I can't found information about the option DEFAULT_CALLOUT_FORMAT_DATA.
You can place this option in your *.hol file and then you can define different CALLOUT_FORMAT for different hole types.
Here is a short example:
This is a very nice functionality. But I cant find this option in the PTC documentation. Is this a hidden option?
This seems like a really nice option, have you tried it?
If yes on which version of proe have you done so?
At the moment I've got a set of standard note which I keep changing for every different type of hole very labor intensive and prone to human error.
I look forward to learn more about this.
yes I have tried this option. It works well in WF4 and WF5. I haven't tried this for lower versions of Pro/ENGINEER.
Attached you find a example. There are 52 different hole types defined in this file. I only have used a consecutive number at the moment. But you can try it with this file and then place the note you need in the column CALLOUT_FORMAT.
I haven't found any documentation about this feature - and it is in deed a really nice feature. So I don't know if this also is supported for newer releases of Pro/ENGINEER.
Thank you for this. I've been trying to figure this out for a couple of weeks. The closest I got was creating separate files for tapped, counterbored and countersinked.
don't mention it. As soon as I get information from PTC I will post it in our group B&W Software.
Has anyone found more information or documenation regarding this feature? I can't find any mention of it in any of the PTC documenation.
I have opened a call for this (C07955386) at PTC. But but without any success. I still wait for information about this.
DEFAULT_CALLOUT_FORMAT_DATA is a very nice feature. But I also can't find any information about this. As soon as I get information I will post it in our group (B&W Software).
you are right. This is a very nice feature. But you don't get any support information about this from PTC. So I'am not sure if we should use this or not. For now it works very well. But what is with newer versions of Pro/ENGINEER or Creo Elements/PRO?
As soon as I have news I will post it here or in our group.
today I received an email with a PDF from PTC support.
In this PDF you find detailed information about the option DEFAULT_CALLOUT_FORMAT_DATA.
So I think we now can use this functionality.
in future you can define different hole notes for different hole types.
Just add the DEFAULT_CALLOUT_FORMAT_DATA to the end of your *.hol file.
You define the CALLOUT_FORMAT for each type of hole in a column of the table.
I attached an example for you.
Just copy it to your computer and set the Pro/E option "hole_parameter_file_path" to this directory. Then place a new hole and you will see how it works.
If you still have problems please let me know.
thank you for all these explanations
but I do not understand the impact of changes on the notes (for exemple for a M30 the nte is m30 that'all)
in the last column of the DEFAULT_CALLOUT_FORMAT_DATA table you find CALLOUT_FORMAT
Here you can define the note text for each hole type.
I just placed the &Screw_Size folowed by a consecutive number.
Please do the following.
Open a part and place a new hole.
Select the thread series A_DIN13-1.
Then open the dashboard register "Note"
You now see the note "M10" for example. If you now add a counterbore the note will change to "M10 2".
If you remove the thread you will get the note "M10 22" and so on.
With DEFAULT_CALLOUT_FORMAT_DATA you will be able to place different hole notes for different hole types.
ok i find the probleme. You have to define hole_parameter_file_path anyway if the default folder (hole)...
I will work of the link between the ligne et size
Thank's a lot
Actually where DEFAULT_CALLOUT_FORMAT_DATA is located at. I am not able to find its location to edit it.
Can you help me out for sorting out this problem
Siva Vinil Krishna .K
the DEFAULT_CALLOUT_FORMAT_DATA is located at the end of the *.hol file.
Find an example here:
I did try to place the A_DIN13-1 in the model and it was sucessful but still i am not able to edit note as i needed because i am not able find the link of getting into hole chart and edit CALLOUT_FORMAT_DATA. I have read the document about the formatting table which u have shared in earlier discussions but I am missing the loop of getting into the hole chart.Can you kindly help me to sort this problem.
Siva Vinil Krishna .K
you find the CALLOUT_FORMAT_DATA at the end of the file A_DIN13-1.hol.
There you can edit the note for each possible type of hole.
Kindly help me out how to open the A_DIN13-1.hol. file. IS that is opened in the notepad and then edited because this is first time i am listening about .hol files. This can also be one of the reason i a not able to find CALLOUT_FORMAT_DATA
Siva Vinil Krishna .K
I added your "A_DIN13-1.hol" file to my hole directory, but it does not show up in my drop-down menu when I go to insert a new hole.
I closed and reopend ProE 5.0 before doing this, but it still does not show up as a kind of .hol file I can use.
Do you have any ideas of what I need to do to be able to see your ".hol" file options?
the hole file seems to be ok.
Not sure why you can't select it.
I need additional information:
1. Which Creo/ProE version are you working with?
2. Move the ISO to another folder - can you still see the ISO in your pulldown?
3. Do you use the Creo option "hole_parameter_file_path"?
Thanks for replying so quickly, Oliver!
To answer your questions,
1. Creo Elements/Pro 5.0
2. Yes I can still see it (strangely enough). I moved my ISO_SES.hol file to another location, but it still shows up in the pulldown.
3. Yes (see attached screenshot. I think it proves that I am using the Creo option correctly)
I think you add my hole file on the wrong location.
Have you copied it to the Creo directory or to the "hole_parameter_file_path" directory?
If you remove a hole file and it is still visible, then something is strange.
Another important thing is the name of the THREAD_SERIES. I think the name has to be unique. So if you try to add "ISO" twice I think only one will be shown (but not sure about this).
I copied the file to the "hole_parameter_file_path" directory (see attached). Is this the correct thing to do?
I am not sure what my "Creo" directory is.
first you have to make sure that you change the hole files in the correct location.
Remove a file from the hole_parameter_file_path_location which you do not have in the Creo hole directory.
You will find the Creo holes in the directory <CREO>\text\hole
There you will find this files:
After removing the file restart Creo and check if it is really not available.
Then we will go on.
Thank you Oliver.
I can now see changes in Creo caused by me removing files from my hole_parameter_file_path_location. It seems like I have to move the file out of the location, and then back in in order for the change to register.
I can now see your A_DIN13 holes from my Creo dropdown menu.
This solves my main problem. I will keep playing with the settings now (according to your previous instructions), and see if I cannot get the hole notes how I want them.
Thank you very much for bringing this to my attention.
I have been waiting for this since they revamped the hole tool several releases back. I spent a considerable amount of time in the past trying to get something to work. The users would end up importing a standard note from text file after the hole was created and wait till the note was shown on the drawing to fix the total quantity.
The set-up of this is still a little hokey but it seems to work. Modifying text files in some location specified by a config.pro option is so archaic. Maybe Creo will have a single centralized GUI interface with plenty of explanatory images and previews for managing all of your settings and modeling and drafting standards.
You still can't modify notes while you are creating the hole.
The quantity still needs some work.
Does anyone know if there is a way to edit the thread note call out for a cosmetic thread? editing the ISO.hol file seems to only update the formatting for notes made thought the hole tool.