Instance Geometry: boolean unite all instanced bodies?

[potrero]

Is there a way to boolean-unite all instanced bodies in an Instance Geometry feature? This way the resulting combined boolean would be parametric to a change in number of instances.

An example of such a case would be a gear with N teeth, created as an Instanced Geometry of N "wedges". Looks to me like Instance Geometry creates N independent bodies, instead of the desired single gear body.

To get a single body, one can do a boolean unite, setting the target body as the original wedge, and the tool bodies as each of the individual Instanced Geometry wedges.

If N changes to, say, N-2, then the gear seems to update fine. However, if N changes to any larger value, say N+2, then the result is 3 bodies (one body with N teeth, and then 2 extra wedges).

Any idea of a recommended solution?

 

[MSPBenson]

Could you create the wedge. Subtract it from your solid. Then group the wedge features (eg the extrude and any sketches surves etc) and the subtract feature. Now instance the group.

I think that would give you what you're after.

Mark Benson
Aerodynamic Model Designer

 

[hudson888]

potrero,

Please always state what version of NX that you're using.
Have a look at this post in NX-4 using NX-5 you can use feature instance.

I think the technique of choice was to create a group and then instance it where it may not have been possible to do so otherwise prior to NX-5.

Also have a look at this previous thread as it contains some examples that may be instructive for your needs.

http://www.eng-tips.com/viewthread.cfm?qid=216055&page=1

Best Regards

Hudson

 

[potrero]

@hudson,
Sorry, NX5. So when I was saying "Instance Geometry", I really do mean the new "Instance Geometry" function.

Is there an option that combines instanced bodies into a single body after instancing?

Thanks.

BTW, a bit of clarification on my example in the original question: I was trying to create an external gear (not an internal gear), by building it up from a 360 degree array of "pie slices". I ended up created a succesful model by starting from a "blank" disc and then cutting out pockets. Final details (ie: a round) were added to a single tooth and then copied to the rest of the teeth by using the old-style "Circular Array" command, and setting the toggle in the Round command to "apply to all instances". Not the process I originally wanted to do, but it works for now.

 

[JohnRBaker]

There is NO operation that will automatically add newly created instances to an existing Boolean unite, however there is a proposal to add such a capability to NX 7.

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.

 

[potrero]

That'd be useful.