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.
