Siemens NX (Unigraphics) Users

Created by Mustafa Aşan on 27 April, 2018

How can I create a non-circular section spring along non-linear shaped helix? (NX)

I want to built a spiral protective cover on the electrical cables in my design. So I have some routing of cable at some diameter. I want to model a protective cover at some length along the cable (routing). The routing is a spline curve. I need to create a spiral around the spline (which is pretty easy). Then create a rectangular section on the beginning of the helix in order to sweep it along the spiral. But the (rectangular) section does not keep tangent to the guide curve (which is an helix). Any solutions?

PS. By the way a circular section (i.e. a spring with a non linear center line) being a symmetric section has no problem.

2 Answers

Hi Schlomo,

Firstly, make sure your swept section is fully defined, perp to the start point of your spline. You will need a 'face' swept along the spline path to orient the section. A tube works fine for this, or any circular sweep.

When you setup your sweep, under 'Orientation Method', you want to select 'Face Normals' then your circular tube/section/etc..

Good luck

I think it's fair to say that we can start from the point where the spline path and helix are created?

These are the steps going forward.

s2: Created a single segment 'Tube' along the spline path

s3: Sketch the square section and fully constrain (center to midpoint line is 'point on curve' to the start point of the spline)

s4: Surface > Swept to create the Swept section (square sketch is section, helix is path and tube face normal is the 'Orientation')

s5: Swept command details

s6: trim ends with endpoint planes

Hope this helps