What's the best method to join bodies (NX5)

[speedster29]

We are making the transition from I-DEAS to NX, and it is going well for the most part, but there is one thing that has me stumped.

In I-DEAS it was very simple to join two bodies (or parts) together to make a new part. For those of you familiar with I-DEAS, the operation was called "join with relations." The result was to add a new "branch" to the history tree of the first part. We would use this technique often to create certain types of parts such as compound spur gears, for which it is convienient to model the two gears separately before joining them together.

I cannot find an equivalent technique in NX. It can be done as an assembly but that is not desirable.

 

[ewh]

Unite

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[JohnRBaker]

Years ago it was called Part Merge, but now you have two approaches that works, depending on where you wish to start from.

If you are in the Part file that you wish to 'Merge' another Part INTO, then use File -> Import -> Part...

However, if you're in the Part file which has the data that you wish to 'Merge' into ANOTHER Part file, use File -> Export -> Part... using the 'Existing' option for the 'Part Specification'.

Note that if there is only a portion of the file that you wish to Merge into another, it's best to use 'Export' since you can control the content of what gets 'Merged'. if you use the 'Import' method, you get everything.

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[speedster29]

Yes, File -> import will merge the parts, but I see no control over the relations between the two merged parts.

Take my gear example. To make a compound gear, you want to attach a face of the second gear to a face of the first gear, maintaining the centerline alignments. Also, if the first gear is modified, say by changing the face width, you want the second gear to move with it. It behaves just like an assembly constraint (touch align, infer centerlines), but it is a single part.

 

[Xwheelguy]

Is there a NEED to have both gears in separate NX files? If not, then just model both bodies in the same part file and then Unite, as ewh stated, or perform whatever Boolean you need to do. NX doesn't care how many solids you have in a single file. If you don't want to go the route of an assembly, then don't create separate NX files...plus, you won't have to use the File -> Import/Export route John pointed out.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[JohnRBaker]

But even if you do model them in separate files, once they've been 'merged' together, there is nothing preventing you from taking the individual bodies and either 'Sewing' or 'Booleaning' them together to form a single larger and more complete model.

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

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[ewh]

If you do need to maintain two separate gear files, bring both gears into one assembly file, apply assembly constraints to locate, extract (wave-link) the required bodies from both, replace the components reference sets with "empty" and unite the two extracted bodies. You can now control the relationships between the two as well as their individual configuration.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]