Customizing Hole Tables

[wwdaugherty]

Where I work we are creating our own custom hole tables. I am not very familiar with how to do this and have hit a few snags. One of the first basic questions is regarding the callout. I would like to have the 3D annotation to look like ANSI standared for a hole callout. How do you manipulate the carriage return to create a new line under the original one? I also need a memory prompt on how to type in the diameter symbol (phi) using text characters. Since the intoduction of the text symbol palatte, I have forgotten the old techniques for manually entering such characters. Is there a reference handy for creation of text symbols manually?


One of the sticking points is the cosmetic threads. We model all threaded features at the basic diameter. For instance, a .250-20 UNC threaded hole is modeled at a diameter of .250, as is the screw. That is our basic philosopy here. We never intentionally model interferences. Imagine a huge assembly with several hundred fasteners. If you were to do a global interference check,you would have a lot of meaningless info to sort through. Well, I would like to turn off the cosmetic threads globally. I modified our tables to have the tap drill diameter equal the basic diameter. I createdseparate table files for different thread series, so the callouts can accurately reflect thedesired thread.


May I humbly request input from all the lurking hole table experts out there? TIA

 

[looslib]

This is from PTC's knowledgebase:


TPI 104111 for the List of Special Symbols and Their ASCII Equivalents that are used when adding symbols to the notes


We do a lot of sheet metal parts and we create our toolpaths directly from the CAD models. Our holes must be tap-drill size or we scrap parts.

 

[wwdaugherty]

Well, that is the debate in a nutshell. The CNC guys had better realize up front that the feature is intended to be threaded. Like you said, it could create a lot of scrap parts. That is why we are striving to use the PTC hole tables and standard holes, as clunky as they are. The function imbeds the note within the feature itself. And the note callout was what I was getting at earlier. My goal is to get it to appear in the 3D annotation just as it would appear on the drawing. So that is why I was asking about the symbols for diameter, counter sink, etc. I wish that PTC had thought out their philosophy of deliberately modleing interferences when they imagined cosmetic threads. Perhaps there could be a special property which could be applied to either certain parts (threaded fasteners) or features (threaded holes) so that the interferences would be ignored on a global interference check. PTC ARE YOU LISTENING ??? LOL... Thanks for the reply Bill Daugherty

 

[robertib]

A way to make the annotaion correct is to make a text file with the inforamtion in it. This is the basic thread annotation that the holes produce.


&METRIC_SIZE &THREAD_SERIES - &THREAD_CLASS &STD_HOLE_TYPE &VAR_THREAD &THREAD_DEPTH[.2]
&NUMBER_SIZE DRILL ( &DIAMETER[.2] ) &VAR_DEPTH &DRILL_DEPTH[.2]


If you look at the hole tables, the parameters are visible as the top lines of the columns. As long as you have the correct information in the file, you can use the table parameters.


As I understand what you are doing, you have used the thread size (VAR_THREAD)as the basic diameter, and the tap drill size (DIAMETER)as the thread diameter, so reversing the 2 in the above annotation will give the correct callout.


What you will need to do is to highlight the existing annotation and go to properties. There is an option to insert text from file (you will need to delete the existing text), so choose the text file created. You can store symbols in the text file, so you may find it easier to modify the annotation and save it.

 

[j.s.srihari]

i want to have British standard pipe thread in my hole wizard. how to add it please guide