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Consult AP2259 Sheet Metal Part modelling for CATIA V5
3.3 Panels
TBD.
3.4 Profiled parts

Consult AP2258 Profiled part modelling for CATIA V5
3.5 Piping

Consult AM2253 Tubing installation modelling for definition phase CATIA V5
3.6 Electricity

Consult AM2254 Electrical installation modelling for definition phase CATIA V5
3.7 Composite
TBD
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 11 of 37
4 Structuring of data in a CATPart
The CATIA V5 modeller was defined in part with the aim of facilitating modifications and
rapidly dealing with changes. In order to get the best out of the possibilities offered, it is
important to take some time to think during the design phase of the structure the data of
a CATPart. Also, a CATPart with an optimised data structure (specification tree) will be
more understandable for a person who has never worked on the latter.
The aim of the following recommendations is to improve the understanding of the design
of a part.
4.1 Design by modelling independent entities
• Foreword
Generally speaking, the more the created objects are independent from each other the
easier they will be to modify individually. This remark also applies with links of external
references type. By modelling parts which abusively use links, designers may rapidly find
themselves in a situation where modification management is inextricable. This is why it is
strongly recommended to limit the use of such mechanisms:
consult AP2XXX
Assembly rules, Work in context chapter.
• Example 1: Creating fillets and chamfers
For the type of part below, it is possible, on creation of a fillet, to apply a radius value to
several edges at same time.
This method which may a priori seem attractive for creation is penalising when the value
of the radius of a single edge is to be modified.
1st case: a single EdgeFillet entity with n selected edges.
To modify the radius of an edge, you must:
• edit the EdgeFillet object,
• deselect the edge which no longer has the same radius value (Ctrl key + edge
selection),
• validate the old EdgeFillet,
• create a new EdgeFillet with the edge which no longer has same radius.
All the radii are grouped in a single fillet
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 12 of 37
Also, if the new radius value gives an unresolved topology for a single edge, this
will be difficult to identify and therefore all selections must be reconsidered.
2nd case: n EdgeFillet entities with one edge in each object.
To modify the radius, simply edit the EdgeFillet object which bears on the edge in
question and validate the new radius value.
Conclusion: only group together edges which mandatory will have same radius value.
Remark: same reasoning applies to chamfers
• Example 2: Creating radii controlled by a formula in a sketch
With multi-selection of the elements of a sketch, it is possible to create all radii in one
operation with command 'Corner'.
During creation, this functionality may seem to be very practical. But, if the value of a
single radius is to be modified, the fact that it is related to a master radius is immediately
a handicap and a hindrance. To modify the master radius and not the others, all
formulas must be destroyed.
Conclusion: use formulas only for real master elements and not for creation comfort
reasons.
A radius controls all the others with a formula
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 13 of 37
• Example 3: Creating several contours in a sketch for a single pocket
Let us suppose that the height of a single pocket is to be modified: the pocket must be
removed to create two new pockets to be able to have two different heights for the
pockets.
4 contours in a single
sketch and a single pocket
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 14 of 37
Conclusion: to manage modifications correctly, initially create 4 pockets bearing on 4
contours. The 4 contours can be either in 4 different sketches or in the same sketch. For
dimensioning contours, it can be suitable to group them in the same sketch. However it
is possible to access a single contour inside the sketch when creating pockets.
Each pocket height will be managed
in each of the Pocket.x features
When selecting the profile, use the
contextual menu to choose “Go to profile
definition” : this command allows a
selection of one profile inside a sketch
　
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