Swept Solid is not solid in NX 9

[FinnAero]

Hi All,

i am trying to build a hollow wing. I created 3 airfoils at the root, the tip and in the middle, which I use as sections for the swept command. I created the trailing and leading edge as guides. Now the outer surface looks perfectly fine, but although i selected "solid" in the command, it is just a hollow sheet with no thickness.
Now i thought i could use thicken, but that command doesn't work. Originally, i wanted to offset the airfoils by the skin thickness i need and create a smaller body with swept to subtract. This subtraction body comes out solid as it should.

Does anyone have an idea on how to solve this? I don't care for the method, as long as i get the required geometry. Thank you very much!

Finn

 

[Lockdain]

Hi,

It would be great if you can provide an example in .prt.

http://www.CADabout.ru

 

[cowski]

Sometimes NX can only create a sheet body even though you request a solid, the result usually has to do with the input. For example, in the extrude command, if one or more of the curves are out of plane, the result will be a sheet body. The swept command probably has similar limitations. Make sure that all of your section curves lie in the plane of the respective section.

If you can only get a sheet body from the swept, you can still get a solid body with some work. Create sheet bodies to cap the ends and use the "sew" command to combine all the sheet bodies. If the sew results completely enclose a volume (there are no gaps between any of the sheet bodies), it will automatically be converted to a solid body.

www.nxjournaling.com

 

[Toost]

Thicken, can it thicken outwards ?
Do the trailing end go into a sharp edge ?
Do you get multiple faces in the sweep.?
Are the edges of these faces logically placed ?
Does the Sweep feature use the Preserve shape option ?

Regards,
Tomas

 

[FinnAero]

@cowski:
The section profiles are made from imported points, they should be in plane. Nevertheless, i tried projecting them onto planes and use the projeceted curves, but that didnt work. I thought of the sew-command before, but the fill-surface-command didn't work either. But your post made me come up with the idea of creating a surface around the profiles and then trim it, which worked greatly. With that the sewing works. So i now got a way to make it work, though its not elegant.

@Toost:
Thicken does not work in both directions
Yes the trailing edge is sharp
Yes i get 6 faces in total
There is one face on the upper side and one on the lower side plus one small stripe at the leading edge

Yes it does, disabling it made no difference though (besides i only have 4 faces now)

Thank you all for your support!

 

[cowski]

If the trailing edge is sharp, I do not recommend using a "closed" type spline for the section curve. Use an open spline and make the end points coincident on the sharp corner. A closed spline will round off the corner, creating an area of high curvature that may not offset or hollow correctly. A similar situation may result if the "preserve shape" option is turned off in the swept command.

www.nxjournaling.com

 

[FinnAero]

@cowski: i did it the way you said, and now i get a solid swept! It still cant't be thickened to the outside, however it is easyier than before

Thank you!