Extruding a curved face along a vector, Please Help!! 5

[Rich944]

Hi all,

Please let me know if this can be done because every time I try this I just get a sheet body rather than solid. Here is the description (Unfortunatly I cant upload due to IPR)

Say I have a solid wing shape, all I want to do is offset a square section of the wing surface along a vector by 8mm.
This is what I did, create a datum plane directly above the wing solid. Draw a sketch of the simple square. Do a divide face projecting the square onto the wing surface. Now that I have a separate surface I thought I could just extrude the edges of this surface along a vertical vector by 8mm, but as I said I just get a square 'frame' made up of sheet sufaces.
I have also tried projecting the sketch onto the suface and extuding the projected curves but just get same result.
I know I could just thicken the divided face but this extrudes along 'face normals' not along a vector.

Grateful for any help as deadline due soon!

BTW I dont have the freeform package, just standard NX if that makes a difference.

NX7.5

Cheers,

Rich

 

[SiW979]

Like this? Use yor selection intent to pick face adges and make sure you hafve solid selected as your output option.

Cheers

Si

Best regards

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

 

[John2025]

JBCad,
That works with divide face, but if I pick the outer edges of the first extrusion, I get a sheet body without the top face. It seems like I run into this alot. Any idea why?
Thanks,
John

 

[SiW979]

I have done another one, is this what you mean? basically all I do is use selection intent to make sure I either pick sheet edges of face edges and then within the extrude dialog, make sure that solid is selected as the ouput. That's the only thing I can think of sorry :-(



Best regards

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

 

[JohnRBaker]

If you use the 'Face Edges' option then the FACE itself is ALSO used to help define the resulting solid. However, if you simply select the edges, as if they were independent curves, since they do not form a planar section it's not possible to create a solid as there is NO way to know exactly what the shape of the 'start' and 'end' capping faces would look like if all you had were four 3D curves and no other inputs.

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.

 

[Rich944]

Many thanks for looking at this Si.

Yes that is what I want, unfortunatly I tried it on my part and couldnt get a solid body (solid body checked on extrude).

The only main difference between your part and mine is that mine is curved in more than one plane.

I managed to recreate the unwanted effect I am getting by doing a square on a sphere.
See attached.

Now im thinking that is the limit of my NX package without the 'freeform' add on??

Cheers,

Rich

 

[Rich944]

Hold on, I will look for Face edges, selected just edges before!

 

[Rich944]

Brilliant! Many thanks guys! Forgot to select face edges in the drop down.

One thing Si, did you really need the projected curves? I was dividing the face directly with the sketch.

Stars all round!

 

[JohnRBaker]

Now im thinking that is the limit of my NX package without the 'freeform' add on??

That should have no effect whatsoever.

And the Face Edge approach works with doubly-curved surface (see attached example).

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.

 

[John2025]

Ha!! Thanks guys, I always thought this was just a limitation. Now I get to show off and tell the other 2 users.