Part features referenced from other part features? 1

[cadman64]

I am working with an NX4 assembly and I've chosen to make a part my "work part". I would like to put tapped holes in this "work part" and locate them by referencing the counterbored holes in a mating part. Is this possible?

Thanks!

 

[JohnRBaker]

The best way to do that is create, in the part that will contain the tapped holes, WAVE linked points created at the centers of the counterbored holes in the other part. Then create your pilot holes for the thread feature by selecting these points as the origin for these holes.


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/

 

[cadman64]

Thanks John!

 

[JohnRBaker]

Note that in NX 5.0.3.2 you are able to, in the context of an assembly, create BOTH the Counterbored Holes and the ajoining Tapped Holes, in one operation and where editing the fastener specification used to define this 'Hole Series', it will cause all of the related parts to update. Note that unlike creating features 'at the assembly level', this 'Hole Series' feature will exist, each part as needed, inside the appropriate piece parts. And you not have to perform any explict WAVE linking operations to prepare for doing this operation.

In some ways, this is a sort of precursor to a more general 'model in context' capability which will be introduced in NX 6.


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/

 

[hudson888]

Thanks also for that John .

If only because I think the linked points are absolutely the way to go. I have seen some horrible methods for this simple task, so much so that I'd occasionally prefer to maintain the relationships manually than endure the alternatives.

I've loaded 5.0.3 32 Bit , whatever was on the website last week. I'll give the new methods a go. I'm a little bit concerned as to whether there are implicit or explicit wave links created that may create a new raft of maintainability issues down the track, but I like the way you're thinking on this.

Best Regards

Hudson

 

[JohnRBaker]

Note that this new NX 6 linking 'on-the-fly' will be under the control of an additional option in Customer Defaults. Currently in NX 5, you can set whether you will allow interpart modeling or not. In NX 6 you will get another 'level' of options where you can allow explicit interpart modeling, but disallow the so-called 'on-the-fly' behavior, which if it were allowed, would permit you to do things like creating an Extrude feature in your Work Part using the normal interaction inside the Extrude dialo except that you could select curves, edges, faces, sketches, etc., from anywhere in an assembly's structure, all without having to first create a series of explicit WAVE-linked objects in your work part. Yet all of these 'on-the-fly' links would be just as valid and associative as if your HAD created them ahead of time.

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/