How do I attach Helix curve parametrically?

[Jamziee]

Hi guys,

Hope you can help. I have created a thread using the sweep command around a helix curve on a shaft. I want to attach the helix to the end of the shaft so that when I increase the shaft length, the helix will follow.

Any ideas?

Many thanks,

Andy.


---------------------
(Using: UG NX4)
Design Engineer

 

[cowski]

The answer(s) you get will depend on what you mean by the helix 'following' the shaft. Do you mean that the helix length increases to match the new length of the shaft, or that the helix length stays the same but just moves to stay attached to the end of the shaft?

 

[Jamziee]

Hi Cowski,

Sorry, I should have been more specific. I want the helix to stay the same length but stay attached to the end of the shaft when the shaft length is increased.

Many thanks,

Andy.

---------------------
(Using: UG NX4)
Design Engineer

 

[JohnRBaker]

The best solution at the moment is to make the fixed end of the shaft and the location of the helix the same point.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[cowski]

I agree with John, but if this situation is not possible there is at least 1 work around available. Make the helix and swept features much longer than you need (in both directions) then attach a datum plane to the end of the shaft (assuming the end is flat) and another datum plane offset from the first by the length of the thread, then trim the swept feature by the datum planes before you unite it. A couple of drawbacks to this approach (other than not being a very 'clean' solution) is
1) the thread start/end will rotate as the shaft length changes - this may or may not be important to your application
2) it will not work so well for a tapered thread.

 

[hudson888]

Any of these are in the right ballpark. I seem to remember working though an example with a previous poster that you may be able to search for. I think the proposal was that you either build the model around the base of the helix because that won't move, or you link in a model of the thread based on a mated part containing that geometry.

Cheers Hudson

 

[JohnRBaker]

Well starting with NX 5, there's another scheme that will allow you to create literally anything and make it's origin associative to some other body.

That function is the new 'Instance Geometry' command.

What you do is create your Helix (or any object) and then create the item that you wish to associate it to. Then using Instance Geometry you do a 'Point to Point' transform and select appropriate references points on both the helix and the object you wish to associate to and make a single 'Associative' copy. Granted, you will technically have TWO Helical curves, but you can hide the original one and just edit it by it's expressions, and of course the other will update since it's an instance of the original. And since the copy is not located relative to the point you selected on the body, if you edit it in such a manner that this point moves, the helix will also move.

Anyway, we've now got another tool to help create objects which you can associate to other objects.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[Jamziee]

Hi all,

Many thanks for all your responses. There's plenty to think about so I'll give some of your ideas a go.

John - we're upgrading to NX5 anytime now, so in the future I'll be able to use the 'Instance Geometry' method.

Regards,

Andy.

---------------------
(Using: UG NX4)
Design Engineer