Customising the thread tables in NX 8.5 1

[PrintScaffold]

Greetings all!

I would like to customise the thread lookup table (tables?) in order to include thread standards and diameters/pitches which are relevant to our tasks and get rid of those which aren't. But so far I failed to understand which tables should I edit and where do they reside. I tried reading NX help, but I have suspicion they information there is not up do date. It well may be of course that I'm simply having a strange bout of thickness. Anyway, could you please provide me with some guidance on the matter? I'm interested in both Thread and Threaded hole tools.

 

[JohnRBaker]

OK, you can find the 'Threaded-Hole' data at...

...\UGII\modeling_standards\nx502_Threaded_Hole_Standard.xml

...and the data files for the simple 'Thread' feature at...

...\UGII\thd_english.dat

...and...

...\UGII\thd_metric.dat


John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.

 

[PrintScaffold]

Thank you very much, John! I now see what I got wrong.

And while we are at it, could you please explain me couple more things about threads, which I not fully understand but failed so far to get round to sorting them out.

1. I'm not fully getting the meaning of the 'Shaft size' option in the Thread tool. If my design is driven by the sketch and feature (as opposed to using the cylinder primitive), Shaft size option creates sort of a circularity - if I leave the default value, I get the error notification 'Cylindrical face diameter is in conflict with thread definition'. If I want to make it equal to the defaul value in the thread table, I need to know it before the application of thread. Also, it's not a common practice to design to the exact values of the thread shafts, because normally parts are designed to nominal dimensions. What am I not getting here and how this option is supposed to be used?

2. In NX own help, there is an advice: 'When creating a thread on a chamfered hole or boss, the chamfer feature should be created before the thread feature. To ensure the proper display of the thread, edit the thread length to include the offset of the chamfer.' I must admit, I'm not fully getting the exact meaning of the 'edit the thread length to include the offset of the chamfer.' What am I supposed to do? I don't remember getting anything badly wrong not following this advice.


Thanks in advance!

 

[JohnRBaker]

I assume that you're speaking only of the 'Thread' feature and NOT Threaded Holes, correct?

OK, the 'Thread' feature, when applied, was designed to adjust the size of the cylindrical face, be it a hole or a shaft/boss, so as to represent the initial size before threading. Note that this was based on a rule-of-thumb taken from the thread design section of the 'Machinery's Handbook'. The problem is that the 'Thread' feature is an older and in reality, partially-obsolete, feature. One of the issues, which you've already noticed, is that there's a problem with the feature's attempt to adjust the size of the hole/shaft/boss, but ONLY if the face was the result of a feature created using the Sketcher. If you had defined say a hole by creating a Cylinder feature subtracted from a body then there'd have been no warning and the size of the 'hole' would have been adjusted. The same if the Shaft was created using a Cylinder feature. Of course, if you're using a Boss feature everything works just fine.

The reason for this is that the 'Thread' feature was originally implemented before there was extensive use of the sketcher. In those days 'holes' were usually created using either subtracted Cylinders or Cylindrical 'Pockets', and Shafts/Studs started life as Cylinders or Bosses. The issue is that the code was attempting to modify the feature's Diameter parameter but it doesn't recognize Sketch parameters (I know, this should have been fixed, but it's not trivial). Of course with the advent of a true 'Threaded Hole' feature with NX 5.0 this was no longer an issue with respect to Hole since they were created together with the Thread feature. However, many people still create Shafts/Studs using Cylinders and Bosses so that's why I stated the the old 'Thread' feature is only 'partially obsolete'. So the rule now is, make ALL threaded holes using 'Threaded Hole' features. Threaded shafts and studs should still start out as Cylinders and Bosses as you do not YET have a new 'Threaded Male' feature.

As for the chamfer issue, that's really just so that the symbolic representation of the thread, the extra dashed circles, look like their in the correct location. If you're not concerned about how they look (this has no effect on how they will appear when you create your Drawings) then just add your hole/shaft relief (chamfers) in whatever order you wish.

Anyway, I hope that helps explain what you're seeing and how to avoid the warnings.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[PrintScaffold]

Yes, I was speaking about the 'Thread' feature. Your explanation clears quite a few questions, thank you!

So I gather that the new modernised tool 'Threaded Male' is being worked on? How soon will it be available?

 

[JohnRBaker]

I can't say that it's "being worked on", but it's on the 'to-do' list.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.