How to model a 3D sweep?

[fast4door]

I'm trying to create a retainer for a USB plug so it doesn't get lost. Think of the thing that keeps your gas cap attached to the car, or the cap retainer on a nalgene bottle. I need to sweep a circular shape through different axes/planes to achieve the shape I need.

I'm more familiar with SolidWorks, and in that platform they have 3D sketches. Is there something similar in NX? I've been reading about basic curves, but I don't know how they work since I just use sketches all the time.

What's the best way to model it? I've attached an image of the part that I'm trying to create. The sweeps were created using multiple sketches and it's just a pain to modify.

Thanks!

 

[jerry1423]

Insert (pull down menu) -> Sweep -> Sweep Along a Guide

If you go to Help -> Command Finder
and enter the command as it is in SW it may help you find the eqivalent command in NX

 

[fast4door]

The issue is not how to execute the sweep command, the issue is how to simplify the guide curve from multiple sketches in different planes to one simple curve.

 

[RKulchy]

You could try either using a stand alone spline and trying to get the shape you are looking for or if you know the path you want you could create a point set and then use spline to connect the dots.

 

[JohnRBaker]

Or use 'Join Curve' to get a single spline from a series of 2D Sketches appropriately positioned.

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.

 

[SiW979]

Have you thoght about using a an associative CSYS to sketch on, this makes the model very easy to control. Have a look at the attached example. Edit the dimensions in the first sketch called dia and angle and you will see the model will behave much better. (for the CSYS, use origin X point y point and make sure it is associative).

Hope this helps

Si



Best regards

Simon NX7.5.4.4 MP5 - TC 8 www.jcb.com

 

[scope63]

i have found that the best way for this is to make 2 different sketchs, perhaps 3 depending on the complexity. 1 sketch is as example the top shape, the next is the for the side. create extruded surfaces for each sketch and then create an intersection curve that will become your 3d driving curve for the sweep. i don't use 'sweep along a guide' but use the 'swept' command as it has more functionality and control. you could also use the tube command.

Scott Copeland
Design Engineering Contractor
Persego Int'l

http://www.persego.com