HD64361: PART: RIB- THE RIB FEATURE CANNOT BE CREATED.

APAR status

• Closed as Permanent restriction.

Error description

• PART: RIB- THE RIB FEATURE CANNOT BE
  CREATED.
  .
  SCENARIO.
  1. Start CATIA V5R16SP09. Work Bench- Part
  Design.
  2. Open the file Rib-err.CATPart.
  3. Select Rib command.
  4. Select Sketch.2 as profile and Intersection.1 as
  the centre curve.
  4. Click OK. The Feature Definition Error message
  is displayed. This is the problem.
  Error: The Rib feature cannot be created.
  .
  .
  EXPECTED RESULT.
  The Rib feature should be created.
  .
  .
  

Local fix

Problem summary

• PART: RIB- THE RIB FEATURE CANNOT BE CREATED.
  PART: RIB- THE RIB FEATURE CANNOT BE
  CREATED.
  .
  SCENARIO.
  1. Start CATIA V5R16SP09. Work Bench- Part
  Design.
  2. Open the file Rib-err.CATPart.
  3. Select Rib command.
  4. Select Sketch.2 as profile and Intersection.1 as
  the centre curve.
  4. Click OK. The Feature Definition Error message
  is displayed. This is the problem.
  Error: The Rib feature cannot be created.
  .
  .
  EXPECTED RESULT.
  The Rib feature should be created.
  .
  .
  

Problem conclusion

• null
  ==========*===========*==========
  THIS PROBLEM IS PERMANENT RESTRICTION IN
  CATIA
  .
  Incident Diagnosis.
  The rib feature can not be created.
  .
  Restriction Explanation.
  The intersection is done in area where edges are
  not smooth. So the generated intersection with a
  plane generate several edges which are sharp. The
  limit for a smooth edge is a discontinuity of 0.5
  degree.
  After the intersection, there is a small tangency
  discontinuity of 0.8 degree. During the sweep
  generation, parallel curve to the center curve has
  to be computed to reach the profile position.
  An extrusion has to be done for each edge of the
  center curve and then a relimitation has to be done
  to connect all the extrusion.
  During this process, because the tangency
  discontinuity is very small, there is confusion area
  (faces almost tangent) and relimitation can not be
  done.
  By replacing the sharp vertex by a smooth vertex,
  sweep can be done in one shot without relimitation.
  .
  By Pass.
  1. Open Rib-err.CATPart in V5R16SP09.
  2. Open Workbench Generative Shape Design.
  3. Select the Curve smooth command and select
  the intersection to be used as Rib centre curve.
  4. Put Tangency threshold value = 1 deg.
  5. Click OK.
  6. Now move to workbench Part design.
  7. Click Rib command and select Sketch.2 as
  profile and Curve smooth.1 as centre curve.
  8. Click OK.
  .
  .
  

Temporary fix

Comments

APAR Information

• APAR is sysrouted FROM one or more of the following:

• APAR is sysrouted TO one or more of the following:

Fix information

Applicable component levels