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changing default note format ...

RobertSchaefer
1-Visitor

changing default note format ...

I'm a long time pro/E user new to Wildfire 4 and I need some quick help. Can anyone here tell me how to change the default format for the tapped hole text? I don't mean just edit the text format for individual tapped holes, I know how to do that. I mean change the default format so all future tapped holes created on any part in any directory will be to my liking when I create them. Best to all, Robert 3D Accuracy www.3d-accuracy.com
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10 REPLIES 10

Robert I think you asking about changing the information that is provided in the hole notes, correct? If this is the case you can edit the .hol tables located in under the text directory hole folder for your Pro-E installation location. You can edit the hole tables with a text with notepad or wordpad. You can also create you own hole tables using the standard Pro-E ones as a reference. You will need to add the new file location to the config.pro (hole_parameter_file_path)if it is located in another directory than the default one. Regards Eric

Hi Eric, Thank you for your response. Actually you answered what was going to be my next question, perhaps you're a little psychic. That was excellent information you provided and I will definitely make use of it. Let me reword my original question and see if I can't make it more clear. When you create a standard tapped hole using the hole dashboard in Wildfire 4 it will create a text note on the model with a default format for the text. If you select the note from the model tree, right click on it and select "properties" it will open the dialog box where you can edit the standard text. The default format (this I want to change) for the text note shown in the dialog box is this: &METRIC_SIZE &THREAD_SERIES - &THREAD_CLASS &STD_HOLE_TYPE &VAR_THREAD &THREAD_DEPTH &NUMBER_SIZE DRILL ( &DIAMETER ) &VAR_DEPTH &DRILL_DEPTH -( &PATTERN_NO ) HOLE which creates a note on the model and associated drawing that looks like this: 1/2-13 UNC - 2B TAP (a downward arrow depth symbol) 1.000 27/64 DRILL (0.422) (a downward arrow depth symbol) 1.250 -( 1 ) HOLE I want to change the default format so all the tapped hole notes read differently when I create the tapped hole and not have to edit each text note individually which can be done but is way too time consuming. There are two things I would like to change: 1) I'd like the drill and tap depth to be a two place dimension instead of a three place in this application only and not affect other decimal place settings for other things ... and 2) I want to re-arrange the default text so the tapped hole text note reads differently. Surely there must be a default text file or config option that controls the default text format for a tapped hole, this is what I'm looking to change. I hope that makes my question more clear. Best to all, Robert 3D Accuracy www.3d-accuracy.com

You change the format of the note by adding parameters to the CALLOUT_FORMAT line in the *.hol file. Files are located in the loadpoint\text\hole directory. You can add the column names to the line by preceding each parameter with the & symbol. (ex. &FASTENER_ID). To format a value to two decimal place add [.2] at the end of the parameter. Adding <CTRL-a>x<CTRL-b> will give the depth symbol. Change the letter x to something else to get a different symbol. You could also try creating a note in ProE to get the symbols and copy and paste them into the CALLOUT_FORMAT line. Copying and pasting the plus/minus symbol gives $. The same symbol is given with <CTRL-a>$<CTRL-b>.

Hi Kevin, Thanks for your post. I checked the .hol file you're talking about, found the CALLOUT_FORMAT line but it's blank. I was expecting to find this: &METRIC_SIZE &THREAD_SERIES - &THREAD_CLASS &STD_HOLE_TYPE &VAR_THREAD &THREAD_DEPTH &NUMBER_SIZE DRILL ( &DIAMETER ) &VAR_DEPTH &DRILL_DEPTH -( &PATTERN_NO ) HOLE which drives the actual text note on the model. I tried typing in the parameters I want behind the CALLOUT_FORMAT line like you suggested and it worked. However, I have one problem that I can't seem to find a solution for. The text note on the model is all on one long line instead of three lines like I typed it. I tried double spacing the parameters and it still ends up on one long text line. I'm ending up with a note that looks like this: xxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxxx what I want is this: xxxxxxxxxxxx xxxxxxxxxxxx xxx Is there a key stroke input that I can place between the parameters where I want it to start a new line? Any thoughts? Thanks for your help, Robert 3D Accuracy www.3d-accuracy.com

The other values are system parameters, you can use those if you prefer. To get seperate lines place a forward slash (/) where you want line breaks.

Thanks Kevin, that did the trick, everythings exactly like I want it now. I did use the system parameters because I have mapkeys set up to automatically swap any size tapped hole on the fly including going from a blind depth hole to a thru hole and vice-versa. Using the system parameters keeps the note text reading correctly. Have a good evening! Robert 3D Accuracy www.3d-accuracy.com

Kevin,

Could you share your mdified *.hol file ?

I have the same problem with Robert but still cannot solve it.

Thanks in advance,

Peearpong

Here is a modified ISO.hol file for Creo Elements/Pro 5. The / is used for line breaks. Look under the Help Center in Part Modeling>Engineering Features>Hole for the sections on Using Hole Charts and Formatting Thread Notes. These sections can help with the CALLOUT_FORMAT.

Hi Kevin,

Thank yo so mch for your help I will try it and let you know.

Peerapong

Robert,

Could you share sample *.hol file to me?

I'm interesting in the same experience you have.

Thanks in advance,

Peerapong

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