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sfinke1-Visitor
1-Visitor
December 15, 2015
Solved

Annotation display for hole features

  • December 15, 2015
  • 3 replies
  • 15964 views

So if I create a threaded hole feature I can see the hole callout on screen giving me the details of the  that hole feature.

BUT

If I create a counter-bored hole feature I get no hole call out.

Why is this? If this is a setting that needs to be adjusted why is it not uniform by default?

    Best answer by lsrutkowski

    If you create a hole feature using the hole tool and select a threaded hole, Creo will automatically generate a note based on the .hol file for the thread style you have selected.  If you select the hole tool, but do not use the thread based portion of the tool, a note will not be generated.  Why this is the case, I do not know, but this has been the norm since the hole tool was added to Wildfire.

    If you want a counter-bored hole for a screw, you can use the threaded hole portion and select to remove the threads.  This will set the hole to be a clear-hole for the thread size selected (once again, based off of the .hol file for the selected thread type).  However, by default, the note for the threaded holes leave a lot to be desired.  There are several threads already on the forums here that detail how you can expand the tables into something more useful (I recommend correcting the mistakes that exist in some of the diameters to start with).

    Calling out Counter bores in Drawings.

    Re: Dimensioning holes/creo2.0

    Counterbore/Countersink hole Notes on Drawing.

    Creo 2.0 Help Center on Hole Tables: http://support.ptc.com/cs/help/creo_hc/creo20_hc/index.jspx?id=hole_tables_about&action=show

    3 replies

    L
    lsrutkowski1-VisitorAnswer
    1-Visitor
    December 15, 2015

    If you create a hole feature using the hole tool and select a threaded hole, Creo will automatically generate a note based on the .hol file for the thread style you have selected.  If you select the hole tool, but do not use the thread based portion of the tool, a note will not be generated.  Why this is the case, I do not know, but this has been the norm since the hole tool was added to Wildfire.

    If you want a counter-bored hole for a screw, you can use the threaded hole portion and select to remove the threads.  This will set the hole to be a clear-hole for the thread size selected (once again, based off of the .hol file for the selected thread type).  However, by default, the note for the threaded holes leave a lot to be desired.  There are several threads already on the forums here that detail how you can expand the tables into something more useful (I recommend correcting the mistakes that exist in some of the diameters to start with).

    Calling out Counter bores in Drawings.

    Re: Dimensioning holes/creo2.0

    Counterbore/Countersink hole Notes on Drawing.

    Creo 2.0 Help Center on Hole Tables: http://support.ptc.com/cs/help/creo_hc/creo20_hc/index.jspx?id=hole_tables_about&action=show

      S
      sfinke1-VisitorAuthor
      1-Visitor
      December 17, 2015

      Thanks.

      If you select the hole tool, but do not use the thread based portion of the tool, a note will not be generated.  Why this is the case, I do not know, but this has been the norm since the hole tool was added to Wildfire.

      Sounds like a pretty big flaw if you ask me.

        C
        cmoreno1-Visitor
        1-Visitor
        July 22, 2020

        Pretty standard for this software if you ask me. Its riddled with flaws and inconsistencies and frustrations to make you pull your hair out. Really feel creo is a russian plot to undermine american productivity.

          A
          anthonyws13-Aquamarine
          13-Aquamarine
          September 24, 2024

          Creo is full of this half baked nonsense. The effort to set up some parameters and configurations (akin to coding) is not worth the time. Just create a note. sadly there is no parametric functionality however. so editing a hole size/profile results in outdated drawing that need careful review and editing. Total productivity killer

            S
            Shumayal11-Garnet
            11-Garnet
            January 9, 2025

            I totally agree. The more I use CREO, the more I miss SolidWorks.

            P
            19-Tanzanite
            pausob19-Tanzanite
            19-Tanzanite
            May 31, 2025

            For sake of completeness, I'm noting that at some point since 2015 (it is there in Creo 10), standardized notes can specified and automatically attached to the "simple" type of holes:

            pausob_0-1748719853447.png

            To be fair, the out-of-the-box hole format remains somewhat awful looking, but it can be customized to fit your standards.

              R
              RaphMORIN16-Pearl
              16-Pearl
              June 2, 2025

              Yes but it doesn't support counterbore or countersink holes. I'm also wondering if we can customize the number of digits.

              P
              19-Tanzanite
              pausob19-Tanzanite
              19-Tanzanite
              June 2, 2025

              Yes, out of the box it doesn't, but you can customize the DEFAULT_CALLOUT_FORMAT_DATA table in the hole files simple_drilled.hol and simple_flat.hol

              For illustration:

              pausob_1-1748882541159.png

              The number of digits can be controlled by the "standard" method of appending the [.n] to the &parameter callout where n is the # of decimal places.  For example above, if my callout definition was &DIAMETER[.1] then note would show Ø0.5 instead of Ø0.500

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