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Problem with hole callout

Valued Contributor
Valued Contributor

I cant create the dimension of one of the threaded holes using hole callout. What am I doing wrong?

9 REPLIES

Re: Problem with hole callout

Legend
Legend

Hi @Javiduc,

hole callout has lot limitations on NX 11 / 12. Try to use 'Feature Parameter' command.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: Problem with hole callout

Valued Contributor
Valued Contributor

Have you achieved to place the dimension with feature parameter in the part attached? I cant, for me, it only shows the diameter but not the thread size.

Re: Problem with hole callout

Legend
Legend

Hi @Javiduc,

in your case I don't have problem using 'Hole callout'.

Done with NX 11.0.2 MP2Done with NX 11.0.2 MP2

Thank you...

Using NX 11 / RuleDesigner PDM

Re: Problem with hole callout

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @Javiduc,

 

I suspect it has something to do with dimensioning an inch thread in a millimeter part file.  If I convert the unit of the part to inch (using the ug_convert_part utility) I have no problem using the 'Feature Parameters' command to insert the callouts (using the ansi template), otherwise, like you I only see the diameter values.  Here's the result having converted the unit:

Screenshot - 9_29_2017 , 8_55_08 AM.png

 

 

I am also able to add the callouts using the Radial Dimension command, with the Method set to "Hole Callout" (without having to change the unit of the file):

 

Screenshot - 9_29_2017 , 8_52_45 AM.png

Files attached.

Regards, Ben

Re: Problem with hole callout

Phenom
Phenom

@BenBroad

NX hole callout is unreliable. It hast its own moments. Sometimes it works and the next moment it’s not. (Even with fully loaded components). 

Our VAR also confirmed this absurd behaviour. Since this is not a reproducible with an example, we are unable to report it to GTAC.

https://community.plm.automation.siemens.com/t5/NX-Design-Forum/Hole-callout-limitation/td-p/421696

 

"Feature Parameters" supposed to be retired soon, but I don't think that you could let it go for good.

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: Problem with hole callout

Phenom
Phenom

Per Sam Bilke at GTAC, on 12/02/2016, when I asked about one of my thread callout ER's:

 

"I've talked with the Developer on ER 7776177. There are currently plans to put this enhancement into a near future release. Additionally, there is currently no retirement release set for Feature Parameters. This tool will not be enhanced, but it will at least remain available for use until a retirement release is set. It seems to be almost certain that the fix for the issue will be implemented before Feature Parameters is retired, thus you should have a workaround until the issue is fixed."

-Dave
NX 11 | Teamcenter 11 | Windows 8.1

Re: Problem with hole callout

Valued Contributor
Valued Contributor

It worked with radial dimension, thank you @BenBroad!

 

I dont understand why it worked with radial dimension but not with lineal dimension as I guess hole callout method should work similar in both commands. Anyway the important thing it that it can be done. Just I hope this problem and other with hole callouts (like not working for promoted bodies or for holes made on cylindrical surfaces)  will be solved soon.

Re: Problem with hole callout

Valued Contributor
Valued Contributor

Hole callout has many issues:

PR 8814089, ER 8830466 , ER  8830471

 

All of which Siemen's is aware of, yet they still insist on not upgrading Feature Parameters!!!!!!!

Not sure of their thought process, but they are shooting themselves in the foot.

 

Hole callout does not work well on Legacy Parts!!!!! It seems as if Siemen's expects users to never clone parts and to always start parts from scratch.

 

That is the only reason for most upgrades that I have seen do not support Legacy Part usage.

 

 

Re: Problem with hole callout

Phenom
Phenom

 

NX got Radial Hole callout development focusing their new hole command.

At the same time NX PDW/MW add-in programmes are developing their own extensive Reuse tool library parallelly to created holes and pockets (Tool subtraction method). This tool library is using mostly outdated NX commands to create its components.

New NX Radial Hole callout not supporting well the holes created by new PDW/MW which utilised old methods in its library components. It’s pathetic to see that NX development resources are not streamlined and updated accordingly with new NX native developments. I’m surprised to see Siemens, a renowned German company is allowing this. (my technical education is based on German standards and know how thorough and well defined it is.)

So as users, when dimensioning holes, first we must find out with what method the holes were created in the models to decide which dimensioning method to apply in the drawing. Also there are different appearances between the Hole Callout and Feature Parameters methods too. So, if the models have used a hybrid method, in the same drawing there are different appearances which make the drawing a quite awkward and messy.

Some of my ERs:

mf_er_20171002.JPGmf_er_20171002_02.JPG

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW