cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

changing tapped hole specifications

ptc-5493477
1-Newbie

changing tapped hole specifications

When adding a tapped hole using the hole feature, a note is added which specifies the tap drill size. How can I change the behavior to not place this info? Is there a table that could be edited that I'm missing? I see that I can edit the note on the drawing, but what a pain to do this. And if someone places a tapped hole and forgets to edit the note, chaos will ensue.

Thanks!


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.
1 ACCEPTED SOLUTION

Accepted Solutions

Yes there are multiple tables you can change to get the note you want out of the box. First set the config.pro (or.sup) option hole_parameter_file_path to the directory where you place your .hol files. You will need a .hol for each thread series, UNC UNF NPT for example.

Change the notes in these to the format you want. I have attached a UNC file with a good variety of notes to get you started.

View solution in original post

9 REPLIES 9

Oh, Jim... are you in for a treat

Hole tables manage these notes and people have invested vast resources to tweak them to their liking only to find another engineer that wants something -slightly- different.

We have had extensive discussions on the subject and not one is a simple answer... well may one.

My recommendation is to forget the built-in functionality and just make the note on the fly. If you have absolute standards and a person assigned to making sure those standards are met, they need to learn how to manage hole tables. In my world... the day is simply not long enough to justify it.

You can choose for the hole feature to not generate the note. By default it does. Third tab over in hole creation; uncheck "add a note".

Yes there are multiple tables you can change to get the note you want out of the box. First set the config.pro (or.sup) option hole_parameter_file_path to the directory where you place your .hol files. You will need a .hol for each thread series, UNC UNF NPT for example.

Change the notes in these to the format you want. I have attached a UNC file with a good variety of notes to get you started.

View solution in original post

Bill, your examples are very helpful. I have another question: Is there any way to suppress the automatic space after the parameter? I.e, the "&PATTERN_NO X" gives me a "3 X " in the note (3spaceXspace). What I really want is "3X " (3X space).

Thanks again.

This has been a long time discussion about PTC not using their "best effort" in making these tables. I have a similar issue with UNC - 2 B... which should be UNC-2B.

If you bracket the characters with {0:&variable}MORE TEXT, you can remove the space delimiter. the problem is that the variables simply do not know where the variable name ends and the resumption of characters resumes. the string -does- know this when using the &... for the next variable.

Thank you Antonius. This is very good!

edit - snippy comment removed -

you can turn off the note during creation of hole.

Thank you all for your speedy and generous replies! I had almost given up on this forum, but now see the value.

I understand the note can be turned off.

I don't want to do that.

I also don't want to manually enter all the data that I want to see on the drawing. That leads to inconsistency and errors.

As others have pointed out - this _IS_ supposed to be parametric and while I don't want to get up onto the 'why does PTC/Creo behave in such a monstrous manner' soap box, I will say that in every single cad package I've ever used for the past 20 odd years (and there are lots of them), this was an easy and simple thing to do.

Thanks again for the example files, I'm sure I can make something which will work as we need.

I commend your vigilence for consistency, Jim. I hope you will continue to participate in the forum.

Announcements