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3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 25 of 37
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.
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 26 of 37
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
AIRBUS AP2255
3D modelling rules for CATIA V5
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.
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 28 of 37
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
AIRBUS AP2255
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
AIRBUS AP2255
3D modelling rules for CATIA V5
Issue: Draft A1 Date: February 2002 Page 30 of 37
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
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