I am new on here, and excited for our company to be a part of the NX community. I just got back from the great PLM world, and thought I would try this out.
This is a real life case of....'We could use advice' What are others doing out there for this? Here is the question and application:
[First let me state, we are newer to NX. We designed aircraft in the past in Creo. Regardless, this is NX, and we are hoping it handles mfg states,.....things much better in this regard.]
So picture a simple bracket, that has small holes in it. In the real world (mfg), this bracket is placed on a structure member, and then "match Drilled" durring final assembly on the floor, (meaning with a bigger holes), to some strut or piece of structure. That structure piece (mating piece) now also has holes in it (at that level in time). So that basically 'alters' two parts right?
We want to simulate this process in the CAD world. We want to have assembly level holes, or cuts to exist where they need to be AT THE LEVEL they need to be in the NX assembly. If you open the part it has smaller holes, if you open it in the context of its assembly, it has larger holes...etc. right?
So to recap:
Parts by themselves, when modeled, purchased etc in a bag, have small holes.
When we assemble, we match drill, to bigger holes (now modifying it) at a certain stage in the process.....
So we are looking for "Component States" and how you people out there deal with this at various levels of an assembly. We are VERY interested in ANY feedback on what peopel are doing for this. MFG states in CAD has plagued a lot of my past engineering jobs, and always had ideas that CAD, well, simply could not satisfy. So, over to you guys! Help us out? thoughts? Techniques?
Thanks again ya'all!
A couple techniques you could look at (search this forum, etc.)
- WAVE linking
- Promote body
Both of these can create an associative body at the "assembly" level, that you can modify in the assembly.
The larger hole could be modeled using a hole feature, or as a (synchronous modeling) "resize face" (or other techniques) depending on details.
I don't really understand the technical differences between the 2.
Also - be careful, as these add solids at the assembly level, they *may* be counted towards the weight of the assembly. (I think there's ways around that, but I'm not sure what they are)
Welcome to the NX world!
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled
I would look into "Promote body", and promote those that get machined at assembly. Wave will work too, but can add some un-needed steps, in this case.
In addition to the above, I'd also throw in Assembly Cut as something to check out when material removal within the context of an assembly is the goal.
Promotions, WAVE links and Assembly Cut all have their strengths and weaknesses.
NX 126.96.36.199 MP11 Rev. A
GM TcE v188.8.131.52
GM GPDL v11-A.3.7
This is great guys! thanks, yes, so....so far we are looking to maybe using reference sets to swap out a whatever level we need, do operations there, but that is prone to some issues. You would have to have all scenerios up front in the model, to be used later, like smaller holes, bigger holes. etc
Maybe (we use Team Center) we could swap a part out at mfg level with rev /02 etc? This might cause problems later as well.
I would say that promote body, was set up for this excactly, similar to "Inheretance" parts in Creo. Thanks Guys! Great feedback!
Hopefully I haven't oversimplified this or misunderstood the post. I tried a quick exercise to see if this is what you were talking about. I created two brackets (one with holes and one without holes). I assembled the two brackets together into an assembly and then created an assembly cut through both brackets. The hole diameter of the assembly cut is larger than the original holes in the first bracket. The finished assembly now has the assembly cut with larger hole diameters, but the original parts are unchanged. The first bracket has original sized holes and the second part still does not have holes. Let me know if you were wishing to accomplish something else.
Pardon the simplified graphic. I did this while I was waiting on some drawing views to update. Thanks.
Yes this is basically what we want to achieve...so did you use "Promote Body" during this? Or just do the cut here at the assembly level? If so, what is the difference with Promote Body?
I believe "Assembly Cut" creates a wave link body, in the background, ie behind the scenes, saving the user a step. (or is it a Promote?)
Use the Assembly Cut command to add a hole or another type of cutout through multiple components in an assembly.
Cut holes or other shapes in the assembly, but not in the piece parts.
"Creating an assembly cut promotes the selected bodies to the assembly level. When you create a promoted body while working in context, the display of the promoted body may hide the original body. If you want to select geometry from the component that is your work part, you may need to first change the displayed part to that component. For more information, see Promote Body in the Modeling help."
Note that the hole function has a "hole series" option that will allow you to create holes through multiple components in an assembly. For instance, if you have 3 components that you are bolting together, you can specify clearance holes for the first 2 components and a threaded hole in the 3rd body, all in the same hole feature.