uniting solid bodies.. 1

[mechjames]

Hi Guys,
I created a part out of 3 solid bodies. I did not unite the solid bodies as I was going along. I could have done this quite simply with the unite option in the extrude command. Can I unite these solid bodies now the part is finished?

many thanks,
James

- found it, new it had to be obvious! thanks...

 

[JohnRBaker]

The only noticeable advantage to performing the Boolean operation (Unite or Subtract) as part of a feature creation operation, such as when you're creating an Extrude feature, is that it will make your Part Navigator less messy as the Booleans are created as part of the feature itself. If you perform the Booleans as separate operations they will each create a feature node in the Part Navigator.

Now in the past, many people avoided using the Boolean option when creating feature because we did not allow you to edit the Boolean at a later date, but that's no longer an issue since the imbedded Boolean is now fully modifiable, even to the point of setting it to no Boolean operation at all. And since that is now the case, starting with NX 7.5 we've implemented 'Inferred' Booleans which means that based on the relationship between the feature body that you're creating and the existing model, the system now attempts to infer the type of Boolean that you are likely to be creating, either a Unite or a Subtract, depending on weather the feature body is going 'into' or 'out of' the existing model, and the feeling is that this will be correct in the vast majority of situations.

As for waiting and doing the Booleans later, there is NO downside whatsoever, other than they showing up as line-items in the Part Navigator.

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

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[cowski]

One note about performing the boolean as a separate feature, if you go this route you will have access to the keep target and keep tool options. These options allow you to keep a copy of the target or tool body, respectively. In most cases these options should be left turned off (unchecked), but on rare occasions I have put the keep tool option to good use. I have not found a good reason to use the keep target option, though I'm sure someone, somewhere out there has.

 

[JohnRBaker]

Yes, but since you can edit the 'internal' Boolean as if it were originally set to 'None', you can always go back and edit your model in such a way so that you can take advantage of the additional options available with an 'explicit' Boolean, if it's needed at a later time.

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

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[mechjames]

excellent info guys, thanks...
this answered a couple of things I had in mind surrounding this!

cheers,
James