Some of you might be aware that Solid Edge has one option where we can convert 'Design Body' to a 'Construction' body & vice versa. These construction bodies don't take part in assemblies & drawings. They are just used to create more features or do operations that require the use of another body.
We have multi bodies in NX as well. We can perform boolean operations with those.
Now that was just a brief idea of this multi body & contruction thing.
In NX, I require some solid bodies to not show up in the drawings & assemblies, & also to use them for assisting me to create other operations (those operations might be associative to the original body so suppressing it won't work).
And yeah, Merry Christmas in advance. & Wishing you all a very happy & prosperous year ahead!
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That's close enough, but that works only in Assembly Application if I'm not mistake.
Isn't there any feature where we just mark some bodies as construction bodies so that later on they don't participate anywhere (not just specifically drafting or assembly but in any application).
Becomes bothersome in some cases, when we have a large assembly to create reference sets at the assembly level.
Thanks for the reply though.
I don't think NX has a specific command as such, as Steve states you also have Reference Sets.
So NX gives you a multitude of options as to how to control visability at specific levels, and along with Wave Linking and Assembly Arrangements you have to come up with a method that suits your intent.
Thanks for clearing things up.
I just felt a feature as small as this can come in handly sometimes (throughout the course of product design).
Any chance for this feature to come up in any future relase of NX? I might be asking for too much.
I would say any company should have a minimum list of standard reference sets.
By default (in Customer Defaults - Assemblies - Site Standards - Reference Sets) a reference set MODEL exists and solid and sheet bodies places in this automatically.
What I would recommend is creating at least a second reference set called CONSTRUCTION BODIES. Then remove all but bodies representing the real component from MODEL reference set and add them to the CONSTRUCTION reference set.
This can be done with the Reference Set command in Assemblies tab.
Was is also useful is to swap the PNT to non-timestamp mode, here all the bodies in the part are listing under the reference set they belong too. Here you can drag and drop bodies between existing reference sets and set bodies in reference set to hide/show.
Another organisation to look at is Product Interfaces. First I recommend giving the bodies (not the features) names. Then in the Product Interface command select the bodies that you want to use in other part files.
In Customer Defaults - Assemblies - General - Product Interface you can set how objects are selectable in WAVE inter-part commands.
Thanks alot @StevenVickers! Those can be very good alternatives while working with multi-body parts.
I, for one, love the WAVE functionality but it introduces a few extra layers in the entire procedure.
I am always on the lookout fo the most efficient method, & that's what helps all of us to increase the productivity ultimately.