Combining faces in NX7 2

[JHLynn]

I am trying to combine a set of faces in NX7. I have sewn the faces and created a body, removed parameters, and NX leaves 3 separate faces. Is there a way to turn these 3 faces into a single face?

 

[cowski]

Try the join face command.
Depending on the geometry, it may or may not be able to combine them into 1 face.

Otherwise you could try to create 1 face from what you have. Perhaps cut some sections (clean up as necessary) and try a through curve mesh.

 

[JohnRBaker]

Only if the 'seams' can be removed without changing the shape of the surface. Generally that's very difficult to accomplish without some sort of 'recreation' effort.

However, you might get lucky so try this first; go to...

Insert -> Combine -> Join Face...

...and start with the 'On Same Surface' option. If that does not remove any of the 'seams', they the other option, 'Convert to B-Surface'.

If that still didn't give you what you're looking for you're going to have to accept an approach which will in essence 'recreate' the surface, but it will be an approximation, but if that will work for you, go to...

Insert -> Offset/Scale -> Rough Offset...

...and with the 'Offset Distance' set to '0.00' and the 'Surface Generation Method' set to 'Cloud Points' and the 'Surface Control' set to 'System Defined' select the complete sheet body and hit OK. If you wish to improve the approximation you can reduce the values for 'Offset Deviation' and 'Stepover Distance', but becareful to not set these value too small as this can have a big effect the speed of computation and the complexity of the final sheet body, so you may need to experiment a bit to get the hang of it all.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[JHLynn]

Thanks John, I will keep that in mind for the future. I had tried Join Face to no success, and even rough offset is not working properly but I think it's just a bad surface.

 

[jerry1423]

Maybe before doing a "join face" try a "replace face" by replacing one face with the other.

 

[Xwheelguy]

It's been a while since I've used NX, but I used to use Quilt for removal of what I felt were excessive faces. You have to do it at the surface level (not on solid unless you Extract the faces, Quilt, then successfully get a Patch to work).

This seemed to work better for me than Join Face ever did working with fairly complex Class A Automotive surfaces imported from Alias into NX.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[JohnRBaker]

The 'Point Cloud' option in the 'Rough Offset' function works similar to the old 'Quilt' command (which is still supported), you just have to set the Offset value to 'Zero'.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[Xwheelguy]

Nice addition....too bad I'm using crappy Catia now. Not sure what people find so great about every associative modeling command in Catia results in hiding the original object and creating a copy to represent the end result. File size ends up being enormous in some cases.

I miss NX quite a bit.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.