×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

NX9: New Option Include Sheet Bodies
2

NX9: New Option Include Sheet Bodies

NX9: New Option Include Sheet Bodies

(OP)
Include Sheet Bodies is a new option on the Top Border that includes or excludes sheet bodies during selection.

It works in conjunction with the Body Rule options:

•Single Body

•Feature Bodies

•Bodies in Group

This option lets you be more specific in the selection of bodies when using commands that infer Boolean operations.

But I don't understand the purpose of this new option. Thanks in advance to help me

Regards
Didier Psaltopoulos
http://www.psi-cad.com

RE: NX9: New Option Include Sheet Bodies

Exactly what functions are you seeing this "new" option in? And when you say "a new option on the Top Border that includes or excludes sheet bodies during selection", is this the normal 'Type Filter' (at the Left end of the top border bar) or something else?

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.

RE: NX9: New Option Include Sheet Bodies

2
OK, I figured it out (I had to go back and read the project documents to get the rational behind this new option and why it was big deal for some of our customers).

Anyway, what happened is that back in NX 5.0 we introduced the so-called 'Selection Rules', starting first with the 'Curve Rules' like 'Single Curve' or 'Tangent Curves' when a function asked you to select curves/edges for say an extrude or an edge blend. And then in NX 7.5 we added 'Body Rules', like 'Single Body' or 'Bodies in Group', when for example you're asked to select the 'Tool' bodies when doing a Boolean operation. And it was this 'Body Rule', particularly when doing a Boolean Subtract that caused a problem for some people.

As you may or may not realize, when doing a Boolean 'Subtract' you can use either a Solid or a Sheet body for either the 'Target' or the 'Tool' body, but in the case of a surface being used as a 'Tool' body it must pass completely through the 'Target' body so that it will basically cut it into two or more pieces. Now under normal conditions, like when selecting 'Single Bodies' you can set the 'Type Filter' to just 'Solid Bodies' if you wanted to make sure that you did NOT select a Sheet body, which often was not something that most people wanted to do. However, once we introduced the 'Body Rule', one of the options allows you to select a 'Feature Group' to define your 'Tool' bodies, but that 'Group' might consist of BOTH Solid and Sheet bodies and you may still NOT want to include the Sheet bodies and of course, at this moment the 'Type Filter' is of no use since what you're really selecting is the 'Group' and not the individual bodies in that group and besides, you might actually want both types (under certain conditions). But when you didn't there was no way to control that, at least not until NX 9.0 where we added this option to the 'Body Rule', that's the new icon with the picture of the surface on it, which when toggled ON will include BOTH Solid AND Sheet bodies, but when toggled OFF will only grab the Solid bodies in the Feature Group and ignore the Sheet bodies. By default this option is toggled OFF since the consensus is that including Sheet bodies when selecting a Feature Group is generally not the norm, particularly for modeling type operations, like Booleans.

Anyway, I hope this clarifies what this NX 9.0 enhancement does and why it might be useful to you. However, I suspect that unless you've encountered this problem of using 'mixed' Feature Groups somewhere, that you can just ignore it.

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.

RE: NX9: New Option Include Sheet Bodies

(OP)
Hi John,

Thanks a lot. It's very clear

Regards
Didier Psaltopoulos
http://www.psi-cad.com

RE: NX9: New Option Include Sheet Bodies

I assume that one or a few very large customers are using very strict and repetitive methods which we , the rest of us, don't. smile
Thanks for the info.

Regards,
Tomas

RE: NX9: New Option Include Sheet Bodies

Yes, without revealing who those customers might be, they appear to have been attempting to replicate certain workflows based on how they had used a competitive CAD system and so this was really an enhancement to make a slight change that made that easier. This will hardly be the first minor change many of us will see as these companies complete their transition to NX.

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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources