AP2257 - Draft A1 - Machined Part Modelling for CATIA V5

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AIRBUS Machined Part Modelling for CATIA V5 AP2257 2 General recommendations 2.1 Applicable rules - Modelling is done in CATIAV5 exact solid form (PartDesign Workshop). The resulting model is a CATPart. Reminders: The intermediary geometry is created by means of sketches and elements obtained from the WireFrame & Surface Design workshop. The main contours bear on defined functional references such as the 3 main planes of the part (XY, ZX & YZ planes). - For parts taken from blanks, modelling must include the draft angles for the sections of the part not machined (by rework of supplier's contractual drawing). - The bores are modelled. - The threads and tapings are modelled by standard "holes" features: • to nominal diameter value for a thread, • to drilling diameter value for a tapping. - Definition of spot facings: Use the "hole" "counterbored" feature - Positioning reference system The part is modelled in its absolute axis system inside the CATPart modelled by the 3 main planes (XY, ZX, YZ). - The curves and surfaces from the SRG (Shape reference group) are defined in the CAD model. These elements have a property giving the reference of the basic GRF file. Before any construction work, the validity of the curve or the surface from the SRG must be checked. If the size of the surface is insufficient, a new reference must be requested from the SRG. - Abundantly use names and explicit comments during CATIA entity creation (right click on preselected entity + properties + feature properties). - For the definition of a feature, perform the Boolean operations at latest possible stage in the history in order to be able to change more easily, during a modification, the topology of the latter. On completion of construction, there must be only one PartBody. Integration of restrictions is not dealt with here. - The construction elements will be located, if possible, on the drawing reference planes. Whenever possible, they must belong to sketches positioned on these planes. These elements will be constructed as and when the designer needs them. - Pockets will be modelled by the "pockets" features even for non-canonical shapes and this with the aim of optimising recognition of native features proposed by CATIA V5 in the machining workshop. - In a "Multi-body" approach, always prefer modelling of 2 bodies for a pocket; one body containing the definition of the pocket without fillets "assembled" with a body containing the fillet radii. This with the aim of more easily integrating the pocket bottom restrictions. Issue:Draft A1 Date: 13 February 2002 Page 4 of 46
AIRBUS Machined Part Modelling for CATIA V5 AP2257 - Parameterising will be done by constraints on a sketch. Caution: all elements used in the current sketch must be defined in this current sketch or on a coplanar sketch plane. They must not be taken from surface elements external to the latter. - Do not create auxiliary co-ordinate systems (Reference axis) used for the positioning of the elements required for the construction of the part. 2.2 Practical advice - When you modify an object (adding a fillet radius to a body), do not forget to activate the "Define in work object" command (Mouse Key 3). - When you want to delete an entity, take care not to destroy the parents but only the element in question. Deleting the parents is to be prohibited when the work of the definition phase is well under way. - The fillet radii of the walls of a pocket must not be defined on the sketch but as "fillet" features. Issue:Draft A1 Date: 13 February 2002 Page 5 of 46
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AP2257 - Draft A1 - Machined Part Modelling for CATIA V5

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