point on geometry that does not exist - then you must make sure that the option Construction Element is set. This option is referenced in Step 1.

  3. Select the lines you created and, in the Tools toolbar (often located at the bottom of the window), click the Profile Feature button . The Profile Definition dialog box displays.

  • In the Name field enter SimplifiedRepresentation.
  • Change the color of the lines. The color used in the sample sections is yellow.
  • Click the down arrow in the Mode field and select Wire (Explicit Definition).
  • Make sure that the Check Connexity checkbox is not selected.
  • Click OK.
  4. The simplified representation displays in the specifications tree. Save the CATPart.