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tapped hole parameters


tapped hole parameters

How do I add to the parameters that Creo 2 assigns to a tapped hole?

I want to add screw_size or ( feature_id from the *.hol file)

then I can add screw size or feature_id to the tree column so I know what size the feature is. Creo now calls all tapped holes (hole in the model tree)

I want this added automaticly, the same way some of these are added now





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You can add parameters to the feature. You can add relations referencing the feature parameters. You can format notes using relations.

Holes are holes... and you can rename the feature type (with limitations) in the tree.

...but automatic? Sorry, this is PTC were talking about.

I am no expert on the .hol files and really don't like messing with them.

the *.hole files have the parameters I am looking to use. Not all of these parameters are listed in a tapped hole.

when you left click on a tapped hole in the model tree and right click parameterss one can see the parameters list for the feature. I am trying to figure out how to add another parameter to this list via paramters listed in the *.hole file.

I want the screw_size or the fastener_id parameter from the hole file so I can add a column to my tree to read this.

then in the tree I would see the 1/4-20 parameter if it was a 1/4-20 tapped hole.

I am trying to get away from labeling the holes in the tree.

I was able to get this to work on my system. I went into the model tree columns display options dialog box. In the type drop down box I selected Feat Params. In the name edit box I typed SCREW_SIZE and clicked on the >> button to add it as a column. For any tapped hole I add it shows what size screw it is for.

Of course, this probably depends on how your .hol file is set up and what you call the parameters for the hole features. Is this what you wanted to achieve?

I have tried this, I get no results in the tree. I have an unaltered *.hol file

YES what you are doing is what I am trying to do.

Is it making the column and just not populating it? Not to sound patronizing, but have you dragged the tree out far enought to the right to view the newly added columns?

Edit: I'm running Pro/E 5.0 M120

very GOOD POINT, I can move the shade all the way across, no results

the items I can get in the tree are the parameters listed in a tapped hole when you query the parameters of the hole.

Antonius has shown an example

I am on wild fire 4.0 and Creo 2.0 M30

Lonny, that is what I am finding too. The parameters for the "note" are different from the parameters in the hole "feature"... and are different form the fields in the ".hol" file. Really confusing.

I know we have discussed this before when it came to formatting the holes on drawings. It is still very convoluted in my mind.

I am trying to get an answer from PTC.

oops, Yes Kyle if I ADD the parameter the way you did I get the same results.

I miss typed my previous answer

I do not want to be adding this on my own.

I tried changing feature_id in the *.hol file to screw_size, NO GO

I tried lying to one of the values for drill_ depth, NO GO

That worked for me, Kyle. I too use default hole charts.

Something magic happens between the hole parameters and the hole note. It has something to do with the default thread note format (callout_format). I tried using FASTENER_ID and it failed. Does anyone know where to find the following relations and how they are derived?












No idea, but I want to know how to predefine a depth of a hole for example. That would be a huge time saver.

By default the standart hole depth is set to 3 times hole diameter, and that's way too deep in most cases.

True, and also the hole depth vs the tap depth. By default, the hole depth is 1.25 of the thread depth but that is easily over-written and is essentially lost upon editing the thread depth.

So yes, something in the hole algorithm is creating a lot of data based on the .hol files. We really should have access to these assumptions.

As a general rule, threaded holes require a minimum of 3x-pitch of complete threads after taking into account the lead-in chamfer/deburr cut. Bottoming taps require a finite depth beyond this. A "real" hole feature would let you check these parameters in an intelligent way. The most tedious to find is the bottoming tap requirement; the depth from the end of the end of the last full thread to either the drill point or the full diameter of the pilot hole.

A part of the hole dialog that checks to manufacturer's conformity would be extremely useful.

Pro/E offers many different ways to customize the model tree. There is a plethora of information that you can add, so this might fit your need. Crane Aerospace and Electronics has a PDF of a presentation of how to customize the model tree, which can be found via a google search.

I'm not sure if you can include hole information, but it's worth looking into.

Thanks Domingo. That helps some. Still a few missing expanations. In Creo 2 you see there are variables for the depth symbol rather than the CTRL codes. Also "TAP" is assigned to a variable not in the hole tables (STD_HOLE_TYPE). The fact that you cannot find these anywhere in parameters or relations is strange and frustrating.

The attached files are from the help docs. One lists all the variables (okay, most all) for hole files and Callout_Format and the second talks about default callout formats in a table format. I've looked for that table but it doesn't seem to exist for editing.

CREO 2.0 M30

I placed a 3/8-16 tapped hole in a plate and I queried the parameters of the hole.

I see the hole has a parameter SCREW_SIZE,

I do not see this parameter in the unc.hole file and I have no idea where Creo is getting the parameters for this 3/8 tapped hole.

I can however add a column to my tree and with a screw_size parameter I can now see what the hole is in the tree.

I can live with this solution in CREO. The screw_size parameter is not available in WF4

True... I too am still trying to figure out where the "hidden" parameters are generated and maintained.

The only logic I can build on this is that the when you create the hole, it uses the hole tables to generate some hidden parameters based on certain elements within hole feature and subsequently assign pattern information "just in case" a pattern is subsequently assigned.

Somehow, I suspect the parameters belong to the note feature itself and therefore do not list when you query the hole feature. It seems you cannot do a parameter query the note sub-feature of the hole. Therefore, the most we will know is what the help pages tell us about the available feature, which can, oddly, be used for such things as generating hole notes and structure model tree columns. I'd say these hole notes require a little more transparency.

I guess &SCREW_SIZE comes from FASTENER_ID from the *.hol file. It's just a naming convention that is different for some reason there. There might simply be some sort of hidden script file in the installdir that does this conversion from used *.hol files.

These *.hol files and their connection to standart holes inside Pro/E propably went through some changes in WF5 or later. The devs propably wanted to keep the *.hol files in the same format, so they are usable in all the Pro/E versions, and maybe that's why they use this said additional hidden file for the conversion in between Creo and *.hol files.

I think some additional transparency would be great. I've always thought that the .hol files were 50% formatting and 50% black magic. It now seems worse since PTC has wanted to change the way hole features and their parameters interact, while trying to keep the .hol formatting the same.I can understand them wanting to keep the formatting the same for legacy users, but in this case it seems to be doing more harm than good. In my opinion I think it would have been fine to change the formatting, as long as they clearly documented the change.

I think the default hole callout format is absolutely atrocious. I've wanted (for a long while now) to create new hole callout formats that are specific to each type of hole. Having a different callout feature for countersunk holes, tapped holes, and even different notes for blind and through holes. It would make my life a bit easier when making drawings. Doing so will require me to dig into the .hol files, something that I have been avoiding. My end goal of having dynamic callout features might require some inelegance within the .hol file itself, something I'm not even sure is possible. Either way this thread has motivated me to give it a shot, wish me luck.

Good luck, Kyle!


You can do different notes based on the type of hole. At the bottom of the .hol file add information on the hole, with the callout format for that type of hole. Basically you build a matrix showing the possible hole variants and the note for each variant. An example is below:




I will give you a starter UNF / UNC file with modified callouts if you would like.



This is exactly what I am looking to achieve; type of hole specific notes. I'm assuming that I uniquely name the callout format under the CALLOUT_FORMAT column, and refer to that unique name when specifying the formatting of that specific note? A started file would save me a ton of time otherwise spent experimenting.

Thanks for the info and help!


Ahhhh.... I was zigging when I should have been zagging. I put the formatting text under the CALLOUT_FORMAT column, not an unique name (face palm)

Kyle, that is what that linked file is above formatting_thread_notes... from the help files. It is just not clear to me what format this file has to be and where it has to be. If you get this to work, please consider posting your file and solution here.

Good Luck Kyle.

I was using notepad++ to edit the *.hole files. I am working on the creation of a dowel.hol file for dowel pins, thru/blind.

I have yet to figure out where the magic between the *.hol file and the Creo dashboard occurs

Several months ago I've also tried the make the *.hol files work for me the way you guys describe.

The attached is a *.hol file I've started from. It's easily editable in notepad, not that well in wordpad.

I got stuck with the problem I couldn't get depth of a countersink into hole note other ways than using relations, which seemed too tedious. So that's why I gave up on the DEFAULT_CALLOUT_FORMAT_DATA as a whole. Just using the THREAD_DATA table to be able to define holes faster, and not bothering with hole notes anymore.

Good luck.

Take a look at the attached hole files. They will at least be a starting point for you.

That is -very- helpful, Bill. Thank you!

Antonius, I was having some interesting issues opening the XPS documentation you attached earlier that mirrored the info the Bill included. I'm bummed I didn't see the DEFAULT_CALLOUT_FORMAT_DATA table documentation earlier!

I was able to get the new .hol files modified and working. I ended up adding every possible combination of standard hole states that is listed in the documentation. In the CALLOUT_FORMAT column I added the string "Empty CALLOUT_FORMAT entry in myUNC.hol file" for every entry in the table. This way I already have most of the infrastructure of the file in place. If I'm making a hole and I see the "Empty CALLOUT_FORMAT ..." string as the hole note, I can quickly add the formatting text in the hole file. This way, I will slowly populate the callout formatting for all of the holes over time. If anyone wants the .txt file with all of the possibilities already typed out let me know (it was not a pleasant experience).

Thanks again for the info and files Bill, they were a huge help. I can't tell you how long I have wanted to make unique hole notes for the different types of holes. This will save me massive amounts of time when making drawings.

-very- clever

I will have to find a better format. I thought XPS was pretty much universal for windows.

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