curves and sketches in assemblies

[mfe4]

Hey,

I'm trying to learn NX 6 and having some constraint issues. I am trying to create a deformable tube that travels through a sphere with a hole in it. I would like to use a spline, but I cannot seem to get it to snap inside the cylindrical hole. I would like to create a curve or sketch that is constrained to move with the sphere and can be used by other components in the assembly so that I could snap the spline to it. Every time I sketch in the component I cannot see it in the assembly and every time I sketch or create curves in the assembly they end up fixed. I realize there is probably an extremely simple answer that I'm missing, but if someone could help me out it would be greatly appreciated.

Thanks,
Mike

 

[JohnRBaker]

If you're adding curves to a component, they will not be automatically added to the Reference Set so you will need to do that manually under...

Format -> Reference Sets...

...and select the 'Model' Reference Set and then select the sketch objects you wish to add to the Reference Set. Now when you go to the Drawing, the sketch curves should be visible.

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.

 

[hudson888]

You can often find that you need to create something else to snap to in such cases. Not being exactly sure of you geometry or design intent I would offer a tentative suggestion that in modelling (not inside the sketcher) you can create associative points to help you define the spline. You can create a point at the centre of the sphere using the "Arc/Ellipse/Sphere centre" method. Similarly you may be able to get an associative line to snap to the centres of two circles at the entry and exit/bottom points of the hole with the surface of the sphere. This second technique only works if the entry edge of the hole describes an arc or an ellipse (in this case you'll never get an ellipse), so if the the hole is off centre or at some oblique angle then the construction technique may fail.

But if you have to use a curve to define the hole axis then you could just save yourself the trouble by building it in the sphere component and linking it to the assembly. If the sphere side of the design is never expected to change then it is just one extra construction curve. If the sphere component does need to change frequently then there are probably a number of associative curve building techniques available that would be appropriate depending on the geometry and the simplest and best probably wouldn't even use a sketch.

For the spline my best guess is that you'd want to use the studio spline command. Associativity is available and tangency/continuity and it works in 3D model space in ways where you'll find that sketched curves fall short of.

Anyway that's a few rough techniques at a guess that may help you to find a suitable method.

Cheers

Hudson

 

[mfe4]

Hey Guys,

Thanks so much for your answers, I think those will really help me out. You've been a huge help.

Thank,
Mike Egan