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NX 10 - Unecessary spacing in Hole callout


Hello again


I have been playing all day long with Hole callout and I like what I see so far. But I am not able to figure out what setting controls the spacing between the callout components (for example between 4 and X in the pattern count as depicted below).




Any ideas? This will be like icing on the cake for me. 


Also, from what I read in the forum, it seems not yet possible to add custom prefixes and suffixes in the defaults or save a favorite. But at least, "inherit" seems to work.





Re: NX 10 - Unecessary spacing in Hole callout

Siemens Phenom Siemens Phenom
Siemens Phenom

You can't see it, but there is actually a space in front of the default suffix and prefix characters for a threaded hole. You can fix this in your Drafting Preferences dialog (so that all new dimensons are created correctly), or the Settings dialog (when you edit an existing dimension).


In either dialog, go to the (Commnon)-->Prefix/Suffix node and in the Hole Callout group do this:

  • Set the Feature option to Threaded Hole.
  • Make sure the Parameter option is set to Pattern Feature Count.
  • In the Suffix option, place your cursor in front of the "X" character and then hit the backspace key to remove the space.
  • Now change the Parameter option to any of the other parameters for which you want to control the spacing and adjust the spaces before and after the Prefix or Suffix character.


You can set preferred characters in your Customer Defaults file, or in your template files, to customize the prefix and suffix characters. Better yet, set up your own Drafting Standard default file, and invoke the standard before you begin a new drawing. This standard file will adjust all of your preferences at one time using the Menu-->Tools-->Drafting Standard command.


Re: NX 10 - Unecessary spacing in Hole callout


Thanks, it works! The callout looks more professional now.

I willl check the customer defaults and drafting standard tomorrow.