Remove non-touching solid (leftovers) after a subtraction.

[AndersPB]

Hi
I have after subtracting a connector shape from a solid(thin plate made as a solid), many smaller leftover non-touching solids that I want to get rid of.
The leftover solids results from that the connector`s pin openings was just that, "open".
What alternatives do you suggest?

Best regards
Anders

 

[SDETERS]

What Version of NX you using?

 

[AndersPB]

Hi.
I am running 7.5

Best Regards
Anders

 

[JohnRBaker]

Without removing the Parametrics of the Boolean feature, about the best that you can do, in NX 7.5, is to either 'Hide' or 'Move' the bodies to an invisible layer.

Note that starting with NX 8.5, we have included the ability to explicitly 'Delete' bodies, even if they are, as in your case, leftover from some Boolean operation and are actually part of a 'feature'.

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.

 

[kapmnit123]

Hi,
You can use synchronous to remove those leftover bodies (in case of NX7.5 ).I assume these solids are secluded from the rest.
Best REgards
Kapil

 

[JohnRBaker]

Are you sure? Deleting all of the faces of the 'secluded' body will NOT work.

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.

 

[kapmnit123]

Hi John,
You got me.... yes i can not delete the body using delete face (probably that was the region why delete body utility is introduced.).
The best we can do is to extart the body seperately and use it.
Best Regards
Kapil Sharma

 

[AndersPB]

Thank you John for your answer.
I am not to familary with the tech of this cad yet so bare with me for two more questions.
"Without removing the Parametrics of the Boolean feature" - what does this mean,is it an option?
'Hide' or 'Move' the bodies to an invisible layer. - will this exclude it during a export to, lets say a STEP-file?

Best Regards
Anders

 

[JohnRBaker]

You can convert any so-called 'smart' body (which was made using Features) in a 'dumb' body, which in your situation would then allow you to 'delete' the extraneous bodies from your model without effecting the remaining model. You can access to operation by going to...

Edit -> Feature -> Remove Parameters...

...and then selecting the body which these extraneous bodies are associated with. Now you can delete whatever you want, however, this has removed all of the parametric, or feature, data from the selected body. it will now be 'dumb', as we say.

As for hiding or moving the extraneous bodies to an invisible layer, NO, under normal circumstances this will not prevent them from ending-up in an exported format like STEP or IGES. Now there may be ways to explicitly limit which objects that you wish to export but if you export the entire file, they will go along for the ride since they still exist in the part file. This is one of the reasons why we implemented the NX 8.5 'Delete Body' function since this will allows you to 'delete' a body, even if it's part of some larger parametric feature, and as far as any downstream application is concerned, including translators, these solid bodies no longer exist in the model. And this is accomplished WITHOUT jeopardizing any of the parametric or 'smart' data in the part file.

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.

 

[AndersPB]

Thank you so much for the explanation.
I will make some trials in the morning.

Best Regards
Anders

 

[cubalibre000]

Use delete face via ST toolbar.

Thank you...

Using NX 8 and TC9.1

 

[JohnRBaker]

That doesn't work if you try to delete ALL of the faces of the extraneous bodies.

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.

 

[AndersPB]

Hi All.
Deleting faces do not work.( In 7.5 )
I have done as John suggested(Remove Parameters) and are happy with the results of this.
My work includes mostly non-complex fixturing so it works fine for my applications.

Greatings from Sweden - Thank you all for your input.

Regards Anders

 

[mmauldin]

You can create a solid that envelopes all the solids in your part. Then unite that solid to the solids you want to get rid of. Then intersect the resulting body with the one you want to keep. This will preserve your history and leave a single solid.