NX6: Assembly cuts. Improvements beyond nx6?

[apekim]

Are there any users who have used the assembly cut functionality in releases beyond nx6? If so, I would like to hear about the functionality before I submit a product enhancement.

The functionality in NX6 is just okay. I would have hoped for something a little cleaner. I am thinking about submitting a product enhancement, but I am unsure if it has already been incorporated into later releases.

I would like to see assembly cuts created as a single step...similar to creating a cut on a single part. Currently, the sketch is created and finished. In the second step you select the assy cut icon.

I would like to see the assy cut icon added to an extrude dialog pulldown along with join, subtract & none.

Also, I am not a big fan of the concept of generating a "tool" from the sketch which is used to perform the cut operation. I can see if you are punching sheet metal and you use a tool library which matches the toolset in the turret (as this will also aid in auto populating your nesting program for the turret). For a machined assembly feature, I just prefer the concept of extruding a sketch through multiple parts. Why the tool concept?

Thx

 

[JohnRBaker]

I think you're missing the point.

The 'Assembly-Cut' operation doesn't care where the 'tool' body came from, whether it was extruded from a Sketch or modeled as a bunch of primitives united together, or for that matter, the 'tool' will actually be another Component altogether.

For example, one of the demos I do when someone wants to know how you would use the 'Assembly Cut' function is the case where I have an assembly where it's critical that a fastened part does not come loose during operation so we use a pre-cross-drilled nut and then at the assembly stage, after the nut has been torqued to spec, we drill a hole through the male-threaded part (using the pre-cross-drilled hole in the nut as a guide) and drive in a roll-pin. This was a very common situation when I was a machine designer, but if you wanted to create a model which represented exactly what was being built, obviously the hole in the male-threaded member can only show-up at the assembly level. So in this case, you model the Pin, add it as a component, and then use Assembly Cut, with the 'Hide Tool' setting option toggled OFF, selecting the Pin as the 'tool' body. Now I have an assembly showing exactly what I want, a pin, driven through a pre-cross-drill nut through a hole in a threaded shaft which only appears at the assembly level, but not in the detailed part that was used to manufacture the pre-assembled parts.

Granted, you can create your 'tool' body at the assembly level by extruding a sketch, if you wish, but you could have just as easily created it as a totally separate part and merged it in as a component and worked from there.

I'm sorry, but I'll opt for the simplicity and flexibility of the current approach, and which, to answer your original question, is working in NX 7.5 exactly as it was in NX 6.0, and as far as I can tell, there are no plans to make any changes in NX 8.0.

Now if you wish to offer some suggestions for improvements, be our guest, but let's not forget that it's hard to make something simpler to use by adding to it.

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

 

[apekim]

John, Thanks for the reply on this. Although our backgrounds are very similar (mine: machine shop/sheet metal shop), I will have to disagree with you on this.

Here is why:
CAD tools (take your pick) typically offer several different approaches to obtain the same result. Where it can get hairy is when the process to obtain the result deviates from typical operations performed in an actual shop environment. I am not insinuating that the CAD tool disallow such a process.

In the example you had offered with the pre drilled nut, the drilling operation indeed occurs at the assembly level. As far as deciding on the appropriate method to perform the cut into the male component, I would tend to perform the assembly cut by referencing the hole in the nut...since the nut is actually what would be used in a machine shop as the drill guide. Using the split pin part as a cutter tool can lead to all sorts of confusion down the road.

I prefer the KISS concept, especially when it can be based on real world fabrication processes.

Adding the assy cut icon to the pull down would result in eliminating the need for separate steps, unless you desire to differ from a real world machine shop process. It would also promote consistency in the functionality for cuts...whereas it could be the same process for part and assembly cuts. The only difference being the assembly selected as the work part.

 

[uwam2ie]

..kiss
I think you want enhancement on the booleans.
Since nx6 you can add tool body direct from assembly level.
I-deas user can do on target selection collect from entire assembly,too.@apekim: the pocket in the Moldwizard and PDwizards have this opportunity.

 

[JohnRBaker]

BTW, there is nothing stopping you from using WAVE to do virtually that same thing. In many respects, an 'Assembly Cut' operation is nothing more than a neatly packaged feature which captures a series of WAVE linking operations with a Boolean subtract thrown it at the end.

And as I said, if you think you've got some good ideas on how to improve this or any other aspect of NX, please feel free to contact GTAC and have them open an ER.

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