Creo 8 hole table issues...STILL.

[Patriot_1776]

Wow, is it THAT time again?  Seems like this was first talked about back in...what, 2014 or so?  And STILL no fix?  Time to talk about how the notes that come from the hole feature are completely unusable out of the box.  We use decimal callouts for inch threads (i.e. .250-20 UNC-2B) in EXACTLY that format, verbatim.  And, of course, the callout you get gives you garbage that you can't use.  WORSE, and we just found this out, is that the ACTUAL GEOMETRY of the threads where the major diameter runs out to 4 places, are actually ROUNDED, i.e. .3125 gets rounded to .313.  Oh, even better, is the fact that you can't change this.  This, needless to say, is NOT to ASME Y14.6-2001 Paragraph 3.2.1.3 which specifies that these fractional threads like this that run out to 4 places are defined correctly, and that fractional threads that end at 3 digits have the zero as the 4th digit get that zero truncated.  Trying to modify the table file seems to do absolutely nothing.  So, considering that the ASME standards are THE standard for all of this, and they existed LONG before PTC, why, has PTC, in all this time, not actually FIXED this?  Oh wait, we DID get "Bold New Graphics!!!".  Oh, and nice of you to change the names of the hole parameters for no reason other than to FUBAR my cut&paste cheat sheet text file.

I can't even use my cut&paste solution knowing that the actual model dimensions are WRONG and give me ".313" instead of ".3125".  I usually use:

{1:&D#}{2:-}{3:&THREADS_PER_INCH:att_feat[.0]}{4: }{5:&THREAD_SERIES:att_feat}{6:-}{7:&CLASS:att_feat}{8: }{9:THRU} 

Well, PTC, how do YOU, or, worst case, we on my end, actually FIX this mess?

Anyone else have any ideas?  I didn't see any actual solution in any of the older threads, although they've all been closed/locked by the mods like they were actually "solved".  LOL

Serious *facepalm*...

[Patriot_1776]

Anyone?  PTC?  Bueller?  LOL

[TomU]

I'm not seeing this problem in Creo 9.  If I modify a .hol file to include values out to six digits, all of the digits are used in both the hole parameters and the final hole sizes.

Extra digits added for testing:

Hole feature parameters:

The precision is still there, it's just that the display is normally rounded to three decimal places:

Using the standard parameters in the notes with the [.<number of decimal places>] syntax will show more than three decimal places.

While I would need to do additional testing to see if it's possible to have everything default to four decimal places upon creation, it does seem like the precision you need is already available, at least in Creo Parametric 9.0.

[Patriot_1776]

'Sup Tom!  Well, the ASME spec actually says that if the thread runs out to more than 3 (non-zero) decimal places, all the places need to be shown, but if the thread is only 3, then truncate the zeroes after that.  So, depending on the thread, or if it changes, a little manual work might need to be done.

They probably changed it in Creo 9 then, because in Creo 8, I actually measured the major diameter threads and it rounds .3125 to .313, even if I change the .hol file.  I think I looked at one or 2 other threads and found the same thing.  We were on Creo 4 for years before we finally jumped to Creo 8, so, I' ain't holding my breath for Creo 9!

Anyone interested with a solution to the note issue?  We want decimal inch as in:

.164-32 UNC-2B

.190-32 UNF-2B

.250-20 UNC-2B

.3125-18 UNC-2B

With that that exact nomenclature, and having the geometry correct (i.e. .3125 actually IS .3125 instead of rounded to .313).  We would like the standard note that our users "show" to be in this correct nomenclature, and would also reflect the number of holes if it was a pattern.

If some company or person has a solution, post up, and I'll contact you and see about getting you a P.O.

[TomU]

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@Patriot_1776 wrote:

... the ASME spec actually says that if the thread runs out to more than 3 (non-zero) decimal places, all the places need to be shown, but if the thread is only 3, then truncate the zeroes after that.

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I'm aware of this for metric values, but I'm not seeing the same thing for inch values.  From what I'm seeing in ASME Y14.5-2018, metric values must be truncated but inch values do not need to be.

Metric

Inch

Regardless of whether or not trailing zeros are present, the interpretation of limits still applies:

The way the hole feature in Creo is currently implemented, I don't think you will be able to get a different number of decimal places automatically displayed based on fastener size.  While there should be no problem making all of them 3-place, or making all of them 4-place, it would probably take an enhancement to get both (either one) at the same time automatically.

[Patriot_1776]

ASME Y14.6 DOES call out decimal places out to 4 for .3125 etc.  This spec is referenced by Y14.5 for how to call out threads, and so far we're using the 2009 version of Y14.5, and in fact JUST moved to that from the 1994 standard I'm certified in.  I'm going to get re-certified in the 2009 spec this year.

[TomU]

Actually, I take it back.  There is a way.  You can add custom columns to the .hol file and then use those in the hole callouts.

[Patriot_1776]

So, adding "MY_HOLE_SIZE" then creates a parameter?

[TomU]

Correct.  Any additional columns added to the .hol file will be parameters in the hole feature.

[Patriot_1776]

Cool!  Thanks!  Maybe I'll try again then, and just add text as needed.  Weird that every time I changed the .hol file, NOTHING changed.  Something strange is going on.

[Patriot_1776]

Ok, another question:  How does it know what kind of parameter to make?  Does it make a string parameter if there's characters OTHER than numeric, and make an integer or real number parameter is there is only numeric characters?  I guess I could make it work by simply manually typing out exactly what the thread should say instead of using any other (threads_per_inch, etc.) parameters as a combination.

Thanks!

You'd think after all these years they would have fixed this, but noooo.....  We STILL can't see the cosmetic thread without setting the viewing mode to wireframe, and that BUG dates back to Wildfire if I remember!

[TomU]

Lol.  I don't know.  I fought with that as well.  It seems like if only numeric characters (and decimal) are present the parameter is REAL.  If any other characters are present it becomes a STRING.  I'm not sure if there is any other logic to it.  I certainly couldn't find anything documented.  That is precisely why I included TPI in my example column.  🙂

[Patriot_1776]

LOL  *facepalm*  Nice.  Not only do they NOT make it work right, but they do NOT give any indication of how it all works.

Well, thanks for that, I think I may simply then create a string parameter for these that includes the entire callout then.  Gott a think about this.

I'm surprised that someone a lot better than coding than me hasn't come up with a solution after all these years.  I was hoping someone would chime in with "For X dollars our company will make what you want.".  Sigh...

Thanks for your help Tom, and if I find a good solution, I'll e-mail ya!

[Patriot_1776]

Soooo, no solution from PTC for this age old problem?  Here, let me show you my resting surprised face...😲

Ok, so, I guess I have to get with the people here that PURCHASE Creo and get them to get me the contact info for an Application Engineer for THEM to come up with a fix then.  I mean, since we're PAYING for a TON of licenses, might as wel actually have them fix this bug...

[TomU]

Probably the best approach is to show them that it's not currently possible to configure the .hol file in a way that is fully ASME Y14.5 compliant, especially if using metric hole sizes where trailing zeros must be truncated.