CATIA V5 – Breakout View

The following example shows how to make Breakout View in a drawing of a simple set. Breakout View is usually a partial cross-section.


CATIA_V5_Breakout_view

In the drawing, it is needed to activate the view on which the breakout is added, and then click the Breakout view  ikona Breakout viewthat is within the Views group. Then you need to draw a profile that will determine the breakout. By closing the profile, 3D Viewer opens to show the level of cutting. The green arrow shows the direction of the view. The plane can be moved manually or in a second view, select the generated geometry (the system does not accept manual addition geometry). By default, the system sets a plane that matches the main coordinate system. If we want to cross through a hole, e.g. it is enough to click in the orthogonal view (relative to the original one) to the center line of that hole. Automatically move to the 3D Viewer.


3D Viewer

In addition to the two cross-sectionalizing options, it is also possible to select the element in the drawing field and enter the depth into the Depth field in the 3D Viewer in the Reference Viewer box. Once the cutting level is set, you need to click OK and View is automatically updated.


Breakout View kreiranje

Breakout View can be created on:

• Projection view

• Auxiliary view
• Section view
• Pogledu koji već sadrži breakout

Breakout View cannot be created on:

• Section cuts
• Detail / Clipping view
• Broken view

Once created, the Breakout View profile can not be modified. The Breakout View profile can not be applied to the same view.

Removing a breakout can be done in two ways:

•Right-click View, then View object and Remove breakout. If there are more breakouts, in this case everyone will be removed
•Right-clicking on any break of the resulting breakout, and then on the Generated Item object will be removed only that breakout

By right-clicking on the View / View object and then Apply Breakout to, the created breakout can be applied to any other view. You just need to click on the desired view. In the same way, it is possible to make a breakout in an isometric view.


catia_v5_breakout_in_an_isometric_view


By default, the breakout area is marked with a zigzag line, which is often not the best solution. Settings can be changed in Tools / Options / Mechanical Design / Drafting and then within the View tab you need to click on Configure with View line type.


catia_v5_linetype_and_thickness

The breakout propagation can also be set up automatically. It is required in Tools / Options / Mechanical Design / Drafting and within the Layout tab enable the Propagation of broken and breakout specification option. In that case every next view which is created from view with the breakout will have the same breakout. Breakout specifications cannot be propagated on Section cut.

The screws used to display the breakout are defined by the standard. They can also be modified by right-clicking on the hat and then within Properties.


Catia_v5_hatching