Locating a helix in part (NX7.5)

[NikonF6]

The problem is how to constrain a helix (or Spring) location? (in 3d) relative to the "hole" center...
Looks once the helix is moved by draging, no way to locate it any more...
This is not for assembly but producing aq part of multiple parts.

Thanks for your time

 

[cowski]

In the spring part file, create a datum axis on the axis of the spring. Now in the assembly, you can switch the spring to the 'entire part' reference set and use the datum axis in a positioning constraint. When it is constrained properly, switch back to the 'model' reference set.

For more complex parts, it may be advantageous to create a dedicated 'constraints' reference set that contains datums to use when constraining to other parts in the assembly.

www.nxjournaling.com

 

[NikonF6]

Assembly is not in the game at all.
The Spring and the another part (base with a hole) are inside one single part file (parts can be substracted, unite, ...).
The Spring is away from the hole (moved). I have to move the Spring so its cebterline is at the hole centerline (please do not ask why this all... it just has to go that way). I can make a new Spring with a small cylinder (or 3d-line) in the middle, but moving a cylinder does not moves the Spring...

If i make a datum axis as a Spring centerline, can i move the datum axis so and Spring moves, ALL WITHIN A PART FILE ONLY.

 

[cowski]

In NX 7.5 and earlier, there is no way to make a helix associative to a datum axis. If the helix is in a known position, you can create a line or datum axis representing the axis of the helix. You can now create a group for the spring geometry (helix and centerline reference); move the group using the centerline as a reference - the centerline will travel with the helix.

An alternative is to use the swept command instead of the helix. Create two lines perpendicular to each other (the result will be an L shape). One line will be the axis of the helix (controlling the length), the other will represent the radius of the helix. Use the swept command with the angular law option to create a helical sheet body. The outer edge of the body can now be used as your helix and its position will be controlled by the input lines.

www.nxjournaling.com

 

[JohnRBaker]

As cowski has alluded to, changes were made to the Helix function after NX 7.5. In fact, if there's any chance at all that you'll be updating to NX 8.0 or newer in the near future, I would advice that you not waste a lot of time coming up with some sort of workaround since the Helix function has been completely replaced with something that does exactly what you want as part of the definition of the Helix itself.

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.

 

[SDETERS]

Try this. Make your spring in a new part. Make sure your spring is centered on the coordinate system. Now in this new part change your selection filter to solid body. Select your solid body the spring and hit CTR+c. (Copy). Now in your PRT file you are wanting to move the spring in hit CTRL+V. This should paste the part as a solid body with the coordinate system still attached. Now you should be able to use move object, so select the solid body of the spring and slide it over. I think you may want to keep move parents selected.

 

[SDETERS]

Oh you said constrain well with associative turned on you can not move your parents. I was thinking of using move object with moving coordinate system to coordinate system. Sorry missed the word constrain in your original post.

 

[mmauldin]

It can be done, only not with a helix. By using a curved wrapped around associative geometry, you can accomplish what you are trying to do.

See attached. Tray changing the parameters of the chamfer, the spring pocket and spring will follow (within limits).

 

[NikonF6]

Thanks a lot to all.
hard to beleive we will update to NX8.
Datum axis does not works at the moment so well (cannot insert dimensions from it to the coordinate system, or anywhre else...)
will tri 2 point and 3d line as a centerline, group it all and change coordinats of the points...

 

[JohnRBaker]

There is NO way to create a feature using the Helix curve function in NX 7.5 that will ever be associative in either its origin or orientation.

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.

 

[NikonF6]

thank you so much. This all saves me a lot of time.

 

[macdacc]

Hi NiconF6,

The one of work around solution for that issue can be creating helix shape with “Low Curve” feature.

I have created expressions and using it made “low curve” (helix curve) which is associated to hole axis. Whenever you change location of hole - helix geometry will follow accordingly.

Please see attached.

Regards

 

[cowski]

low law curve

www.nxjournaling.com

 

[NikonF6]

Thanks to all. I did not expect that much ... This is a great forum.

 

[mmauldin]

One last post to further show the benefit of the wrapped curved method. You can build your driving sketch in a way that the end result is a more realistic closed end spring.

Updated part file: