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Hi,
I am using Creo Parametric 10.0.4
I've created a hole table in my creo drawing and I want to modify the parameters in the hole table. For example, in the picture, the fourth column is the description of the hole and it currently reads 'M5x.8 ISO' instead of this I want it to read 'M5 x.8 Tap THRU'
Any ideas on how I can make this change.
Not exactly easy (to do or to explain), but you can use "standard holes" driven by custom .HOL tables.
Add a column "MY_DESCRIPTION" to the custom .HOL table and then display this "MY_DESCRIPTION" parameter in the drawing hole table.
Please read through the documentation "Using Hole Charts" and "About Hole Tables" before asking follow up questions.
ou can modify the hole table parameters in Creo Parametric 10.0.4 by following these steps:
Double-click the hole table in your drawing to open the Hole Table Editor.
Select the column containing the description you want to change. In this case, it's the fourth column.
Right-click on the column header and select "Edit Column Properties".
In the "Column Properties" dialog box:
In the "Hole Table Description Format" dialog box:
Click "OK" in all the dialog boxes to close them.
The hole table will now update with the new description format.
Important notes:
By following these steps, you can easily modify the parameters in your hole table and customize the description format according to your needs.
I think the best way is to use custom hole table.
Any text that you see with the hole feature is defined in a .hol file.
The contents of a .hol file looks like this, and you can open .hol file in any txt editor.
So, if you find the .hol file you are using and change ISO to Tap THRU, then restart Creo, you will see Tap THRU appear in your hole table instead of ISO.
If you do not always want Tap THRU, but other text depend on your design, you can create multiple .hol files, and choose to create holes from those file.
Multiple holes in the same .prt file can be defined from different .hol files. For examples, I have multiple .hol files and can choose from this dropdown menu each time I create a hole:
To find the folder of your .hol files, find this configuration option.
hole_parameter_file_path
If you do not see that option, then the files are in default folder.
Thank you for the response.
I've updated the ISO.hol file. The hole description has successfully changed (see snap-1 & snap-2). but the description in the hole table hasn't changed (see snap-3). I've of course deleted and recreated the table a few times to ensure it's updated with the changes made in the .hol file.
Sorry for replying late.
The default ϕ column is from .hol table, but it is not the hole note.
In the image above, the text M4 ISO_ is from ID and Series in .hol file
Although in the hole table, your note will not show, you can add parameters to show hole depth, boring diameter, thread depth, boring depth, etc.
You can control how the parameters appear in the table by editing "Name" column in the Hole Table window shown above.
The list of parameters can be found here.
https://support.ptc.com/help/creo/creo_pma/r11.0/usascii/index.html#page/part_modeling/part_modeling/Standard_Hole_Parameters.html
So instead of showing "M5 Thru" it is possible to show M5 <thread series> in a column and "Thru" in another column (indicating depth).
I haven't done it yet but maybe you can add your own parameter, as described in this answer
Re: Modify Parameters in na Hole Table - PTC Community
Hi @Anantj18,
I wanted to follow up with you on your post to see if your question has been answered.
If so, please mark the appropriate reply as the Accepted Solution.
Of course, if you have more to share on your issue, please let the Community know so that we can continue to help you.
Thanks,
Anurag