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BC_108485724-Participant
4-Participant
Oct 8, 2026 4:15 PM UTC
Question

Parameter Suffix

Hi, I usually input the number of pattern instances using the parameter from the model into a drawing note and that will display the number of instances. Now, when I do that, it includes the suffix, which it never did before. Is there a setting I can change that toggles this behavior? I am using Creo 9.0.12.0.

For example, with a feature patterned 4 times:

  • Before: &p267 would display “4”
  • Now: &p267 displays “4 EXTRUDES”

I can manually delete the suffix text as a workaround, but I’m curious what changed from “before” to “now”.

      6 replies

      KenFarley
      KenFarley21-Topaz II
      21-Topaz II
      Oct 9, 2026 2:39 PM UTC

      When I want ot use these things in drawing notes/dimensions, I also find that I need to “fix” things.

      I usually edit the pattern dimension in the model. If I still want to have the suffix but don’t want it to contaminate my note/dims on the drawing, I put the suffix text on a second line int the “Dimension Text” box while deleting it from the Suffix box. I seem to recall this becoming necessary after we switched to Creo 9 from Creo 4.

      This is one of those things that is annoying when using pattern dimensions, but can be nice for other dimensions, like if I want to use a diameter dimension in a note, it will include the diameter symbol. Or if I have a depth dimension I want to use I can add something like “ MIN” to the dimension and it will show up in the references.

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        BC_108485724-ParticipantAuthor
        4-Participant
        Oct 19, 2026 7:25 PM UTC

        The strange thing for me is that I’ve been using Creo 9 the entire time at this current company so I must have inadvertently changed the setting myself or something on the administrative IT side that they can’t identify changed the behavior in the background.

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        MikeBennett
        MikeBennett17-Peridot
        17-Peridot
        Oct 27, 2026 12:41 PM UTC

        Hi ​@BC_10848572, 

         

        I see ​@KenFarley has replied on a few other Community posts regarding this topic of pattern suffix text in the last few years.  According to CS280937, there is no option to toggle/control the suffix from pattern text.  There was a more recent attempt at requesting suffix control documented in CS461978 with the same result.  However, in the internal notes in this SPR, I found a detail that the change solidifying the displayed suffix occurred in Creo Parametric 8.0.12.0 and parallel newer builds (probably +/- 2 months from Jan 2025 so roughly 9.0.10.0, 10.0.8.0, 11.0.3.0)  If you were using an earlier datecode of Creo 9.0 before updating to 9.0.12.0, that would explain the difference.

         

        If you think this is worth creating a Product Idea to request a toggle and can explain a good usecase/example for inclusion, a Product Idea would be the best method for requesting that addition.

         

        Hope this information helps clarify that change,

        Mike

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        Srinivasan-Iyer15-Moonstone
        15-Moonstone
        Oct 27, 2026 6:54 AM UTC

        Hi,

        Have a look at the following link and set the callout format accordingly.

        Hole Note Format

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        Knowing, what we know is just a fistful of Earth, brings in humility.
        KenFarley
        KenFarley21-Topaz II
        21-Topaz II
        Oct 27, 2026 4:12 PM UTC

        The question has nothing to do with hole notes. The person asking is trying to understand the behavior of Creo when the pattern dimension for the number of pattern members is referenced in a note.

        My suspicion is that at some point the code was changed so the “EXTRUSIONS” or whatever the descriptor text is was moved from the “Dimension text” portion of the dimension to the “Suffix” portion. The former does not get pulled into a reference, the latter (as well as the “Prefix”) does get pulled in.

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        Srinivasan-Iyer15-Moonstone
        15-Moonstone
        Oct 28, 2026 4:25 AM UTC

        Hi Ken,

        I understand the concern of the original post. It is that of suffix “HOLES” added to the @p# parameter. There was a video on YouTube on how to tackle this via defining the Hole Callout Format. On the page that I shared, there are attributes that the Pattern parameter picks up.

        Here are a few good videos:

        https://www.youtube.com/watch?v=HpzO3HqrbO4

        Creo Parametric - Custom Hole Charts (Part 2 of 3) (watch all the three parts)

        To be honest, I have not had the time to read and understand it thoroughly as it is really long and age has caught up with my ability to grasp new things.

        I use &PTC_ACTUAL_PAT_MEMBERS instead of &p# and it works.

        Syntax to include the Feature ID

        Hope it helps.

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        Knowing, what we know is just a fistful of Earth, brings in humility.
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