3D modelling rules for CATIA V5

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AIRBUS AP2255
Procedure
Issue: Draft A1 Date: February 2002 Page 1 of 37
3D modelling rules for CATIA V5
Owner’s Approval:
Name : Bruno MAITRE EMK-T
Function : Head of CATIA V5 Methods for French
Team
 Airbus 2002 . All rights reserved. This document contains Airbus proprietary information and trade secrets. It shall at all times
remain the property of Airbus; no intellectual property right or licence is granted by Airbus in connection with any information
contained in it. It is supplied on the express condition that said information is treated as confidential, shall not be used for any
purpose other than that for which it is supplied, shall not be disclosed in whole or in part, to third parties other than the Airbus
Members and Associated Partners, their subcontractors and suppliers (to the extent of their involvement in Airbus projects),
without Airbus prior written consent.
Authorization:
Date :
Name : Ulrich SCHUMANN-HINDENBERG
Function : Head of CAD-CAM CM (EMK)
SCOPE:
The aim of this document is to list the general rules to be complied with for the 3D
modelling of all types of parts.
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 2 of 37
Table of contents
1 Introduction............................................................................... 4
2 General rules............................................................................. 5
2.1 Designation and numbering of files......................................................... 5
2.2 Positioning baseline .................................................................................. 5
2.3 Elements to be distributed on layers....................................................... 5
2.4 Modelling of parts in context.................................................................... 5
2.5 Modelling of detail parts............................................................................ 5
2.6 Modelling of equipped parts with unique representation...................... 6
2.7 Modelling of equipped parts with multiple representations.................. 6
2.8 Symmetrical parts...................................................................................... 7
2.9 Variant parts ............................................................................................... 8
2.10 Parts with complex surfaces .................................................................... 8
2.11 Conditions of supply ................................................................................. 8
2.12 Drill-holes ................................................................................................... 9
2.13 Removability volume................................................................................. 9
2.14 Kinematic volume...................................................................................... 9
3 Specific rules........................................................................... 10
3.1 Machined parts......................................................................................... 10
3.2 Sheet metal parts ..................................................................................... 10
3.3 Panels ....................................................................................................... 10
3.4 Profiled parts............................................................................................ 10
3.5 Piping ........................................................................................................ 10
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3D modelling rules for CATIA V5
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3.6 Electricity.................................................................................................. 10
3.7 Composite ................................................................................................ 10
4 Structuring of data in a CATPart ........................................... 11
4.1 Design by modelling independent entities............................................ 11
4.2 Grouping elements in the various bodies of a CATPart. ..................... 15
4.3 Explicitly renaming elements ................................................................. 22
5 Optimised modelling for updates .......................................... 23
6 Modifying and correcting a model......................................... 29
6.1 Modifying a model ................................................................................... 29
6.2 Design with update cycle........................................................................ 29
6.3 Correcting errors ..................................................................................... 30
7 Check of a model before officialisation ................................ 35
7.1 Destroy all unnecessary elements......................................................... 35
7.2 Do not use red for solids......................................................................... 35
7.3 All elements except solid in no-show.................................................... 35
7.4 Publish reference elements .................................................................... 35
7.5 Check that solid is updated .................................................................... 35
Reference documents ........................................................................................... 36
Group of redaction ................................................................................................ 36
Approval and authorization .................................................................................. 36
Record of revisions ............................................................................................... 37
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 4 of 37
1 Introduction
This document includes all of the 3D modelling rules. It also directs the designer to
specific manuals (subsidiaries) for consultation. In addition, it includes recommendations
for the structuring of the part data and verifications before officialization.
It mainly concerns use of the Part Design, Generative Shape Design and Sketcher
workbenches. For the use of these CATIA V5 workbenches consult others specific
documents, as AM2119 Part Design, AM2117 Wireframe & Surfaces, AM2118 Sketcher,
AM2252 CATIA V5 Multi-models links …
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3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 5 of 37
2 General rules
2.1 Designation and numbering of files

Consult AP2610.
CAUTION: In CATIA V5, when a new xxx.CATPart file is saved in a directory, the Part
Number field of the part properties (visualised in the tree) is not systematically filled in
with the xxx character string.
Correspondence is absolutely necessary between the filename
(l53s12345200.CATPart) and the part reference (Part Number = l53s12345200).
On creation of a new part (File + New + Part or command New Part in Assembly Design
workshop), immediately fill the Part Number field in the Part name window. Then save
the file (Save As): the filename is then initialised with the part reference.
Remarks:
• The Part name window is systematically proposed when option ‘Tools + Options +
Infrastructure + Product Structure + Part Number + Manual input’ is activated. This
option should be locked by the CATIA administrator.
• To modify the Part Number, modify the properties of the part (contextual menu).
• If properties are modified after 'Save As', the part reference must be entered twice.
2.2 Positioning baseline
TBD
2.3 Elements to be distributed on layers

Consult AP2622 CAD layers organisation.
2.4 Modelling of parts in context
TBD
2.5 Modelling of detail parts
• To allow use of detail part file in CAM, model one part per CATPart file.
• In a CATPart, there must only finally be one main part body (PartBody),
except for conditions of supply which must be created in the bodies of the
secondary parts if the manufactured parts are different once installed on
aircraft.

Consult Conditions of supply chapter.
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2.6 Modelling of equipped parts with unique representation
An equipped part must be an assembly of its various detail parts and standard elements.
• No data duplication.
• A single part body per CATPart and not one main part body and secondary
part bodies for standard elements.
• CATProduct evolves simultaneously with the CATPart of the standard
element.
2.7 Modelling of equipped parts with multiple representations
Example: equipped rod
TBD
2 instances of same part
positioned in the assembly
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3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 7 of 37
2.8 Symmetrical parts
Procedure for producing the geometrical model of symmetrical part:
• Create a new file .CATPart: File + New Part.
• Modify the name of the part (Properties) and save the file with the reference of
the part -201.
• Open in same session the file of part -200.
• Copy the solid into the document -200.
• Paste the solid into document -201 (Paste Special AsResultWithLink).
• Produce symmetrical solid in relation to the symmetry plane. If this plane is
specifically defined in part –200, previously import this plane into part –201
(Copy / Paste Special + AsResult).
• Assemble the main part body "PartBody" and the copied solid (Insert +
Boolean Operations + Add).
• Position part 201 in the assembly.
Caution: Do not copy / paste part –200 in a CATProduct.
Advantage: all changes to part -200
will automatically be taken into
account for the symmetrical part
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3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 8 of 37
2.9 Variant parts
Creation of a variant:
• Create a new reference -203 from part -200 (File + New from followed by Save
As).
• Make the modifications.
• Save.
• Replace, if applicable, part -200 by -203 in the assembly "Replace
component".
Remark: for a variant, "copy AsResultWithLink" is not used to access the specification
tree for the modifications.
2.10 Parts with complex surfaces
• Parts modelled with reference: during design, the surfaces (from Master
Geometry, of shape label) used for the modelling of the part must be
duplicated in specific open bodies. The designer decides whether the
modelling and/or surface modification must pass via the Shape Reference
Group.

Consult Chapter 4 Structuring of data in a CATPart.
• Part with unreferenced surface: the unreferenced surfaces created for the
modelling of a part will be grouped in a working open body. The designers
ensure full responsibility for the modelling of the surfaces that they produce.

Consult Chapter 4.2.2 Ordering various bodies in specification tree.
2.11 Conditions of supply
The conditions of supply are integrated into the definition dossier:
• Length / overthickness installed on aircraft: the length or overthickness is
integrated into the part solid, that is the main part body.
Example: for installation dispersion reasons and to ensure the minimum holeto-
edge distance of 10 mm, the part contour is drawn at 12 mm.
Minimum hole-to-edge distance 10 mm Part contour defined at 12 mm
Disadvantage: if a change to part -200 must be passed on to part -203, the
modification must be done manually.
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3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 9 of 37
Specific case of so-called "internal" restrictions:
These restrictions are integrated into the solid defining the part, that is the
main part body.
• Length/overthickness adjusted on installation: the solid is isolated in a
secondary part body.
Example:
• Handling and installation lug: the solid is isolated in the secondary part
body.
Parts which are different once installed on aircraft but identical at storable part
stage must bear different references (part number) (File + New from then
modification of properties + Save as).
The drill-holes and bores are modelled at nominal diameter.
Unless specified otherwise on the drawing, the solid is represented with mean
dimensions.
Except in special cases, the following are not taken into account in the CAD
model: sealant or interfay thicknesses, protection thicknesses and part contact
face tolerances which lead to the upward adjustment phenomenon. This
upward adjustment is absorbed by the tolerance of the TDD on the external
shapes. For this purpose, the CAD model does not represent perfect
modelling at mean dimensions.
2.12 Drill-holes
TBD.
2.13 Removability volume
TBD.
2.14 Kinematic volume
TBD.
10 min after fitting
Solid in secondary part body
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3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 10 of 37
3 Specific rules
3.1 Machined parts

Consult AP2257 Machined part modelling for CATIA V5
3.2 Sheet metal parts

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
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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
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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
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3D modelling rules for CATIA V5
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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
containing several profiles.
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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.
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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.
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• 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
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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.
• 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
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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.
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• 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.
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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
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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
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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
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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.
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The solution in this example could be to create a plane with an other type. For
instance, a plane through a planar curve and then to select the feature Intersect.1
which is a planar curve. The Intersect.1 would be, as Intersect.2, a stable
specification to store.
In the plane definition, plane through two lines,
the Line 1 corresponds to a feature selection
(Intersect.2) which is a stable specification
stored. The Line 2 corresponds to a 3D
geometrical representation selection (Edge.1),
which is not a stable specification stored.
In our example the user has selected an edge of
this curve to specify a line.
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Example 2 :Creation of an element based on a multiple intersection
To be able to select a feature when the specification is the result of a multiple
intersection, use the ‘Near’ command.
In this example, the intersection of the line and the surface results in 2 points. Then, the
Multi-Result Management window appears and proposes to keep only one element.
Press Yes if you already know at this step which point you want to keep.
The Near Definition command
is automatically launched
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Issue: Draft A1 Date: February 2002 Page 27 of 37
Select the reference element (the nearest) to indicate which point you want to keep.
Don’t forget to try to select a stable element, for example Point.1.
Press OK to create Near.1 linked to Intersect.1.
The result is the creation of a Near.1 feature, a stable specification if you
have to select a point, rather than a vertex.
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Remark :
If you don’t create the Near feature during the intersection creation (Pressing No instead
of YES in the Multi-Result Management window), you can use the Near command
afterwards.
Pressing NO, you obtain:
Use Insert + Operations + Near to distinguish one point between the two points
computed during intersection.
Intersect.1 is a non connex element
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3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 29 of 37
6 Modifying and correcting a model
6.1 Modifying a model
• For an important modification requiring complete remodelling of the part, do not
duplicate the CATPart. Mandatory ’Get’ the CATPart in VAULT, destroy the existing
data in CATPart and restart definition (UUID conservation problem).
• To store a change in geometry:
1. Create a specific body called ‘Modifications’.
2. Extract the main modified faces from the solid in the ‘Modifications’ body.
3. Position these faces on the modification layer (
Consult AP2622 CAD layers
organisation).
4. Place these faces in No Show mode.
Remark: The DMU Space Analysis workshop offers the possibility of comparing the
differences between 2 CATProducts or 2 CATParts. This comparison can be stored in
image form.
6.2 Design with update cycle
An update cycle is generated when an element is created from specifications which
depend upon it. An update cycle, rare during a creation phase, is however much more
common during a modification phase, the replacement of an element (Replace) and the
reorganisation of an element (Reorder). Also, the possibility of creating an update cycle
is increased during hybrid design.
Compliance with the methodological instructions in this manual limits the risk of update
cycles.
Example: Modification of a plane defined from 3 points
Creation chronological order:
• In PartBody, creation of an extrusion Pad.1
• In Open_body.1: creation of Plane.1 from Point.1, Point.2, Point.3
• In PartBody: creation of Split.1, cut of Pad.1 by Plane.1
Pad.1
Plane.1
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To modify Plane.1, edition of plane specifications (the 3 selected points) in Plane
Definition window. Attempt to replace one of the 3 points by a point of Pad.1.
Pad.1 depends on Plane.1 as it is cut by it. It is therefore impossible that definition of
Plane.1 bears on a geometry of Pad.1:
• Pad.1 becomes red.
• A window appears to indicate that Split.1 is involved in an update cycle.
• 'Warning' symbols appear in the specification tree.
CAUTION: All update cycles are not necessarily detected by CATIA V5. Under these
circumstances, the update of the model will not be completely executed and the result
will be an endless loop during execution of the ‘Update’ command.
6.3 Correcting errors
The update of a model, required after a modification or a change of version may be
interrupted due to errors. These errors must be processed one by one to reobtain an
equivalent definition before starting update.
To process an error, edit the element which cannot be reconstructed and modify the
specification posing problems. Any uncorrected errors will lead to an inactivated element
and therefore all constructions bearing on this inactivated element will be invalid.
Selection of a Pad.1 point to modify Plane.1
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3D modelling rules for CATIA V5 for CATIA V5
Issue: Draft A1 Date: February 2002 Page 31 of 37
Example: Update of a part subsequent to a change of version (from V5R4 to V5R6).
• If problems are encountered during execution of command 'Update', CATIA will stop on the first error encountered (option
selected for update). Here, for an unknown reason, reconstruction of Sketch.8 is not done correctly. Thus revolution solid
Shaft.1 cannot be rerun.
The user is warned by the 'Warning' symbols in the
specification tree.
Windows analysing the error are displayed to inform the user:
• Shaft1: the profile intersects the axis, change profile or
axis
• Sketch.8: unable to find a consistent solution
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Issue: Draft A1 Date: February 2002 Page 32 of 37
• At this stage, the element causing problems can be deactivated, destroyed or edited. In deactivation and destruction cases, any
constructions bearing on the element in question will be lost. It is therefore strongly recommended to edit the element to correct
the specification in order to continue the update. Process in this way, one after each other, all errors detected.
Remark: in certain cases, the user may possibly decide that it is quicker to destroy the element then reconstruct it rather than
correct it.
Avoid deactivating or destroying.
In our example, the choice ‘Deactivate’ leads to new
errors for the points and edges and subsequently for
the fillets constructed from Shaft.1
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3D modelling rules for CATIA V5 for CATIA V5
Issue: Draft A1 Date: February 2002 Page 33 of 37
• Rather than deactivating, select ‘Edit’ option:
• In our example, sketch of Shaft.1 no longer corresponds to the initial geometry. It must therefore be corrected to reestablish the
definition.
A window recalls the source of the error: click ‘OK’ to
display Shaft.1 definition window
Click command Sketch in ‘Shaft Definition’ window to
modify the sketch.
AIRBUS AP2xxx
3D modelling rules for CATIA V5 for CATIA V5
Issue: Draft A1 Date: February 2002 Page 34 of 37
• Work in 'Sketcher' workshop to correct the sketch.
Once the sketch has been corrected, exit the
‘Sketcher’ workshop. Update can continue, Shaft.1 is
reconstructed together with the fillets bearing on it.
AIRBUS AP2xxx
3D modelling rules for CATIA V5 for CATIA V5
Issue: Draft A1 Date: February 2002 Page 35 of 37
7 Check of a model before officialisation
7.1 Destroy all unnecessary elements
For coherence, size and therefore model performance and legibility reasons, all
geometrical elements generated during design which are no longer useful must be
deleted (especially if the geometry was imported and is no longer referenced).
7.2 Do not use red for solids
Avoid red for geometric elements especially solids. This colour can be confused with
highlighting and especially is the colour used to indicate that an element must be
updated.
7.3 All elements except solid in no-show
For mock-up reviews and data exchanges, all construction elements (surface, wireframe,
etc.) must be in no-show mode.
7.4 Publish reference elements
To be able to use the elements in a context, publish the geometry which will be used as
reference for the modelling of other parts.
7.5 Check that solid is updated
Check the positioning of the elements in the layers

Consult AP2622.
AIRBUS AP2xxx
3D modelling rules for CATIA V5 for CATIA V5
Issue: Draft A1 Date: February 2002 Page 36 of 37
Reference documents
AM 2117 CATIA V5 Wireframe & Surfaces
AM 2118 CATIA V5 Sketcher
AM 2119 CATIA V5 Part Design
AM 2253 Tubing installation modelling for definition phase CATIA V5
AM 2254 Electrical installation modelling for definition phase CATIA V5
AM2252 CATIA V5 Multi-models links
AP 2257 Machined part modelling for CATIA V5
AP 2258 Profiled part modelling for CATIA V5
AP 2259 Sheet metal part modelling for CATIA V5
AP 2610 Naming and Numbering for New Projects
AP 2622 CAD layers organisation
Group of redaction
Team members Company/Department telephone
F. Kautz Airbus Deutschland
S. Lerat EMK-T
P. Cano Airbus España
M. Horwood Airbus UK
Approval
This document has been approved on behalf of the following:
(signatures or proof of agreement are archived together with the master document)
Organization Approval
ACE/SPD/Cax
Technology/Method
CANO-RODRIGUEZ Pedro-Jesus
Airbus España
EM Quality Assurance
representative
Nicole Lamothe (EMZQ)
CoC Structure H Schnell (ESDS)
CoC Systems and
Integration tests
F. Capecchi (EYD)
AIRBUS AP2xxx
3D modelling rules for CATIA V5 for CATIA V5
Issue: Draft A1 Date: February 2002 Page 37 of 37
Record of revisions
issue Date Summary and reasons for changes
Draft A1 February 2002 Initial issue
If you have a query concerning the implementation or updating of this document,
please contact the Owner on page 1
Or a team member of the group of redaction
For general queries or information contact:
Airbus Documentation Office,
Airbus
31707 Blagnac CEDEX,
France
Tel: 33 (0)5 61 93 49 93
Fax: 33 (0)5 61 93 27 44

hellosharp

Good, Thanks

viplixuan

thks alot 。非常感谢

chrislt

Good work, thank you

lizhiming0707

什么啊 这还有什么rule啊