HD92667: DRAFTING - TEXT AFTER HAS A GAP BETWEEN DIMENSION VALUE AND TEXT AFTER.

APAR status

• Closed as user error.

Error description

• Scenario :
  1- Start CATIA in Administration mode with provided xml file
  located in Drafting Standard environment
  2- File / Open the CATDrawing file
  3- Go to Tools / Standards - In category 'Drafting', select
  the provided xml file
  4- Inside Dimensions node, set the two parameters 'Horizontal
  offset of Before text' and 'Horizontal offset of After text'
  to Zero
  5- Save this new xml file (Save as New) and select OK for
  Standard Definition window
  6- File / Page Setup and update the Drawing with the xml file
  created on step 5
  7- Create a new dimension in the Drawing
  8- Set an associated Text before and after this dimension,
  using MB3 on this dimension / Properties / Dimension Texts
  tab
  Problem :
  There is a gap between the 'dimension value' and the 'Text
  after'.
  Expected Result :
  There is no gap between the 'dimension value' and the 'Text
  after'
  

Local fix

• empty
  

Problem summary

Problem conclusion

Temporary fix

Comments

• Incident Diagnosis:
  Even if the standard parameter "Horizontal offset of After
  text" is set to 0, the distance between the Dimension Value
  and the Text After for the providied dimension is not null.
  Correct Application:
  The "Horizontal offset of After text" specifies the distance
  from the dimension value. The value includes the tolerance,
  and in the provided data, a tolerance of type "DIN_NUM2" is
  set, with +/-0mm for values. But if you look into the
  Interactive Drafting documentation / Administration Tasks /
  Pre-defined Styles Definition, you will see that this
  tolerance (DIN_NUM2) format is specified to not show the
  tolerance values if they have null values (TolShowNull=3).
  Note that in 'Dimension Tolerance Formats' chapter, you can
  read in Parameter 'Display of null Tolerance Values (for
  numerical tolerances only) that the Parameter Name
  (TolShowNull) is equal to 3 (No Display of null value)
  This however does not prevent the "Offset between dimension
  value and tolerance" parameter to apply, and in this case
  this offset is defined to 0.6 (TolExtX=0.6 for Tolerance
  DIN_NUM2)
  .
  As a conclusion, to get the desired result, either the
  tolerance should be unset, or a new tolerance format should
  be defined with a parameter TolExtX set to 0 : go in Tools /
  Strandards / General / Allowed Tolerance Formats and add a
  tolerance with TolExtX set to 0 in the list.
  Documentation:
  Manual Reference: Interactive Drafting
  Chapter: Administration Tasks
  Topic:
  Pre-defined Styles Definition
  Dimension Tolerance Formats
  

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