Subtract surface from solid in NX 9.0.2.5

[tryitagain]

I just started working in 9.0 and tried to subtract a surface from a solid. NX gives me the option to selct a surface, but doesn't select it.
What do I have to do in order to make it work?

Thanks

 

[cowski]

Surfaces in NX have zero thickness. Subtracting a surface from a solid may not result in the desired outcome. If the surface entirely cuts through the solid body, you can use "trim body" to remove a portion of the body or the "split body" command to cut the body into 2 pieces.

www.nxjournaling.com

 

[SvenBom]

Do you want to remove one surface from a solid body and so create a sheet body from a solid?
1. If so, select Delete Face command.
2. In Delete Face dialog box, open the Settings group.
3. Uncheck the Heal option.
4. now select a face on a solid body and click OK
The face is removed from a solid body and solid body is converted to a sheet body.

 

[jerry1423]

Can you show a picture of what you are working with ?

Jerry J.
Milwaukee Electric Tool

http://www.milwaukeetool.com/

 

[Toost]

I played with it, It turns out that in NX7.5 one can select and subtract a sheet from a solid, and thereby split the body if the sheet is large enough.
In NX9 - NX10 the sheet cannot be selected , despite the selection filter states" sheet body".

I have not written an IR to GTAC and will not since i do not see the logic in using subtract on this combination of data.


Regards,
Tomas

 

[jerry1423]

Sheet bodies have been subtract-able from solid bodies since pre UGV10.
Sometimes it's a nice option when working with a closed loop sheet body.

Jerry J.
Milwaukee Electric Tool

http://www.milwaukeetool.com/

 

[JohnRBaker]

Note that I've verified that this capability, being able to use a Sheet Body as the Tool Body during a Boolean Subtract, has been working as far back as at least NX 5.0 although prior to NX 6.0 this would result in the loss of all parametrics.

I've opened a Priority 1 PR (I classified it as a 'regression') and will report back what I learn.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[JohnRBaker]

OK, I got some feedback as to why this change was made in NX 9.0 and what you can now do.

The issue which promoted the change had to do with a previous enhancement which allowed you to select a 'group' of Bodies for the Tool Body but since a 'group' could contain both Solid and Sheet bodies it was felt that since Sheet bodies, when used as a Tool Body, does not actually perform a Boolean Subtract but rather splits a Body that they should be ignored so that the result would be more predictable. However, so as to provide a way so that IF the user ACTUALLY wanted to include Sheet Bodies in these operation, whether they were part of a 'group' or just being selected individually, an option to 'Include Sheet Bodies' was added to the Selection Bar. This is one of those icons that can be toggled ON or OFF and once selected will remain set. Now it's a very good chance that this icon is currently disabled so you'll need to go into the Selection Bar and enable it. This can be done by simply going over to the far Right of the selection bar and selecting the small down arrowhead and then in the 'Selection Group' item select the 'Include Sheet Bodies' item (It looks like small 'gold' sheet body). Note that this icon will only appear in the Selection Bar when the 'Body Rule' item is present, such as when being asked to Select the Tool Body during a Boolean Subtract. The 'Include Sheet Bodies' icon should, by default, be located just to the Right of the 'Body Rule' item. So if you leave this icon toggled ON, then NX will behave like it did prior to NX 9.0 and you'll be allowed to select a Sheet Body as a Tool Body when performing a Boolean Subtract.

Now this may sound complicated but since using Sheet Bodies as Tool Bodies when performing Booleans is not really kosher, just that we've allowed it for so many years, that it was felt that this new approach allowed users to make this an exceptional behavior if they so desired but for most people, NX would behave in a more logical way since we do have explicit tools when one wishes to Trim or Split Solid Bodies using Sheet Bodies as 'tools'.

And who says we don't look out for our legacy user when we're making changes so that new users can more easily understand how NX works and how they should use it


John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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