Tip to use Simplified Threaded Hole Callouts
SOLIDWORKS has an usual method to control hole callout formats. Most other types of callouts are managed from with SOLIDWORKS settings. However, hole callouts are controlled with an obscure file buried deep within its folder structure on the hard drive. That file is calloutformat.txt (X:\Program files\SOLIDWORKS Corp\SOLIDWORKS\lang\english). Additionally, there is also a calloutformat_2.txt. What’s the difference between these files? Calloutformat.txt is the default file which SolidWorks uses to determine how to form threaded hole callouts created with the Hole Wizard. This file establishes the rules to show both the nominal drill diameter and the thread detail in a leadered note. This is the most common method for threaded hole callouts. However, as mentioned, this method has flaws.
Thankfully, SOLIDWORKS provides an alternative with simplified callouts. The user doesn’t have to go through and modify each and every callout instance in calloutformat.txt. As obscure calloutformat.txt is, one would expect the alternative to be even more obscure; and it is! The alternative file is calloutformat_2.txt, with no identification or in-file description to tell anyone of this fact.
Here’s the tip to use simplified threaded hole callouts. Before SolidWorks is started, launch Windows Explorer and goto X:\Program files\SOLIDWORKS Corp\SOLIDWORKS\lang\english (or similar, depending on SOLIDWORKS installation location). Rename calloutformat.txt to calloutformat_1.txt. Rename calloutformat_2.txt to calloutformat.txt. (Make a backup copy of course.)
The one drawback is that SOLIDWORKS uses different methods to callout the thread between the calloutformat.txt and calloutformat_2.txt. This places a # in front of every threaded hole callout in this simplified format, and leaves off the series designation. The work around for this is to simply open calloutformat_2.txt with Notepad, then use pulldown Edit>Replace to replace “<hw-threadsize> <hw-threadseries>” with “<hw-threaddesc>” in all instances prior to the renaming. (Again, always make backup copies!)
Additional Networking Tip
Once calloutformat_2.txt is modified and renamed to calloutformat.txt, copy it to a network drive location that is available to all other SolidWorks users. On each system, goto pulldown Tools>Options>File Locations>select Hole Wizard Favorites Database. Point the folder to the network location of the new calloutformat.txt. Also point Hole Callout Format File to the same new folder. There are various methods to save this setting for future installs and updates, such as Copy Settings Wizard or Admin Image.
P.S., Cosmetic Threads
One caveat to this whole story is how SOLIDWORKS automatically labels cosmetic thread annotations on ANSI standard drawings. When you create the drawing view that contains the cosmetic thread, you get a surprize; something like “8-32 Machined thread” is added. It doesn’t really conform to any standard, and cannot be edited at the Part level within the cosmetic thread feature (unless you use a customized thread called “None”). This callout can be inserted on drawings of other standards, such as ISO, by right-clicking on the cosmetic thread and selecting “Insert callout”.
If edited manually in the cosmetic thread feature properties, one can enter anything they want, and that will be the callout for the cosmetic thread on the drawing. If you want your threaded holes to say “Stop poking me!”, your hole callout will say “Stop poking me!”. But there is no automated method to use the correct callout without directly entering it within the cosmetic thread’s property field and using a custom thread. One advantage is that if this field is edited, it does automatically update drawing where it appears. However, if I’m relying on Hole Wizard information, I wouldn’t want to use the cosmetic thread annotation callout on my drawing anyway.