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containing several profiles.
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 15 of 37
4.2 Grouping elements in the various bodies of a CATPart.
The specification tree must be organised and the created elements must be grouped
logically to make location easy.
4.2.1 Using various types of bodies present in a CATPart
• Main part body: PartBody. A single main part body at output in a CATPart. Without
this recommendation, certain tools such as inertial calculation or automatic bill of
material will not operate.
Specific case of sketch: caution, a sketch used to create a Part Design or Sheet Metal
Design element must be created in the main part body and not in an open body.
Otherwise it will be duplicated and its management will be trickier.
Example:
Creation of Sketch.1 in Open_Body.1
Creation of Pad.1 by selecting Sketch.1: it is duplicated in PartBody and is therefore
present twice in the tree.
In Open_body.1, Sketch.1 is linked with no elements and its destruction is possible.
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 16 of 37
With the ‘Delete all children’ option: a window indicates the error.
Without this option, Pad.1 is destroyed.
In our example, the consequences are immediately visible as the part initially contains
only one Pad.1 extrusion. However, we can easily imagine that the disappearance of an
element bearing on a sketch will go unnoticed when the part is complex and the
specification tree includes around one hundred elements.
Conclusion: Duplication of Sketch.1 must be avoided. Remember to create the sketch
directly in the part body which will contain the element bearing on the sketch or move the
sketch before selecting it to create the element which bears on it.
• Secondary part body: Body. Secondary part bodies are used for the design of
complex parts requiring a Boolean operation between 2 solids (union, intersection,
addition, etc.). There may be therefore two separate solids in a CATPart, but
temporarily, before the Boolean operation. An exception is made for certain
installation restrictions:
Consult Chapter 2.10).
Example: a part body per pocket for machined parts.
Consult AP2257 Machined
Part modelling for CATIA V5.
• Open_body: The wireframe and surface elements are all placed by default in a
single body. It is recommended to create new Open_bodies to group data. In
particular, create a body including all the construction elements, from other parts,
which are not in the 'External references' body. Thus, in case of change of one of
the imported elements, location to replace it and do the update will be almost
instantaneous.
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 17 of 37
• External references: During work in context, for direct selection in a graphic
window of environment elements, these will be automatically duplicated in a specific
open body called External References. Elements can be imported into this body by
copy. However, any element created directly in this body cannot be displaced in
another body.
4.2.2 Ordering various bodies in specification tree
When design becomes hybrid (mixing of part bodies and open bodies to create entities),
the sequence of the various bodies in the specification tree must be ordered logically.
By default, the wireframe and surface geometry is created in an Open_body in parallel
with the PartBody. There will be no chronological trace of the design if the tree remains
as such.
Two possibilities to work on specification tree order:
• Before creation of elements: possibility of inserting new Open_bodies inside
PartBody (Menu Insert + Open_body).
• After creation of elements: possibility of displacing an Open_body inside a PartBody
(Drag&Drop) and possibility of displacing an element in the body (Reorder).
Remark: According to CATIA V5 versions, the elements created are not always placed
chronologically in the specification tree. In this case, use command ‘Reorder’ to displace
them or command ‘AutoSort Open body’ in the contextual menu.
Example:
• Creation of an extrusion in PartBody.
• Creation of a sweep surface in an Open_body.
By default, the sweep surface is
created in an Open_body placed in
the tree in parallel with the PartBody
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 18 of 37
• Method 1: The extrusion is cut with the sweep surface and a solid is created by
giving a thickness to this surface.
　
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