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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
AIRBUS AP2xxx
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
AIRBUS AP2xxx
3D modelling rules for CATIA V5 for CATIA V5
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
AIRBUS AP2xxx
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
　
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