You might not be getting a response to your question because this
isn't a common practice. I also wouldn't say that calling out the bit
size is "expected". Normally, process specific notes are not added to
the drawing (unless you are making a process drawing). Calling out
the bit instead of the actual hole size is reference to the process.
It also removes your ability to tolerance the hole as you are not
longer calling out an actual diameter. With that said, I don't
believe theres an automatic way to have SW call out the hole by it's
bit size. There may be a look up table that is used by SW to name the
hole features in the model mode. I'm not sure where that would be
Co-moderator of http://tech.groups.yahoo.com/group/solidworks
Thank you for the reply, I was making an 'in house' drawing and a couple
of our machinists are rather old-school, ie don't quite grasp ansi
standards/symbols. I had assumed that since a letter size drilled hole
was available in the Hole Wizard I would be able to retrieve the hole
size in the Hole Callout...
Change the Dimension Text over in the Dimension Properties, on the
left, from <hw-diam> to <hw-fstsze>. Down in the lower left corner of
the Dimension Text box is a button called Variables, click on that and
you can see all the potential system variables that you can use on
your dimension text.
If you want all your hole callouts to show the <hw-fstsze> you can
modify the calloutformat.txt file found in
C:\Program Files\SolidWorks\lang\english. Be sure to back-up before
modifying. Also, if all your users need access to these standards,
copy the file out to the network and set a path under System Options >
File Locations > Hole Callout Format File.
I will usually change this callout on an as needed basis on the shop
drawings we create for our guys. Sometimes the drill size is good
enough for size and tolerance.
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