Acess al feature parameters

Hi,

try contacting PTC Support.

Oh, the hidden gems of Creo 🙂

In the dark corners of the internet, you can find references of how you can switch pattern tables with relations.

Eng-tips (februari 2004)

https://www.eng-tips.com/viewthread.cfm?qid=86497

PTC Article CS25675 (juli 2011)

https://www.ptc.com/en/support/article?n=CS25675

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Description
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Using part relations to specify the use of a specific pattern table within a part.


Alternate Technique
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After creating more than one pattern table, select #Add from the Relations menu 
and enter in the following syntax: 
        pattern_table:fid_(pattern_table_id_number) = "pattern_table_name"

Where pattern_table_id_number is the Feature ID of the first feature in
the pattern and pattern_table_name is the name given to the pattern table.

For example, with two pattern tables, FOUR_HOLES and EIGHT_HOLES, the design
requires that pattern table FOUR_HOLES be used when the LENGTH of a part is 
less than 10 and greater than zero. Pattern table EIGHT_HOLES is to be 
used when the LENGTH of the part is greater than or equal to 10. In this
example ADD the following relation to the part by selecting #RELATION #ADD: 

  IF LENGTH > 0 & LENGTH < 10
        PATTERN_TABLE:FID_21 = "FOUR_HOLES"
  ELSE 
        IF LENGTH > 10 | LENGTH == 10
                PATTERN_TABLE:FID_21 = "EIGHT_HOLES"
        ENDIF
  ENDIF

NOTE: The text for the name of the pattern table *must* be in uppercase letters.
Pro/ENGINEER is case sensitive to this variable, and will issue an error message
if the value contains lowercase letters.