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• Method 2: To obtain a more logical tree, insert the Open_body in the PartBody
before creating Split.1 and ThickSurface.1.
The 2 elements Split.1 and ThickSurface.1 which use
Sweep.1 are created in the PartBody. The specification tree is
no longer logical in relation to the design. The chronology of
the various steps is not conserved.
Open_body.2 is now in PartBody.
2 solutions:
• Menu: Insert + Body before creation
• Drag&Drop after creation
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 19 of 37
• Even with this method, CATIA will create Part Design elements in the tree before the
Open_body.
• In order to reestablish chronology, the elements can be reordered.
Split.1 and ThickSurface.1 which use Sweep.1 are created
before Open_body.2
Select Open_body.2 + contextual menu + AutoSort Open_body.
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 20 of 37
• Interest of second working method: on a modification of the sketch of the sweep
surface, for example, only the operations done before creation of Open_body are
visible.
Method 1 (Open_body in parallel): During
edition of Sketch.3 of Sweep.1, all tree
elements are visible in the graphic window.
Method 2 (Open_body in PartBody): On edition of
Sketch.3 of Sweep.2, only the elements created
before Open_body.2 are visible in the graphic
window.
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 21 of 37
4.2.3 Preparing Boolean operations
The PartBody cannot be used (CATIA limitation) as tool for the Boolean operations (Add,
Remove, etc.). Therefore, the tool must always be created in a secondary body.
Contextual menu
for PartBody
Contextual menu for a
secondary body
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 22 of 37
4.3 Explicitly renaming elements
Location in an element tree will be easy if grouping is organised. It will be easier still if
the elements have a clear and explicit designation.
Examples:
Remark: all entities created in the specification tree will appear by default in the form:
When naming elements, it is useful to conserve the type and rename only the number
part in order to conserve the method for obtaining the element (trim, extract, translate,
join, split, etc.).
Examples:
Designation not explicit
Icon type.number
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 23 of 37
5 Optimised modelling for updates
CATIA V5 modeller can be particularly efficient for modification management. In the
previous chapter, we have seen how to structure the data. Here we want the user to be
aware of the internal mechanism for updates in order to integrate a strong
recommendation when modelling:
As far as it is possible, try to create features based on selection of other
features and not on selection of sub-elements geometrical representations.
In other words, when you create an element, try to select a point rather than
a vertex, a line rather than an edge, a plane rather than a face.
The reason is that CATIA V5 is not often able to update elements bearing on edges,
vertex and faces when geometry is rebuilt during the modification.
When the modification is only a modification of some parameters and does not generate
creation of some new geometry, the update can run till the end. However, when you
replace geometry by another one (for example a surface by another one), all the
geometry based upon the surface is not modified but re-built. Then the specifications
stored to create geometry must be stable. That is not the case of vertex, edges and
faces.
Example 1: Update interrupted because of the definition of a plane
In this example the external surface is replaced
by a new one. All the wireframe elements of the
design principle have to be updated
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 24 of 37
When the replace of Surface.1 by Surface.15 is performed, a window appears when
some edges, vertices or faces cannot be replaced.
In our example, update is interrupted on the Plane.1 definition. A window appears to
indicate the diagnosis of the problem (a face, an edge, or a vertex is no longer
recognised). Press the ‘Edit’ button to modify the Plane.1 definition.
If you press OK at this step, update will stop for
all elements created upon edges, vertices or
faces with no selection.
AIRBUS AP2255
　
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