Threaded Hole through multiple body 1

[barbarus]

i try to find a method to make a threaded hole through multiple bodies.
i see that with the extrude command there's an option called "through all" inside "Limits" tab where i choose subract from "boolean" tab and select multiple body, but in the hole command i not find any similar..maybe there's something (a command or a macro) like assembly cut that working with bodies and not with component.
Other CAD like solidworks or SE make this operation without no problem so i think is strange that NX not doing it..
we use NX 8.5 in our company but we are planning to pass to NX 9.0.1

Thanks

 

[cowski]

Try "hole series".

www.nxjournaling.com

 

[barbarus]

i try the hole series but not make threaded hole though all bodies but only with the last (from the "start" and "middle" tab cannot select threaded like the "end tab")

 

[JohnRBaker]

In the real world, there is NO way to properly thread two separate parts and then have them be assembled with a single threaded feature through both of them.

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.

 

[barbarus]

Yes i know that in real world is absurd but i think that is really useful for people that make carpentery and i not understand why SE can make it and NX no..

 

[JohnRBaker]

Well, since NX's heritage was born in the MANUFACTURING world, we've always tended to only allow the creation of parts that CAN be manufactured. For example, this is why we don't allow you to create non-manifold models. By definition, non-manifold models cannot exist in the physical world so we don't allow them to be created in the first place.

Now if you want to create two back-to-back threaded holes, be our guest, but don't expect NX to create a single, fully-threaded hole though more than one part in one operation.

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.

 

[barbarus]

The company where i work is already siemens guest so maybe i try to contact they for ask the creation of a tool or a macro.

Thanks everybody for the help

 

[JNieman]

I'm curious why one would want two parts threaded adjacently. Since carpentry was mentioned, I assume you're talking about wood screws? If that is the case, don't you typically call out a type of fastener class/length, and simply a minimum spacing? Depending on context/industry. If you really need specific X/Y screw locations, I would just create a bunch of tiny 'simple holes' with a unique diameter, and then when my hole table is created, change that range of X/Y results to be (1/8 x 2" DECK SCREW) or whatever you need. It will give a small visual cue on the drawing, with location called out, without being over-complicated to the point of inaccuracy. It seems excessive, superfluous, and unnecessary to create a threaded hole in the model. You're never going to have a threaded hole - you never thread a hole THEN put in a wood screw. This is my novice, heavy-handed solution, anyways.

I think what Mr Baker is getting at is... sometimes it is best to step back and try to see the forest despite the trees, and decide if you're /asking the right question/ before you get stuck on retrieving any answer that satisfies your current urge.

I honestly believe, given the information at hand, you may be asking an inappropriate question.

 

[barbarus]

i ask to our production foreman and they tell me that is not absurd to make a threaded hole through two or three body (we use principally plate with 10-15mm of depth)..it's better not to make it but in some emergency situation is the only thing to do..
i put an example of what i try to do..the result of this hole feature create a thread hole into the last body and not into the first and second body..

thanks

 

[JohnRBaker]

Then you will just have to create two separate hole features, one in each body, that align with each other.

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.

 

[barbarus]

yes i know..but if i have ten or more body is a bit recurring..anyway i ask to siemens man if can customize it with a macro or tool to do what i want automatically.

thanks to all again

 

[JohnRBaker]

Are these parts separate Components in an Assembly or just individual bodies in the same part file? If they're separate Components, do you want the holes to exist in the detailed parts or only as a feature within the context of the Assembly? In other words, do the holes represent an operation that will be physically performed after something has been at least partially assembled in the shop?

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.

 

[barbarus]

it's bodies in the same part file..

 

[JohnRBaker]

Are the bodies such that they touch each other by a common planar face? Like a cover on something? If so, could you model your two parts, create a Datum plane where the two parts touch, unite them into a single body, create the fully-threaded Thru-hole and then Split the single body back into the two original bodies afterwards? Look at my attached example and follow the workflow (use 'Feature Replay') to see what I mean.

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.

 

[FrankSwinks]

Can I suggest a workaround as follows. Create a cylinder placed on the centre of the threaded hole of length through the multiple bodies and the diameter just slightly larger than the drill hole size. The cylinder should be united only with the top body. The cylinder outline are still visible in the lower bodies. When you create the threaded hole the top chamfer is correct but the bottom chamfer is not created (because the chamfer is in the cylinder portion of the upper body).

Frank Swinkels

 

[barbarus]

John thanks for your help, i also know this method but is a bit "boring" if you have ten or more body..anyway now we ask to siemens man if they can do something to help us..

Frankswinks i try your method but when i make the threaded hole i got the top body thread correctly but the other body not threaded correctly so i think that workaround not work well or is useless for my request..

thanks anyway.

 

[FrankSwinks]

Here is an example part. The thread is through the three plates because the cylinder is the full depth.

Frank Swinkels

 

[barbarus]

Yes, same result as me. but i think that workaround not work flawless with drafting..if i make a section on this hole the result is not correct for what i need..i attach an image of the result..

thanks anyway

 

[KhimaniMohiki]

In the hole command under boolean, selct none, this will create a hole tool body, or multiple hole tool bodies, then use Trim to remove the hole bodies (using selction intent feature bodies) from the targets, I do this quite regularly.

Khimani Mohiki
Design Engineer - Aston Martin
NX8.5

 

[barbarus]

thanks KhimaniMohiki for your suggestion..it's not bad