Split Body using Non-planar surface? 1

[sluzzer]

How to split a body using a non-planar surface as tool?

 

[jerry1423]

you can either subtract the non-planar surface from the solid body
or you can trim to it

 

[cowski]

Set the split body tool option to "face or plane", adjust your selection intent rule if necessary, and select the faces to use as the split tool.

www.nxjournaling.com

 

[sluzzer]

@jerry1423
thanks for your reply.
I don't want to subtract or trim the body. I just want to split the single body into two bodies using its non-planar surface. Is it possible?

 

[aluminum2]

From what I understand the split body command keeps both bodies. no exceptions.

The trim body command is the one where a body is subtracted on a specified side of a surface or plane.

 

[sluzzer]

@cowski
Not able to set a non-planar face as tool to split.
I am using NX8

Thanks

 

[jerry1423]

You are able to use subtract and get the same result as if it was a split of a planar surface, just give it a try (you can always undo it)
and make sure the menu is fully expanded with the toggles set the way you want them

 

[carlharr]

Split body works fine for me with a non-planar surface?

The subtract is nice as well though didn't know you could do that!

http://www.jcb.com

NX 8.5 with TC 8.3

 

[sluzzer]

@jerry1423
in 'subtract' option, I am not able to select the 'face' as tool. It asks for 'body'.

 

[cowski]

Not able to set a non-planar face as tool to split.

The option exists and it works. Does the face you are attempting to use completely divide the body?
Perhaps a pic of what you are attempting to do would help.

www.nxjournaling.com

 

[jerry1423]

you should be able to select the face, check what your selction filter is set to

 

[sluzzer]

Thanks everyone for the reply..
Yes it works
But in some model it not works for me. I think I have not understood something properly. I am trying to use the face of the body itself to use as tool. please see the attached model. I want to split the model into 2 bodies & I want to use the spherical face as the tool. How to do it?

From the question by cowski "Does the face you are attempting to use completely divide the body?", I understands that the face which we are going to use as a tool should completely divide the face. In the attached model, the spherical face does not pass through the intersection. So in this case, how to split it?

Thanks

 

[sluzzer]

here is the model..
nx8 version

 

[carlharr]

You can't use a face of the body to split the body, it needs to be a separate feature.

So you could extract a copy of the spherical face to use as your "splitting object", but you are left with a hole in the top of the extracted face.

So your best bet actually would be to create a new "splitting object" as a sketched and revolved surface.

http://www.jcb.com

NX 8.5 with TC 8.3

 

[carlharr]

Pic attached

http://www.jcb.com

NX 8.5 with TC 8.3

 

[jerry1423]

you can extract a face and toggle "delete holes" and then you can do what needs to be done here

 

[cowski]

An alternative method

www.nxjournaling.com

 

[sluzzer]

@ jerry1423 & cowski.. Thank you very much