NX Shaft partially threaded from each end

[MattBaumann]

I want to make a shaft that has a through hole. I want each end to have a thread that goes in a certain distance, but not a complete threaded hole. No matter what I do, it only shows up as being threaded on one side in my drawing. To get it to show correctly, I have to manually add a Thread to the other side. How do I accomplish this all in one step? FYI, using NX8.5.

 

[JohnRBaker]

Why are you insistent on "accomplish(ing) this all in one step"? I mean, it's not like the guys in the shop are going to be able to manufacture it "all in one step"...

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.

 

[MattBaumann]

Just assumed it was possible to accomplish in one step since it shows it correctly in the model, just not the drawing. That's all. It works if I don't have a thru hole, but once I do it hides one side of the threads.

Matt

 

[JohnRBaker]

Have you tried creating the two threaded holes, each deep enough to just overlap a bit in the middle?

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.

 

[MattBaumann]

Yes, as soon as they create a thru hole (even if they only overlap 0.1mm), it only shows one thread. If I keep it so it isn't a true thru hole, it works fine. I'm assuming it's a glitch.

 

[djflesse]

If I create the shaft by extruding from midplane, then use the hole feature to add a threaded hole drill all the way through but only threaded my set distance I can the mirror it to get my shaft with a through hole but threaeded both ends.

When I go into drawing it shows up correctly, but it is split in the center from the mirror feature. If I then go back into the model to unite the two halves, when I go back into the drawing I can no longer see the split, but once again it removes the threaded hidden lines from the other side.

 

[JohnRBaker]

I tested with with NX 9.0 and it behaves the same as you saw in NX 8.5. Note that I've opened a PR and I'll report whatever I learn.

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.

 

[jtrist]

I have had this issue with water lines in my tool design and have always ended up add a symbolic thread to the missing end. I would also like to know what you find out. Currently using NX 8

 

[JohnRBaker]

OK, I've gotten feedback from my PR and it's as I suspected. The behavior of NX in this case is as expected. The proper modeling workflow should be one of the following:

1) Create a single simple thru hole the length of the shaft and then add, using Symbolic Thread features, both threaded sections, one from each end.

2) Create a singled Threaded Hole feature whose pilot hole goes all the way through the shaft and then add the second threaded section at the other end using a Symbolic Thread feature.

Either of these two workflows are what is recommended, and in reality, closer duplicates how such a part would actually be manufactured.

Note that while the Symbolic Thread feature appears to be from a past era of NX, it is still fully supported and there are plans to update it and bring it up to meet the new UI and feature standards including linking it to the common Thread Data files used by the current Threaded Hole function.

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.