CATIA V5 – Overload Properties

The Overload Properties feature is very useful when creating a set drawing. Sometimes there is a need for not all parts to appear within a particular view of the drawing (for clarity of view), which can easily be achieved using the Overload Properties feature. It is possible to display certain sections in section (screws, nuts) without hatching, with or without visible edges. In addition, it is possible to set graphics attributes for individual components (color, type, and line thickness). The following example shows the use of the Overload Properties functions in a simple assembly drawing. Only one view was created here (Top view) and a cross-section A-A is made as shown in the picture below. As you can see, the system automatically adds a hinge to all parts of the cross-section.


catia_v5_overload_properties_functions

To run Overload Properties, you need to right-click on View, View Object, and Overload Properties.



catia_v5_starting_overload_properties

A new window opens where it is necessary to mark the sections for which Overload Properties is set. Parts are then visible in the window, in order to edit some part, it should be selected and clicked on Edit. It is also possible to edit multiple parts at a time (using the CTRL key is a multi-select) if it has the same attributes.


catia_v5edit_multiple_parts

Clicking Edit opens a new window where it is possible to turn off Cut in section views (useful for screws and nuts), which is default enabled. You can also turn off Use when projecting, which means that the selected parts will not be displayed in this view. Represented with hidden lines shows invisible edges.


catia_v5_cut_in_section_views

After the Cut in section views is turned off and clicking OK View is updated and the marked screws and nuts are not screwed on.

In addition, it is possible to change the color, type, and line thickness for individual parts (it can be useful when creating screenshots for presentations).


Catia_v5_overload_properties _changing_colorCatia_v5_overload_properties _changing_color2

Drafting Properties for some part can also be set in 3D-clicking on Part, then to Properties, and then in the Drafting tab.


catia_v5_drafting_properties

Drafting Properties can be activated in two ways:

  • Tools / Options / Mechanical Design / Drafting → On the View tab, turn on Apply 3D specifications
  • Right click on View, then on the Properties to turn on the 3D spec option