HD95549: GSD: PLANE: UNABLE TO CREATE OFFSET PLANE WHEN REFERENCE PLANE I S SELECTED FROM SPECIFICATION TREE.

APAR status

• Closed as suggestion for future release.

Error description

• SCENARIO:
  1. Start CATIA V5
  2. Select File / New / Part
  3. Deactivate ￢ﾀﾜEnable hybrid design￢ﾀ  option and click ok.
  4. Click on Positioned sketch icon
  Sketch positioning dialog box appears
  5. Right click at Reference, select Create Plane to have an
  aggregated plane within the positioned sketch
  Plane definition dialog box appears
  6. Select XY plane as reference and input offset distance as
  20 mm
  7. Click Ok in plane definition dialog box and then into
  sketch positioning dialog box
  8. Create a rectangular sketch and click exit workbench
  Observation:
  Rectangular sketch is created on Plane.1 which is 20mm offset
  to XY plane.
  9. Expand the specification tree
  Observation:
  Plane.1 is located under Absolute axis
  10. Right click on Plane.1 and select Hide/show to make it
  visible.
  11. Select Plane icon
  Plane definition dialog box appears
  12. Select Plane type as offset from plane, Select plane.1
  from 3D geometry area and input any offset value and click Ok
  Observation:
  Plane.2 is created-This is correct behavior.
  .
  13 Select Plane icon
  Plane definition dialog box appears
  14. Select Plane type as offset from plane
  15. Try to select plane.1 from specification tree-This is a
  key point
  Observation:
  Instead of Plane, sketch is selected and highlighted and
  error appears.
  Update error:
  Reference point missing.
  You must specify a reference point to create a plane normal
  to a closed curve.
  The default middle point cannot be used in this context.
  Select a reference point.￢ﾀ
  .
  16. Click ok on error
  Observation:
  Plane definition dialog box appears and plane type is changed
  to Normal to curve
  .
  PROBLEM:
  Unable to create offset plane when reference plane (which is
  aggregated under positioned sketch) is selected from
  specification tree.
  .
  EXPECTED RESULT:
  It should be possible to create offset plane even though
  reference plane is selected from specification tree.
  

Local fix

• empty
  

Problem summary

Problem conclusion

Temporary fix

Comments

• Dear Customer:  we have reviewed the problem report you
  submitted and determined that the function referenced is
  working within the scope of the original design
  specification. However we recognize the value of your
  feedback and will consider including resolution of this issue
  as a product enhancement in a future release, if one is made
  available.  We thank you for your input.
  Additional Closure Information:
  .
  INCIDENT DIAGNOSIS:
  In Non-hybrid body, it is not possible to create offset plane
  if a reference plane (aggregated under a Sketch) is selected
  from specification tree. Instead of Plane, sketch is selected
  and highlighted and error appears. However it is possible to
  create offset plane if a reference plane (aggregated under a
  Sketch) is selected from 3D geometry area
  .
  Development Request Justification
  In CATIA, each command scans the path of object selected by
  mouse. This path is the list of the fathers that aggregate it
  and it is analyzed according to the types of features that
  can be accepted at any state of the command. The issue relies
  in the analysis of the path, which is made by analyzing all
  the fathers with respect to the acceptable types of feature.
  Then, as long as the sketch is acceptable as an input,
  it is selected instead of the plane. The construction of the
  path itself differs between the Hybrid and non-Hybrid mode,
  and between the selection in the 3D and in the graph.
  When the user selects the object from 3D geometry, the path
  is built regardless of the specification tree structure, and
  there is only a plane (the one that is selected) and a part.
  Consequently, only acceptable object in the list is the plane
  itself that is why the selection from the 3D geometry is
  possible.
  .
  When the user selects from specification tree, the path is
  built with the selected object and the different
  features (tools) that aggregate it in specification tree. In
  hybrid mode, the Sketch is considered as a tool, and it
  belongs to the list and since it is acceptable, plane
  aggregated under sketch can be selected.
  On the contrary in non hybrid mode, it is not considered as a
  tool and hence it does not belong to the list and hence plane
  aggregated under sketch cannot be selected.
  To conclude, this issue is linked to the main principles of
  the selection in CATIA.
  In order to correct this problem, huge development is
  necessary as it requires complete rewriting of existing code.
  However such a huge enhancement cannot be done on the current
  levels as this is be highly impacting and may affect other
  functionalities as well.  So please open an ERD for this so
  that the development team can completely analyze the request
  with respect to its impact on the code and then implement it.
  .
  By-Pass:
  Select feature from 3D geometry or move the plane into a
  Geometrical Set.
  

APAR Information

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Fix information

Applicable component levels