Create a pipe using a spline as a guide - NX9 6

[CAD2015]

Hi,
How could I create a pipe (OD 12mm and ID 10mm)using the points in the file attached?

Thanks

MZ7DYJ

 

[cowski]

Create a spline through the points (studio spline, through points option). Then use the "tube" command to create the tube using the spline as a guide.

www.nxjournaling.com

 

[CAD2015]

Thanks!


MZ7DYJ

 

[Toost]

In this case, due to the position of the points, you might instead want to create lines between the points and then create arcs ( fillets) tangent to the lines. When creating the tube, use the "Tangent Curves" +"Follow fillet" option in the selection intent .


Regards,
Tomas

 

[CAD2015]

Thanks, Toost!

MZ7DYJ

 

[Xwheelguy]

Currently working for an emissions control company and I'd have to second Toost's suggestion. Use analytic geometry (lines & arcs) for tubing whenever possible. It will make detailing the parts easier in the long run.

Tim Flater
NX Designer
NX 9.0.2.5 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[CAD2015]

Thank you, all!
The main point of the topic is that I need to get the ability to modify very fast the location of the points, based on engineering request.
Will you, please, update your answer based on this new task?
Thanks!

MZ7DYJ

 

[cowski]

Do as Toost says. Use associative lines and arcs. The endpoints of the lines will be associative to the points and the arcs will be associative to the lines. When you move one or more of the points, the lines/arcs will update.

www.nxjournaling.com

 

[ewh]

Agree with the others. I have also combined methods, using lines and arcs with splines (to represent coiled hose). Easily updates when done correctly.

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[JohnRBaker]

If you don't want to break the path into a series of straight lines and arcs but you would still like to get the performance benefit of doing so, simple set the 'Output' option, in the 'Settings' section of the Tube dialog, to 'Multiple Segments'. You can control the number of segments by adjusting the 'Tolerance' value (a larger 'Tolerance' value will result in less segments).

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

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

 

[CAD2015]

Thank you !

MZ7DYJ

 

[cowski]

I believe that using lines and arcs would be more for manufacturability reasons than CAD performance reasons...

www.nxjournaling.com

 

[Xwheelguy]

Also helps in drafting if you're dimensioning the true views of bends - you'll get a full radius rather than different radii along the spline segments.

Tim Flater
NX Designer
NX 9.0.2.5 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB