nx2206: how close a swept wrap curve

[o0omirkoo0o]

Hi everyone and happy new year to all

I'm facing some difficulty to get a solid geometry from a wrapped curve that was extruded using the swept command.
As you can see in the attached image, i get this result and i'm not able to make it solid.

I sketched a rectangle on a plane, then i wrapped it to a cylindrical face to get a proper shape of the rectangle on the cylinder side face.
But it is a sheet and not solid..

Thanks to everyone for your support.

 

[Toost]

if you skip the wrapping and instead sweep the planar rectangle, you will get a solid body.
If you in that operation include the automatic boolean operation ( I am guessing a Unite operation)NX will create the corresponding edges in the intersection.
( corresponding to the wrapped curves)

NX will allow you to sweep "any shape", 2D and 3D but it will not "fill" an enclosed area unless it is planar, If the section isn't planar, "that face" could be any shape.
If you sweep a face, then that shape is defined and NX will produce a solid body, the swept face will be replicated in the end of the sweep.

Regards,
Tomas



The more you know about a subject, the more you know how little you know about that subject.

 

[o0omirkoo0o]

Hi Toost
Thanks for your suggestion.

I sweep the wrapped rectangle because only if i sweep it i can get a proper shape of the 'rectangle' connection to the cylinder.
As far as i can see, into sweept dialog window, there's no boolean type to choose, oly body type ( solid or sheet ) and both give me the samre result ( a sheet extrusion ).
Have a look to the attachment comparison between swept planar rectangle instead the wrapped one.

 

[Toost]

If you let that swept shape also sweep a little into that larger body , you can combine these two with a "Unite Operation".
If moving the sketch / adjusting the guide etc is cumbersome, use the feature "Move face" and pull the face some random distance into the larger body. Then Unite.
This will remove the overlap and produce new edges very similar to the wrapped curves.

Regards,
Tomas

The more you know about a subject, the more you know how little you know about that subject.

 

[o0omirkoo0o]

Ho Toost.

Yes, that solution i've already tried, but to be honest i was looking for a better ( or more 'elegant'? ) solution, instead extrude a bit more into the cylinder and unite them.
But maybe in some case, these are the only solution possible to achieve the desired design intent
Thanks a lot.

 

[cowski]

If you do not want the pieces united, you can sweep the rectangle into the cylinder and then trim it back to the cylindrical face. Perhaps if you could describe your 'design intent', we could give other options.

www.nxjournaling.com

 

[Toost]

As Cowski notes, we do not know your design intentions.
How do you mean elegant ?
Replace Face ?

Regards,
Tomas


The more you know about a subject, the more you know how little you know about that subject.

 

[mmauldin]

I wouldn't use a sweep in this case. I'd extrude the guide curve with offsets to form the rectangle, either replace face or offset the face adjacent to the cylinder and then unite.
Much cleaner than a sweep.