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Circle U Symbol

A

Atropos89

New member
I'm trying to define a surface tolerance and need to usea custom symbol. I'm sure many of you are familiar with it - A circle with a capital U in the center. I can create the symbol, but can't add it to my symbols palette. Does anyone know how to add acustom symbol to the symbol palette?


This is what I have right now:
View attachment 5424


This is what I want (I just have a note behind the circle for this picture):
View attachment 5425
Edited by: Atropos89
 
You can create a symbol with symbol gallery and then add it to the symbol palette. I guess you wouldThe other GD&T modifier symbols are special ASCII characters. Don't know if PTC added the U symbol to the list, or where you can find a list.
 
Yes, I have created the symbol. There isn't one by default in the Creo from what i can tell. But how do I add it to the palette? I can see no way of editing the content of the palette or any other way of using a custom symbol in a Note (or other text box).
 
You can add a symbol to a note with the code &sym(symbol_name). I was not able to get it to work in a feature control frame.


Searching through PTC online I found that Pro-E stores some of the text symbols in a file called special.src. It's in /text/usascii. I opened it up in notepad and i can see that there is mention of a "profile gtol 'Unequal' symbol", but the document is mostly unreadble code.
 
Root Profile is a callout for the thread shape on a screw. It details things like thread root land and the radius between the root land and the sides of the adjoining threads. Basically, the root profile is whatever shape you use with a helical sweep to make your screw.


I found the special.src file, and it does mention this symbol. I'm guessing the list of numbers is a set of coordinates for the sketch. There's got to be a way to use this in Creo.
 
Open your symbol drawing (find in your config.pro "symbol_instance_palette_file") and create the symbol there then save, it is now part of your symbol pallete.
 
Assuming it's the same as WF5 there is also a drawing option gtol_display_style you need to set to asme_y1441 for it to show correctly on a drawing. It appears they haven't updated to the 2009 standard.
 
Atropos86:


Ok. I was not thinking "thread". I assume this could also be used for gear profiles as well?
 
@Roger: I don't have any experience with gears, but I imagine this could be used for gear profiles too.


@kdem: I have the ASME Y14.41 box checked, but still can't get the unequal symbol to show up.It seems as though gtol_display_style is not a config option for Creo. All my searches online end in this thread!





View attachment 5471
 
Are you looking in the config.pro or the drawing options? The gtol_display_style is a drawing option. Looking at the documentation for Creo they still have it listed.
 
Ah, got it. I've gotten used to working with modeling questions, so sometimes I forget there is a separate drawing config! gtol_display_style was my problem. Thanks for the help!
 
In searching for this, I am left with the feeling someone is pulling our collective leg. Profile is profile. You can have your tolerance symetrical above and below the line, all above the line, or all below the line. But, to say that a thread root would have a different callout is not quite adding up.
 
Sorry, I didn't explain the application very well. Thisscrew has a varying thread pitch and a varying root land width.This calloutshould be just specifying a non-symmetrical tolerance. Just like saying a hole is .5 , +.05, -0.00 for its diameter, this is saying that thewidth of the root can vary a certain amount bigger, but a different amount smaller. It's a failry complex screw.
 
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